? Acceleration with jerk limitationTo achieve an optimum acceleration pattern with reduced wear on the machine's mechanical parts, you can select SOFT in the part program to ensure a continuous, jerk-free acceleration profile. When you select "jerk-free acceleration", the velocity characteristic over the path is generated as a sinusoidal-shaped curve. Access protection
Access to programs, data and functions is protected in a user-oriented hierarchical system of 8 access levels. These are subdivided into:
SINUMERIK controls thus provide a multi-level concept for controlling access rights. Protection level 0 has the highest, protection level 7 the lowest access rights. A higher protection level automatically includes all protection levels below it. Access rights for protection levels 0 to 3 are preprogrammed by Siemens as standard. An entered password takes precedence over a keyswitch position, and machine manufacturers or end users can change access rights for protection levels 4 through 7. Subprograms can only be protected in their entirety against unauthorized reading and displaying. Action logThe "action log" records all operator actions and pending alarms for diagnostics purposes. Actual-value system for workpieceThe term "actual-value system for workpiece" is used to designate functions which allow the SINUMERIK user to:
Advanced Position Control (option)The natural frequency of the machine can have a detrimental effect on the maximum speed of the machine and the surface characteristics of the workpieces. The APC option that is available from software version 6 (HMI and NCK) raises the KV factor (position control loop gain), improves the surface and therefore increases the productivity. APC requires implementation of High-Performance closed-loop controls. Advanced Processing 1 and 2 (option)The function "Advanced Processing 1" permits reduction of the interpolation cycle down to 4 ms with the SINUMERIK 840Di/ 840DiE system software Universal and Plus. The function "Advanced Processing 2" only applies to the SINUMERIK 840Di/840DiE software Plus, and permits reduction of the interpolation cycle down to 2 ms. Alarms and messages
Programming and displaying message texts
Example 1:
Example 2:
You will find a list of responses to the various alarms in the Startup Guide. The alarm text must be configured. Alarm numbers 65000 to 67999 are reserved for the user.
Example 3:
Analog axis (option)This function is intended for individual motors on machines which cannot be controlled with digital drives, such as large spindle motors or motors for tool changers. An analog axis can be used very much like a digital axis. It can be programmed like a digital interpolating path axis or spindle. Pure functions of the SIMODRIVE 611 drive control system are, of course, not possible for external drive units linked via an analog speed setpoint interface. This involves functionalities which fall back on internal axis feedback and communication via the drive bus, such as torque feedforward control, filters for damping mechanical resonance, "Safety Integrated", and so on. Separate EMC measures must be taken for external drive units where applicable. Analog axes can be implemented in two different ways:
A technology PC card is no longer required starting with this software release, since the functionality is already included in the NCU system software. Analog value controlWith the system variable $A_OUTA(n), values from up to eight possible analog outputs can be preset directly in the part program. A submodule "DMP Compact 1 A analog" for analog outputs is required in the connected NCU terminal block (on the SINUMERIK 840Di PROFIBUS DP and S7-300 output modules). Prior to being output to the hardware, the value preset by the NCK can be modified by the PLC in DB10. The hardware outputs are written in the interpolation cycle. Asynchronous subprograms> Interrupt routines with fast retraction from the contour An asynchronous subprogram is a CNC program which can be started based on an external event (e.g. a digital input) or from the PLC. Inputs are allocated to subprograms and activated by programming SETINT. If the relevant event occurs, the CNC block currently being processed is immediately interrupted. The CNC program can be continued later at the point of interruption. Multiple asynchronous subprograms must be assigned different priorities (PRIO) so that they can be processed in a certain order. Asynchronous subprograms can be disabled and enabled again in the CNC program (DISABLE/ENABLE). Auxiliary function outputWith "auxiliary function output", the PLC is informed when the part program wants the PLC to carry out certain machine operations. This is accomplished by transferring the appropriate auxiliary functions and their parameters to the PLC interface. The transferred values and signals must be processed by the PLC user program. The following functions can be transferred to the PLC:
The "Auxiliary function output" may be carried out either with reduction in velocity and PLC acknowledgment up to the next block or before and during the movement without reduction in velocity and without block change delay. Following blocks are then retracted without a time-out. Axes, coupled motionWhen a defined master axis moves, the coupled-motion axes (following axes) assigned to it travel the traverse paths derived from the master axis, taking into account a coupling factor (setpoint coupling). Together, the master axis and the following axes form a coupled-axis grouping. Definition and activation of a coupled-axis grouping take place simultaneously with the modal-like instruction TRAILON. A coupled-axis grouping can consist of any desired combinations of linear and rotary axes. A coupled-motion axis can be assigned up to 2 master axes (in different coupled-axis groupings). A simulated axis can also be defined as the master axis, in which case the real axis actually does the traveling, taking into account the coupling factor. Another application for coupled axes is the use of 2 coupled-axis groupings to machine the two sides of a workpiece. Axes/spindles or positioning axes/auxiliary spindles> Spindle functions Axes In accordance with their functions, the axes are subdivided into:
Positioning axes: Non-interpolating feed and positioning axes with axis-specific feed; axis movements beyond block boundaries are possible.
Spindles Spindle drives can be speed-controlled or position-controlled. Auxiliary spindles Auxiliary spindles are speed-controlled spindle drives without actual-position encoders, e.g., for power tools. Axial coupling in the machine coordinate system (option)
This option is required in order to be able to use coupled axes implemented in the basic coordinate system for transformations as well. A coupling is carried out 1:1 in the machine coordinate system. The participating axes can be reconfigured following Reset. On machine tools with separately movable heads on which a transformation must be activated, the orientation axes cannot be coupled using the standard coupling methods (COUPON, TRAILON). The axes participating in the coupling are determined via axial machine data that is updated with RESET. This makes it possible to redefine pairs of axes during operation and enable and disable them via CNC language commands. There are master and slave axes. A master axis can have more than one slave axis, but a slave axis cannot be a master axis at the same time (no cascading). To protect the heads from collisions, collision protection can be set and activated via either machine data or VDI interface. Axial data output via PROFIBUS (ADAS) (option)This function sends up to 28 data packets from the SINUMERIK NC kernel to the PROFIBUS DP of the integrated PLC hardware module. The communication cycle time can be configured in multiples of the position controller sampling time. Each data packet contains a 4-byte-long integer element with axial data. The signal types and associated machine axis can be defined freely during runtime. Axis container (option)> Link axis 
Example of axis container: following rotation of the axis container by 1, the channel axis Z is assigned to axis AX5 on NCU 1 instead of axis AX1. On rotary indexing machines/multi-spindle machines, the work-holding axes move from one machining unit to the next. Since the machining units are subject to different NCU channels, the axes holding the workpiece must be dynamically reassigned to the corresponding NCU channel if there is a change in station/ position. Axis containers are used for this purpose. Only one workpiece clamping axis/spindle is active on the local machining unit at a time. The axis container combines the possible connections to all clamping axes/spindles, of which only one is active at a time for the machining unit. The following can be assigned via the axis container:
The available axes that are defined in the axis container can be changed by switching the entries in the axis container. Shifting can be triggered by the part program. Axis limitation from the PLC> Protection zones The preactivation of protection areas with specification of a position offset is programmed in the part program. You can put the preactivated protection zones into effect in the PLC user program via the PLC interface. As a result, the relevant protection area is activated, for example, before a tool probe is swiveled into position in the work area to see whether the tool or a workpiece is in the path of the swiveling probe. The PLC can put another axis limitation into effect by activating the 2nd software limit switch via a PLC interface signal. This reduction of the working area may become necessary, for example, when a tailstock is swiveled into position. The change is immediately effective, and the 1st software limit switch plus/minus is no longer valid. Axis/spindle replacementAn axis/a spindle is permanently assigned to a specific channel via machine data. With the "axis/spindle exchange" function, it is possible to release an axis/a spindle (program command RELEASE) and to assign it to another channel (command GET), i.e. to exchange the axis/spindle. The relevant axes/spindles are determined via machine data. Backlash compensation
Positive backlash (normal case) During power transmission between a moving machine part and its drive (e.g., ball screw), there is normally a small amount of backlash because setting mechanical parts so that they are completely free of backlash would result in too much wear and tear on the machine. In the case of axes/spindles with indirect measuring systems, mechanical backlash results in corruption of the traverse path. For example, when the direction of movement is reversed, an axis will travel too much or too little by the amount of the backlash. To compensate for backlash, the axis-specific actual value is corrected by the amount of the backlash every time the axis/spindle reverses its direction of movement. If a 2nd measuring system is available, the relevant backlash on reversal must be entered for each of the two measuring systems. Backlash compensation is always active in all modes following reference point approach. Basic offsets in the workpiece coordinate system> Work offsets With HMI-Advanced, you can define up to 16 channel-specific and 16 global basic frames which are then effective for all part programs. Block searchFor testing part programs or following interruption of machining, it is possible to select any point in the part program using the "block search" function in order to start or resume at this point. You have a choice of 4 different search options:
You can specify the search destination by:
Cartesian PTP travelFor handling and robot-related tasks, two types of movement are required, either in the Cartesian coordinate system (continuous path, CP), or as a point-to-point (PTP) movement. With PTP, the shortest way to reach the end point is with activated (!) TRAORI transformation. PTP generates a linear interpolation in the axis space of the machine axis. By smoothing from PTP to CP movement, it is possible to switch from fast infeed to a mounting or positioning movement with optimum timing. PTP travel does not result in an axis overload when traveling through a singularity (such as the changing of an arm position during handling). PTP travel is also possible in JOG mode and does not require Cartesian positions (e.g., from CAD systems) to be converted into machine axis values. Cartesian PTP travel is also used for cylindrical grinding machines with an inclined axis: With active transformation, the infeed axis can be moved either according to Cartesian coordinates or at the angle of the inclined axis. Circle via center point and end pointCircular interpolation causes the tool to move along a circular path in a clockwise or counter-clockwise direction. The required circle is described by:
The circle center can be programmed as an absolute value with reference to the current zero point or as an incremental value with reference to the starting point of the circular path. If the opening angle is apparent from the drawing, then it can be directly programmed. In many cases, the dimensioning of a drawing is chosen so that it is more convenient to program the radius in order to define the circular path. In the case of a circular arc of more than 180 degrees, the radius specification is given a negative sign. Circle via intermediate point and end pointIf a circle which does not lie in a paraxial plane but obliquely in space is to be programmed, an intermediate point can be used to program it instead of the circle center. Three points are required to program the circle: the starting point, intermediate point and end point. Clamping monitoring> Position monitoring, standstill monitoring "Clamping monitoring" is one of SINUMERIK's many extensive monitoring mechanisms for axes. When an axis is to be clamped following conclusion of the positioning procedure, you can activate the clamping monitor with the PLC interface signal "clamping in progress". This may become necessary because it is possible for the axis to be pushed beyond the standstill tolerance from the position setpoint during the clamping procedure. The amount of deviation from the position setpoint is set via the machine data. During the clamping procedure, clamping monitoring replaces standstill monitoring, and is effective for linear axes, rotary axes, and position-controlled spindles. Clamping monitoring is not active in follow-up mode. When the monitor responds, its reactions are the same as those of the standstill monitor. Clearance control
Components for setting up laser machining with SINUMERIK 840D powerline Clearance control makes it possible for sensor signals, for instance, to be evaluated via the NCK I/O's high-speed analog input (A/D conversion: 75 µs). The "clearance control 1D in the IPO cycle" is used to compute a position offset $AA_OFF for an axis via synchronous action. The "clearance control 1D/3D in the (LR) position control cycle" (which includes the IPO cycle) controls three machine axes as well as a gantry axis and makes it possible to automatically maintain the constant clearance that is technologically required for the machining process. The most important applications for this are water jet cutting and laser cutting, for example, the radial cutting of rods with non-circular cross sections. "Limited functionality with SINUMERIK 840DE powerline: only clearance control 1D in the LR cycle and restricted to maximum of 4 interpolating axes." CNC program messages> Alarms and messages All messages programmed in the part program and all alarms recognized by the system are displayed on the operator panel in plain text. Alarms and messages are displayed separately. You can program messages in order to provide the operator with the latest information on the current machining situation during the program run. CNC user memoryAll programs and data, such as part programs, subprograms, comments, tool offsets, and work offsets/frames, as well as channel and program user data, can be stored in the shared CNC user memory. The CNC user memory is battery-backed. Concatenated transformations
Grinding a TRANSMIT contour with inclined axis With the TRACON command, two transformations can be concatenated: TRAANG (inclined axis), as the base transformation, can be linked with TRAORI (5-axis transformation), TRANSMIT (front end machining of turned parts) or TRACYL (cylinder surface transformation). Applications:
Connection for SIMATIC HMI via PLCAll PLC variables (inputs, outputs, memory bits, data values, timers, counters, and so on) can be displayed on the SIMATIC HMI operator panel. It is currently only possible to access the CNC variables from the OP7/17. Further versions will be available soon. Continue machining at the contour (retrace support) (option)When using 2D flat bed cutting procedures, e.g., laser, oxygen or water jet cutting, the machine operator can return to the program continuation point (damage point) following an interruption in machining without exact knowledge of the part program in order to continue machining the workpiece from there. The functionality "Retrace support" contains a ring buffer for the geometric information of the executed blocks. A new part program is generated from this for the reverse travel. Retracing is used, for example, when the machine operator only notices the failure or interruption a few blocks after the actual interruption. The head has usually already progressed further in the machining, and must, therefore, be appropriately returned for continuation of machining. Continuous dressing (parallel dressing)
Parallel dressing With this function, the form of the grinding wheel can be dressed in parallel with the machining process. The grinding wheel compensation resulting from dressing the wheel takes immediate effect as tool length compensation. When the tool radius compensation is programmed to machine the contour and the tool radius changes because of the dressing of the grinding wheel, the CNC computes the dressing amount online as a true tool radius compensation. Limited functionality on the SINUMERIK 810DE powerline/840DiE/840DE powerline: Only one measured variable (e.g. actual axis value, analog input) can be evaluated and subsequently only one correction made (e.g. axis correction during dressing of the grinding wheel); (functionality is not limited from NCU SW version 6.5 upwards). Continuous-path mode with programmable rounding clearance
Continuous-path mode with programmable rounding clearance The aim of the continuous-path mode is to avoid excessive deceleration at the block boundaries and to achieve as constant a tool path velocity as possible during tangential transitions from one block to the next. Because the tool does not stop at block boundaries, no undercuts are made on the workpiece. If continuous-path mode (G64) is selected, reduction in velocity takes place and contour corners are rounded on non-tangential transitions. A soft contour transition without a jump in acceleration can be programmed with G641 ADIS=... Contour definition programmingContour definition programming allows you to input simple contours quickly. With the aid of help displays in the editor, you can program 1-point, 2-point or 3-point definitions with transition elements chamfer or corner easily and clearly by entering Cartesian coordinates and/or angles. Contour handwheel (option)> Feedrate interpolation When the "contour handwheel" function is activated, the handwheel has a velocity-generating effect in AUTOMATIC and MDA modes on all programmed traversing movements of the path and synchronous axes. A feedrate specified via the CNC program becomes ineffective and a programmed velocity profile is no longer valid. The feedrate, in mm/min, results from the handwheel pulses as based on pulse weighting (machine data) and the active increment. The handwheel's direction of rotation determines the direction of travel:
Contour monitoring> Travel to fixed stop The following error is monitored within a definable tolerance band as a measure of contour accuracy. An impermissibly high following error might be caused by a drive overload, for example. If an error occurs, the axes/spindles are stopped. "Contour monitoring" is always enabled when a channel is active and in position-controlled mode. If the channel is interrupted or in the reset state, contour monitoring is not active. Contour monitoring is also deactivated during execution of the "travel to fixed stop" function. Contour monitoring with tunnel function (option)With the function "contour monitoring with tunnel function", the absolute movement of the tool tip in space can be monitored in 5-axis machining or when complex workpieces are being machined. This function provides optimum protection for high-quality workpieces. A cylindrical tunnel (tolerance field) with a definable diameter is placed around the programmed path. If during machining the deviation from the path caused by axis errors is greater than the defined tunnel diameter, the axes are brought to a standstill immediately. The deviation from the path can be written simultaneously to an analog output. Control unit management (option)
M:N link with SINUMERIK 840D powerline In SINUMERIK control systems, the M:N link can be used to allocate several control units (M) to multiple CNC controls (N) via a shared bus (BTSS/ MPI). In the basic configuration, up to 8 NCUs can be controlled by one PCU. The "control unit management" option makes it possible to operate up to 9 NCUs on up to 9 PCUs via active, passive and displacement mechanisms. Cross-mode actions (option)> Interrupt routines with fast retraction from the contour Asynchronous subprograms (ASUB) make it possible to respond immediately to high-priority events not only during program execution, but in all modes and program states. In the case of such an interrupt, it is also possible to start an asynchronous subprogram in manual modes. The asynchronous subprogram can be used, for example, to bring the grinding wheel to a safe position to avoid collision. This option also enables statically effective IDS synchronous actions, which are active in all modes. Cycle storage separate from CNC user memory (option)Files which have not been modified online (e.g. Siemens and machine manufacturer cycles) can be relocated using this function from the SRAM into a DRAM file system for cycle storage. More memory space is then available in the SRAM for part programs. The function can only be used in combination with HMI-Advanced. Cycle support> Expand user interface The technology cycles for drilling, milling and turning and the measuring cycles are supported by cycle screens. Similar input displays are also available for geometric contour programming. You can, however, also define a number of softkeys, input fields and displays yourself using the functionality of "expand operator interface". Data backupSoftware is delivered on floppy disk, CD-ROM, or installed on the hardware. Floppy disks or CD-ROMs (for large data quantities, e.g. PCU 50 with hard disk) are used as the medium for data backup. The following data backup methods are available. Data management software: ADDM – Automation and Drives Data Management for PG or PC, including server link.
Data exchange between machining channels> High-level CNC language In the "program coordination" function, variables shared by the channels (NCK-specific global variables) can be used for data exchange between the programs. The program message itself is separate for each channel. Diagnostics functionsFor service purposes, a self-diagnostics program and testing aids have been integrated in the controls. The status of the following can be displayed on the operator panel:
For testing purposes, signal combinations can be set for the output signals, input signals, and bit memories. All alarms and messages are displayed in plain text on the operator panel along with the corresponding acknowledgement criterion. Alarms and messages are displayed separately. In the "service display" menu, it is possible to call up important information about the axis and spindle drives, such as:
Differential resolver function (DRF)> Handwheel override The "differential resolver function" generates an additional incremental work offset in AUTOMATIC mode via the electronic hand-wheel. This function can be used, for example, to correct tool wear within a programmed block. Dimensions metric/inchesDepending on the measuring system used in the production drawing, you can program workpiece-related geometrical data in either metric measure (G71) or inches (G70). The control can be set to a basic system regardless of the programmed dimensional notation. You can enter the following geometrical data directly and let the control convert them into the other measuring system (examples):
With the G700/G710 programming expansion, all feedrates are also interpreted in the programmed measuring system (inch/min or mm/min). In the "machine" control area, you can also switch back and forth between inch and metric notation using a softkey. Display functionsAll current information can be displayed on the operator panel's screen, such as:
Important operating states are displayed in plain text, for example
Dynamic Swivel Tripod (DST) transformation (option)The DST kinematic transformation is a 5- or 6-axis transformation with serial-parallel kinematics. This package thus allows an axially symmetrical tool (milling cutter, laser beam) to be oriented to the workpiece in the machining space. The restriction to dynamically balanced tools no longer applies with six axes. The path and path velocity are programmed in the same way as for 3-axis tools. The tool orientation is programmed additionally in the traversing blocks. The real-time transformation performs the calculation of the resulting motion of all 5 or 6 axes. The generated machining programs are therefore not machine specific. Kinematic-specific post-processors are not used for the 5- or 6-axis machining operation. The calculation also includes tool length compensation. Dynamic preprocessing memory (FIFO)The traversing blocks are readied prior to execution and stored in a preprocessing memory (FIFO = first in/first out) of specifiable size. In contour sections that are machined at high velocity with short path lengths, blocks can be executed from this preprocessing memory at very high speed. The preprocessing memory is constantly reloaded during execution. Block execution can be interrupted with the STARTFIFO command until the preprocessing memory been filled, or STOPFIFO (start high-speed machining section) or STOPRE (stop preprocessor) can be programmed. Electronic gear (option)The "electronic gear" function allows highly accurate kinematic coupling of axes with programmable gear ratio. Linking can be specified and selected for any CNC axes via program or operator panel. The "electronic gear" function makes it possible to control the movement of a following axis, depending on up to five master axes. The relations between the master axis and the following axis are defined for each master axis by a fixed gear ratio (numerator/denominator) or as a linear or non-linear coupling using a curve table. The following axis can be a master axis for another gear system (cascading). Real as well as simulated linear and rotary axes can be used as the master and following axes. Master input values can be setpoints generated by the interpolator (setpoint linkage) or actual values delivered by the measuring system (actual-value linkage). The electronic gears with non-linear linking available starting with software release 6 of the SINUMERIK 840D powerline also permit e.g. compensation of non-linear properties of the process in addition to the manufacture of convex teeth when machining gear wheels. Functionality limitations on the SINUMERIK 840DE powerline/840DiE: The number of simultaneously traversing axes is restricted to four. Electronic handwheels (accessories)Using electronic handwheels, it is possible to move selected axes simultaneously in manual mode. The handwheel clicks are analyzed by the increment analyzer. If coordinate offset or coordinate rotation is selected, it is also possible to move the axes manually in the transformed workpiece coordinate system. The maximum input frequency of the handwheel inputs is 100 kHz. A third handwheel can also be operated over the actual-value input of the SIMODRIVE 611 digital's control modules or the CCU unit. The "Contour handwheel" option permits use of a handwheel on conventional turning machines (applications for ManualTurn and ShopTurn) and also during grinding for traversing on a contour. Once "contour handwheel" has been activated, the handwheel has a velocity-generating effect in AUTOMATIC and MDA mode, that is, a feedrate specified via the CNC program is no longer effective, and a programmed velocity profile is no longer valid. The feedrate, in mm/min, results from the handwheel pulses as based on pulse evaluation (via machine data) and the active increment (INC1, INC10, etc.). The handwheel's direction of rotation determines the direction of travel: clockwise in the programmed direction, even over block boundaries, and counter-clockwise up to the block start. Electronic transfer (option)> position switching signals/cam controller, > polynomial interpolation, > master value coupling and curve table interpolation, > cross-mode actions, > I/O interfacing via PROFIBUS DP, > synchronized actions stage 2, > pair of synchronized axes (gantry axes) In presses with transfer step tools as well as in large-part transfer presses, a modern transfer system handles part transport. Positioning drives are controlled in step with the press's main motions. The "electronic transfer" option makes it possible to control sequences of motion in transfer systems (such as gripper or suction lines, etc.), depending on a master value, which corresponds to the current ram position of the press. The "electronic transfer" option includes the options
Combinations of these individual options satisfy all requirements for highly dynamic and accurate transfer controls. When using the "electronic transfer" option, the "spindle" and "tool offset" functions cannot be activated. Limited functionality of export control versions: The number of simultaneously traversing axes is restricted to four. Electronic weight counterbalance (option)
Electronic weight counterbalance With weight-loaded axes without mechanical or hydraulic weight counterbalance, the vertical axis drops when the brake is released and the servo enable is switched on. The undesired lowering (dZ) of the axis can be compensated by activating electronic weight counterbalance. After releasing the brake, the constant weight counterbalance torque maintains the position of the vertical axis. Sequence: 1. Brake holds Z axis. Evaluation of internal drive variables (option)With the "evaluation of internal drive variables" function, a second process variable (such as a path-specific or axis-specific feedrate) can be controlled (adaptive control) in dependence on a measured process variable (such as spindle current). This permits, for example, the cutting volume to be kept constant when grinding, or faster covering of the grinding gap when scratching ("first touch"). Evaluation of these drive variables also permits machines and tools to be protected from overloading, as well as shorter machining times and an improved surface quality for the workpieces to be achieved. The "Evaluation of internal drive variables" is the prerequisite for implementation of adaptive control. Adaptive control can be parameterized within the part program as follows:
The following real-time variables can be evaluated as internal drive variables: $AA_LOAD drive capacity utilization in % $AA_POWER drive active power in W $AA_TORQUE driving torque setpoint in Nm (actual power value in N only with SIMODRIVE 611 digital/with hydraulic linear drives HLA) $AA_CURR actual axis/spindle current in A Restricted functionality of the "evaluation of internal drive variables" with SINUMERIK 810DE powerline/840DE powerline: Only one measured variable can be evaluated at a time (e.g. spindle current); no functionality restriction from NCU SW version 6.5 on. Execution from hard diskExtremely long part programs or programs which no longer fit in the CNC program memory, can be saved on the hard disk and also executed from there. This can also be carried out in several channels. You can use the "EXTCALL" command to also call programs from the hard disk for cascading. This "Execution from hard disk" has an effect beyond a reset or the end of a part program, and is only terminated by selection of a program which is located in the CNC program memory. To process the subprograms from hard disk, a FIFO buffer (first in/first out) whose size can be adjusted using machine data is organized on the CNC. Note concerning all above-mentioned forms of this external execution: If a part program is executed more rapidly than further data can be provided externally (e.g. via V.24 interface), the CNC waits for further data without sending an alarm. Execution from network drive or PC card> PC card as additional program memory Execution of extremely long part programs is possible via a network server. PCU 20, PCU 50 and PCU 70 already have the Ethernet connection onboard. With the PCU 20, you require the option "Administration of network/disk drives for PCU 20", and with the PCU 50.3 the optional SINUMERIK software MCIS DNC Machine. The PC card plug-in unit of the PCU 20 can also be used as an additional program memory together with a PC card. Execution via the V.24 interfacePart programs that are too large for the CNC program memory can be processed using HMI-Embedded via the V.24 interface in punched-tape format and simultaneously executed. Extended stop and retract (incl. generator operation) (option)A safe position is assumed from the machining level without any collision between tool and workpiece. As an extension to the independent drive stop/retract function possible from software version 5, software version 6 or higher now offers the functionality "CNC-controlled stop/retract". To permit gentle interpolated retraction on the path or contour, the path interpolation can be processed further for a definable period following the triggering event. The retraction axes are subsequently driven in synchronism to an absolute or incremental position as programmed. These functions are primarily used for gearing and grinding technologies. Fast-IPO-Link (option)Non-circular machining can be carried out for general workpiece contours using polynomial interpolation or, with sinusoidal default settings, using master value coupling and curve table interpolation. In the case of very fast non-circular machining, "Fast-IPO-Link" permits transfer of the non-circular task (e.g. movement of X-axis) to a separate NCU with fast cycle. Speeds greater than 3000 rpm (for sinusoidal movements) can then be achieved. Feedforward controlUsing the function "feedforward control", you can reduce axial following errors almost to zero. This feedforward control is therefore also called "following error compensation". Particularly during acceleration in contour curvatures, e.g. circles and corners, this following error leads to undesirable, velocity-dependent contour violations.
Feedrate interpolation (feed characteristic)> Polynomial interpolation 
Programming example for feedrate interpolation N1 Constant feedrate profile F1000: FNORM N2 Abrupt set velocity change F2000: FNORM N3 Feedrate profile via polynomial : F = FPO (4000, 6000, -4000) N4 Polynomial feedrate 4000 as modal value N5 Linear feedrate profile F3000: FLIN N6 Linear feedrate 2000 as modal value N7 Linear feedrate, as modal value N8 Constant feedrate profile with abrupt acceleration change F1000: FNORM N9 All subsequent F values are linked by splines F1400: FCUB N13 Switch off spline profile N14 FNORM In accordance with DIN 66025, a constant feedrate over the part program block can be defined via address F. For a more flexible definition of the feedrate profile, programming to DIN 66025 is extended by linear and cubic profiles over the path. The cubic profiles can be programmed directly or as an interpolating spline. This makes it possible, depending on the curvature of the workpiece to be machined, to program continually smooth velocity profiles, which in turn allow jerk-free acceleration changes and thus the production of uniform workpiece surfaces. You can program the following feedrate profiles:
Feedrate overrideThe programmed velocity is overridden by the current velocity setting via the machine control panel or by the PLC (0 % to 200 %). In order for the cutting velocity on the contour to be kept constant, the feedrate calculation is referred to the operating point or tool end point. The feedrate can also be corrected by a programmable percentage factor (1 % to 200 %) in the machining program. This factor is overlaid (multiplication) on the setting made on the machine control panel. The velocity setting from the PLC is axis-specific. Follow-up modeIf an axis/spindle is in follow-up mode, it can be moved externally, and the actual value can still be recorded. The traverse paths are updated in the display. Standstill, clamping and positioning monitoring functions are not effective in follow-up mode. Following cancellation of follow-up mode, it is not necessary to carry out a reference point approach again. Frame conceptFrame is the common term for a geometric expression describing an arithmetic operation, e.g. translation or rotation. On SINUMERIK controls, the frame in the CNC program transfers from one Cartesian coordinate system to another, and represents the spatial description of the workpiece coordinate system. The following are possible:
The frame concept makes it possible to transform Cartesian coordinate systems very simply by offsetting, rotating, scaling and mirroring. The following instructions are used to program these options:
The instructions can also be used several times within one program. Existing offsets can either be overwritten or new ones can be added. Additive frame instructions: ATRANS additive programmable work offset AROT additive rotation in space or in a plane ASCALE scale factor (multiplication) AMIRROR repeated mirroring AROTS additive rotation referred to the solid angle projected into the planes If swivel-mounted tools or workpieces are available, machining can be implemented very flexibly, for example:
From software version 5 and higher, NCK-global frames are also available for all channels of an NCU. Generator operation (option)With the "Generator operation" function, brief power outages can be bridged or power provided for retraction. To make this possible, the energy stored during spindle rotation or axis movement is fed back into the DC link, following the same principle as that used by generators. Generic coupling Basic: CP Basic (option)This option offers:
Generic coupling Comfort: CP Comfort (option)This option offers:
Also:
Generic coupling Expert: CP Expert (option)This option offers:
Also:
Generic coupling Standard: CP StandardThe basic version already offers:
Generic couplings (basic version/options)For generic (general) coupling (CP) of axes/spindles, we offer 4 different performance levels. The functionality is scalable via the number of master axes to one slave axis, via coupling characteristics ranging from simple functionality through to technological innovations and via the simultaneously activatable coupling types. The options CP Basic, CP Comfort and CP Expert are available. These options can be combined as required. Functionality limitations on the SINUMERIK 840DE powerline/840DiE: see the functional limitations for each of the above-mentioned functions and options. Generic transformationThe function "Generic transformation" is used to define any tool orientation in the space with the initial setting of the axes, and not just according to the Z-direction. It can then be used much more flexibly and universally. It is then possible, for example, to also control machine kinematics from the CNC, where the orientation of the rotary axes is not exactly parallel to the linear axes. Starting with software release 6, extension of the generic 5-axis transformation to the 3-axis and/or 4-axis transformation is also possible for machines with only one rotary axis (rotatable tool or workpiece). Geometry axes, switchable online in the CNC program
Geometry axes, switchable online In the CNC, geometry axes form axis groupings per channel for the interpolation of path motions in space. Channel axes are assigned to geometry axes via machine data. With the "switchable geometry axes" function, it is possible, from the part program, to assemble the geometry axis grouping from other channel axes. This makes problem-free operation of machine kinematics with parallel axes possible. Grinding wheel surface speed, constantAutomatic conversion of the grinding wheel surface speed to a speed of rotation as a function of the current grinding wheel diameter. This function can be active for several grinding wheels simultaneously in one CNC channel. The grinding wheel surface speed is monitored. A constant grinding wheel surface speed is not only useful during processing of a part program in the AUTO and MDA modes, but can also be effective immediately after power-up of the controller, on reset, and at the end of the part program, and remain in force beyond all mode changes (depending on the machine data). Handwheel override
Handwheel override in AUTOMATIC mode With the function "Handwheel override", an axis can be traversed or the velocity of an axis can be overridden. The function is effective blockwise. At the same time, additional axes can be traversed simultaneously or using interpolation. The actual-value display is continuously updated. Application: grinding machines. Helical interpolation
Helical interpolation: Thread milling with form cutter "Helical interpolation" is especially suitable for machining inside or outside threads with profiling cutters and for milling lubrication grooves. The helix comprises two movements:
The programmed feedrate F either refers only to the circular movement or to the total path velocity of the three CNC axes involved. In addition to the two CNC axes performing circular interpolation, other linear motions can be performed synchronously. The programmed feedrate F refers to the axes specially selected in the program. Interpolation with more than 4 axes requires export approval. HEXAPOD, PARACOP, TRICEPT transformations and pantograph kinematics (options)
HEXAPOD animation 
PARACOP animation 
TRICEPT animation HEXAPOD, PARACOP, TRICEPT kinematic transformations and pantograph kinematics are used on parallel-kinematics machines (PKM). Parallel kinematics means that the drive forces engage on the spindle head (Stuart platform) simultaneously (virtually in parallel). With HEXAPOD, the Stuart platform is moved by six actuators, whose lengths can be modified. The Stuart platform can be moved to any position, including within the working area, by these six actuators, and its inclination in space (orientation) can also be set specifically. This allows workpieces to be machined on 5 axes on these machines. The orientation angle is only limited by the mechanical properties of the cardan or ball joints. PARACOP and TRICEPT machines are TRIPODEN types, whereby the Stuart platform is moved by three actuators. Design measures are used to ensure that the Stuart platform cannot move in an undefined manner on these TRIPODEN types. On PARACOP machines, two parallel rods run on a slide for each actuator. These machines are suitable for 3-axis machining. On TRICEPT, an additional passive telescope (center tube) is used. On TRICEPT, two additional rotary axes are required to define the tool orientation in space. These axes can be arranged as with a fork head on a 5-axis machine, for example, thus the design allows the machine to carry out 5-axis machining. "Pantograph" kinematic transformation is a type of 2-/4-axis transformation with parallel kinematics. It can work with fixed-length rods, or rods whose lengths can be modified. When using kinematic transformations, workpieces can be programmed in Cartesian coordinates as usual. The SINUMERIK control calculates the required movements of the machine axes online. Therefore, the programmer can create part programs in the same way as on a conventional machine, and does not have to take the special kinematics of the machine into account. High-level CNC languageTo meet the various technological demands of modern machine tools, a CNC high-level language has been implemented in SINUMERIK that provides a high degree of programming freedom. System variables The system variables ($.) can be processed in the CNC program (read, partially write). System variables allow access to, for example, machine data, setting data, tool management data, programmed values, and current values. User variables If a program is to be used flexibly, variables and parameters are used instead of constant values. SINUMERIK gives you the option of executing all CNC functions and addresses as variables. The names of the variables can be freely defined by the user. Read and write access protection can also be assigned using attributes. This means that part programs can be written in a clear and neutral fashion and then adapted to the machine as required, for example, free selection of axis and spindle address designations. User variables are either global (GUD) or local (LUD). LUDs can also be redefined via machine data to make them into global program user data (PUD). They are displayed in the Parameters operating area under the user data softkey, where they can also be changed. Global user variables (GUD) are CNC variables that are set up by the machine manufacturer. They apply in all programs. Local user data (LUD) are provided for parameterizing CNC programs. These data can be redefined in every CNC program. These variables make programming more user-friendly and allow the users to integrate their own programming philosophy. Indirect programming Another option for the universal use of a program is indirect programming. Here, the addresses of axes, spindles, R parameters, etc., are not programmed directly, but are addressed via a variable in which their required address is then entered. Program jumps The inclusion of program jumps allows extremely flexible control of the machining process. Conditional and unconditional jumps are available as well as program branches that depend on a current value. Labels that are written at the beginning of the block are used as jump destinations. The jump destination can be before or after the exit jump block. Program coordination (in several channels) Program coordination makes it possible to control the time-related execution in parallel operation of several CNC channels using plain text instructions in the part program. Programs can be loaded, started and stopped in several channels. Channels can be synchronized. Arithmetic and trigonometric functions Extensive arithmetic functions can be implemented with user variables and arithmetic variables. In addition to the four basic arithmetic operations, there are also:
Comparison operations and logic combinations Comparison operations with variables can be used to formulate jump conditions. The comparison functions that can be used are:
The following logic combinations are also available: AND, OR, NOT, EXOR These logic operations can also be performed bit by bit. Macro techniques Using macros, single instructions from a programming language can be grouped together to form a complex instruction. This shortened instruction sequence is given a freely definable name and can be called in the CNC program. The macro command is executed in the same way as the single instructions. Control structures The control normally processes the CNC blocks in the order in which they are programmed. Like program jumps, control structures allow the programmer to define additional alternatives and program loops. The commands make structured programming possible, and make the programs much easier to read:
High-speed CNC inputs/outputs> Position switching signals/cam controller The "high-speed CNC inputs/outputs" function makes it possible to read in or to output signals in the position control/interpolation cycle. The high-speed CNC inputs/outputs can be used for machines, such as those used for grinding and laser machining, as well as in SINUMERIK Safety Integrated.
Output signals are possible for the following:
High-speed data exchange between CNC and PLCFor fast, immediate information exchange between CNC and PLC, 1024 bytes are available in the communications buffer for bidirectional input/output. Transfers are handled immediately. $A variables are used for CNC access, and a function block with which the data in the dual-port RAM (DPR) are immediately (rather than at the beginning of the PLC cycle) read or written is used for PLC access. This allows you, for instance, to respond to I/O signals right away in the part program, independent of the PLC cycle. HMI-Advanced user-interface on PC/PGWhen an MPI card is installed in a PC or PG, the complete user interface is available on that PG or PC. This allows user-friendly start-up and servicing of the controller when the system is operated with an OP 030 or without a console. It also makes setting up the machine and editing and executing workpiece programs easy and problem-free. I/O interfacing via PROFIBUS DP (option)> PLC area PROFIBUS DP represents the protocol profile for distributed I/Os. It enables extremely high-speed cyclic communication. Due to generation of an optimum subset of the PROFIBUS message services and increasing of the data signaling rate to a maximum of 12 Mbit/s, the bus cycle times are virtually negligible. Despite all this, the many advantages of PROFIBUS remain the same: high availability, data integrity and standard message structure. Activation of the integrated PROFIBUS DP interface connection for the NCUs/CCUs is available as a separate option. The NCUs/CCUs can be operated as master or slave. Distributed I/O devices (such as the ET 200) are connected for communication purposes. Even if the interface connection integrated in the NCUs is not activated, I/O devices can be operated via a SIMATIC S7-300 equipped with an IM 361 interface module and a CP 342-5 communications processor. In the case of SINUMERIK 840Di: the PROFIBUS DP interface is available on the MCI board in the basic version (for I/O and drive). Inclined axis (option)
Oblique plunge-cut grinding: machine with non-Cartesian X axis (U) The "inclined axis" function is used for fixed-angle interpolation using an oblique infeed axis (used primarily in conjunction with cylindrical grinding machines). The axes are programmed and displayed in the Cartesian coordinate system. Tool offsets and work offsets are also entered in the Cartesian system and transformed to the real machine axes. For oblique plunge-cutting with G05, it is necessary to program the start position with G07. In JOG mode, the grinding wheel can be traversed either in the Cartesian coordinate system or in the direction of inclined axis U (selection via the channel DB). Inclined-surface machining with frames> Frame concept 
Inclined-surface machining with frames Drilling and milling operations on workpiece surfaces that do not lie in the coordinate planes of the machine can be performed easily using the function "inclined-surface machining". The position of the inclined surface in space can be defined by coordinate system rotation. Intermediate blocks for tool radius compensation> Tool radius compensation Traversing movements with selected tool offset can be interrupted by a limited number of intermediate blocks (block without axis movements in the compensating plane). The permissible number of intermediate blocks can be set in system parameters. Interrupt routines with fast retraction from the contour (option)"Interrupt routines" are special subprograms which can be started on the basis of events (external signal) in the machining process. Any part program block currently in progress is interrupted. The positions of the axes at the time of interruption are saved automatically. It is also possible to save such things as the current states of G functions and the current offsets (SAVE mechanism) in buffer storage, making it possible to resume the program at the point of interruption later without difficulty. Four additional program levels are available for interrupt routines, that is, an interrupt routine can be started in the 8th program level and lead as high as the 12th program level. An interrupt (for example, the switching of a high-speed CNC input) can trigger a movement via the special subprogram, which allows fast retraction of the tool from the workpiece contour currently being machined. The retraction angle and the distance retracted can also be parameterized. An interrupt routine can also be executed following the fast retraction. Inverse-time feedrateOn the SINUMERIK, it is possible to program the time required to traverse the path of a block (rpm) instead of programming the feedrate for the axis movement with G93. If the path lengths differ greatly from block to block, a new F value should be determined in every block when using G93. When machining with rotary axes, the feedrate can also be specified in degrees/revolution. Involute interpolation (option)Using involute interpolation, it is possible to program a spiral contour with the shape of a so-called circular involute in one CNC block instead of many approximated individual blocks. The exact mathematical description of the contour enables a higher path velocity to be achieved, together with a reduction in machining time. Undesirable facets, which could result from coarse polygon functions, are thus avoided. Furthermore, it is unnecessary to define the end point for the involute interpolation exactly on the involute defined by the start point; it is possible to enter a maximum permissible deviation using machine data. Job listYou can use this function to create a "job list" (load list) for every workpiece to be machined. The list contains instructions on making the following preparations for executing part programs, even when multiple channels are involved:
You can also save your own templates for job lists. Following loading and job list selection, CNC start initiates the processing of all programs and data required for workpiece production. Languages/language expansionsOur control speaks your language! A user interface for the SINUMERIK controls is available in a number of different languages: The basic languages of English, German, French, Italian, Spanish and simplified Chinese have already been implemented for display texts on the user interface in the HMI-Embedded, HMI-Advanced, ShopMill and ShopTurn software. The operator can switch back and forth online between foreground and background languages. Laser switching signal, high-speed (option)For high-speed laser machining, e.g., of aperture plates, an automatic, high-speed, position-dependent signal is implemented for switching a laser on and off. Under the prerequisite that all movements for which the laser must be switched off are made in rapid traverse mode G0, it is possible to logically combine the switching signal for the laser with the rising or falling edge of G0. Furthermore, the laser switching signal can also be coupled to an adjustable G1 feedrate threshold value. To achieve the fastest possible responses, the switching on and off of the digital laser signal is controlled by the position controller, depending on the actual axis position. No programming measures are required for switching the laser itself on and off, as these procedures are directly linked to the programmed G functions. The overall procedure, however, requires programming of a release (at the beginning of the program) with CC_FASTON (DIFF1, DIFF2). Together with this release, the two offset values, which can offset the switching on and off of the laser by a specific path differential in relation to the position setpoint are entered. A negative value means an offset before the setpoint (derivative action), a positive value means an offset after the setpoint. If the programmed derivative action value is too high, that is, if the setpoint had already been exceeded when the edge was detected, the signal is switched immediately. Leadscrew error compensation / measuring system error compensationIn the SINUMERIK controls, "interpolating compensation" is divided into two categories:
The measuring principle of "indirect measurement" on CNC-controlled machines is based on the assumption that the lead of the ball screw is constant at every point within the traversing range, so that the actual position of the axis can be derived from the position of the drive spindle (ideal case). Tolerances in leadscrew production, however, result in more or less large dimensional deviations (referred to as leadscrew error). Added to this are the dimensional deviations occasioned by the measuring system used, as well as the assembly tolerances for that system on the machine (referred to as measuring system error) and any other machine-related error sources. Because these dimensional deviations directly affect the accuracy of workpiece machining, they must be compensated for by the relevant position-dependent compensation values. The compensation values are computed based on the measured error curve, and are entered in the controller in the form of compensation tables during startup. The relevant axis is compensated using linear interpolation between the intermediate points. Limit switch monitoring
Overview of travel limits Preceding the EMERGENCY-STOP switch, hardware limit switches, which take the form of digital inputs controlled via the PLC interface, limit the traversing range of the machine axes. Deceleration is effected either as rapid deceleration with setpoint zero or in accordance with a braking characteristic. The axes must be retracted in the opposite direction in JOG mode. Software limit switches precede the hardware limit switches, are not overtraveled, and are not active until reference point approach has been completed. Following preset, software limit switches are no longer effective. A second pair of plus/minus software limit switches can be activated via the PLC. Linear interpolation"Linear-Interpolation" is understood to be the CNC-internal calculation of points on a straight path between the programmed starting and end points. Up to 4 axes can already be linearly interpolated in the basic configuration of the SINUMERIK 810D powerline/840Di/840D powerline controls. Optional expansions are listed in the overview of functions. Limited functionality on the SINUMERIK 810DE powerline/840DiE/840DE powerline: interpolation with max. 4 axes. Link axis (option)Link axes are axes that are physically connected to another NCU and are governed by that NCU's position controller. Link axes can be assigned dynamically to channels on another NCU. Look Ahead> Continuous-path mode with programmable rounding clearance 
Comparison of velocity response with exact stop G60 and continuous-path mode G64 with look ahead for short displacements. During the machining of complex contours, most of the resulting program blocks have very short paths with sharp changes in direction. If a contour of this type is processed with a fixed programmed path velocity, an optimum result cannot be obtained. In short traversing blocks with tangential block transitions, the drives cannot attain the required final velocity because of the short path distances. Contours are rounded when traveling around corners. With the "look ahead" function, a specifiable number of traversing blocks are read in advance in order to calculate the optimum machining velocity. With tangential block transitions, the axis is accelerated and decelerated beyond block boundaries, so that no drops in velocity occur. On sharp changes of direction, rounding of the contour is reduced to a programmable path dimension. Look-ahead detection of contour violations
Behavior when tool radius > circle radius With CDON (Collision Detection ON) and active tool radius compensation, the control monitors tool paths through look-ahead contour calculation. This makes it possible for the control to actively detect and avert possible collisions. The control detects the following critical machining situations, for example when the tool radius is too large, and compensates through tool path modification.
Machining channels> Mode group Idle times can be shortened via a channel structure using parallel sequences of motion, such as moving a loading gantry during machining. A machining channel must be regarded as a separate CNC with decoding, block preparation and interpolation. The channel structure makes it possible to process the individual channels' part programs simultaneously and asynchronously. The relevant channel with the associated images is selected by pressing the "channel switchover" button on the operator panel. Part programs can then be chosen and started for that specific channel. With SINUMERIK 810D powerline/840D powerline, each of the maximum possible channels can be operated in its own mode group. Additional machining channels are optional. Machining package 5 axes (option)
Universal milling head Five-axis machining tasks, such as the milling of free-form surfaces, can be solved easily and in a user-friendly manner. To this end, the "5-axis machining package" provides the following functions:
Main program call from main program and subprogramIf machining operations recur frequently, it is advisable to store them in a subprogram. The subprogram is called from a main program (number of passes ?9999). Eleven subprogram levels (including 3 levels for interrupt routines) are possible in a main program. A main program can also be called from within another main program or subprogram. Master value coupling and curve table interpolation (option)> Measuring, stage 2; synchronous spindle 
Example for cyclic machines: Flying saw For special technologies (presses, transfer lines, printing machines, etc.), the replacement of mechanical, cyclic transport tasks with electronic functionality in AUTOMATIC mode requires constant coupling and decoupling functions between master and following axes. To this end, the "synchronous spindle" functionality has been expanded to include the "master value coupling" function, which makes it possible for linear master and following axes to be coupled via curve tables in the CNC program. Any and all functional associations between axis positions can be approximated. Soft coupling avoids the sudden change in velocity that occurs when the master axis is activated. Offsets (e.g., 12°), scalings (e.g., 1.00023) and mirroring using frame instructions are possible. Electronic curve table interpolation replaces the cam discs that were once required for the control of cyclic machines. Complex sequences of motion can be easily defined using familiar CNC language elements. The external reference variable (e.g. "line shaft") is formed by the controller's master value. The functional relation between leading and following axis can be subdivided into segments of the master axis (curve segments). In these curve segments, the link between master value and following value is described using mathematical functions (normally through 3rd degree polynomials). So-called "cyclic machines" are distinguished by constantly repeated cyclic operations with high throughput and high productivity in machining, transport, packaging and parts handling (for example packaging machines, presses, wood processing machines, printing machines). SINUMERIK makes it possible to implement technological functions, such as synchronism, electronic transfer and positioning for cyclic machines. Mechanics (line shaft, gearing, cam discs, couplings and cams) are replaced by an electronic solution (master value coupling, curve tables, synchronous actions, and electronic cams). In addition, the electronic functionality permits fast, axis-specific optimization, high-speed phase and path compensation, fast responses to faulty or missing parts, and fast synchronization and resynchronization, as well as decoupling from the master axis and executing autonomous movements. Axis cycles and synchronization calculations are carried out in the IPO cycle. Measuring from synchronous actions, for example, is used for detecting edges on continuous workpieces and for measuring pressure marks (on continuous film, for example). Starting with software release 6.3 of the NCU 572/573, the tables can also be saved and processed in the DRAM. The memory size can the set during the user memory configuration (maximum value is system-dependent). Limited functionality on the SINUMERIK 840DiE/840DE powerline: The number of simultaneously traversing axes is restricted to four. Master/slave for drives (option)
Example: Axis 1 is simultaneously the master axis for axis 2 and axis 3 The "master/slaves for drives" function is required when two electrical drives are mechanically linked to an axis. In a link of this kind, a torque controller ensures that both drives produce the exact same amount of torque, as otherwise the two motors would work against each other. In order to attain tensioning between the master and slave drives, a tension torque specifiable via machine data can be applied on the torque controller. Application examples:
An axis can also be a master axis for multiple links. Starting with software release 6.2, this functionality is already included in the NCU system software, i.e. a technology PC card is no longer required. Measuring stage 1You can connect up to two switching touch probes to the control at the same time. In the case of channel-specific measuring, the measuring process for a CNC channel is always activated from the part program running in the relevant channel. All of the axes programmed in the measuring block take part in the measuring process. You can program a trigger event (rising or falling edge) and a measuring mode (with or without deletion of the residual path) for each measuring process. The results of measurements can be read in the part program or with synchronous actions in both the machine and the workpiece coordination system. You can test the deflection of the touch probe by scanning a variable and outputting it to the PLC interface and deriving responses in the part program. The "measuring stage 2" option provides you with expanded functionality (for example for axial measuring, evaluating up to 4 trigger events, and cyclic measuring). Measuring stage 2 (option)While the measuring function in motion blocks in the part program is limited to one block, you can activate measuring functions from synchronous actions at any time, independent of the part program. The measuring events can be assigned to the axes in the CNC block. In the case of simultaneous measuring, up to 4 trigger events can be evaluated per position control cycle. Measured values are read as a function of the three parameters: touch probe, axis and measuring edge. In the case of continuous (cyclic) measuring, the measurement results are written to a FIFO variable. Endless measuring can be achieved by reading out the FIFO values cyclically. Measurement results can be optionally logged in a file on the controller or output to a printer or PC via the V.24 interface. The standard protocol contained in the measuring cycles can be modified by the user as required. Limited functionality on the SINUMERIK 810DE powerline/840DiE/840DE powerline: Measuring from synchronous actions and cyclic measurement are not possible (no functional limitation from NCU SW version 6.5). Measuring system 1 and 2, selectableFor special applications, two encoders can be assigned to one axis, e.g., a direct measuring system for the machining process with high demands on accuracy, and an indirect measuring system for high-speed positioning tasks. The switchover between measuring systems 1 and 2 is performed via the PLC. Measuring system error compensation> Leadscrew error compensation / measuring system error compensation Measuring systemsOn the SINUMERIK 840D powerline/840Di, the measuring systems are evaluated by the SIMODRIVE 611 digital drive modules with high resolution. The SINUMERIK 810D powerline evaluates the measuring systems directly on the CCU module. With the SINUMERIK 810D powerline, additional measuring systems can be connected via axis expansion with SIMODRIVE 611 digital modules. Mode group (MG)A mode group (MG) combines CNC channels with axes and spindles to form a machining unit. A mode group contains channels that must always be in the same mode at the same time during the machining sequence. Within a mode group, every axis can be programmed in every channel. A mode group can be regarded as an independent, multi-channel CNC. Additional mode groups are optional. Monitoring functionsThe controls contain watchdog monitors, which are always active. These monitors detect faults in the CNC, PLC or machine in time to prevent damage to workpiece, tool or machine. When a fault occurs, the machine operation is interrupted and the drives brought to a standstill. The cause of the fault is saved and displayed as an alarm. At the same time, the PLC is notified that a CNC alarm has been triggered. Monitoring functions exist for the following areas:
Motion Control with PROFIBUS DPCompatible extension of the PROFIBUS DP standard for the synchronization of bus nodes, making it possible to implement reliable control algorithms, such as the closing of a position control loop, via the bus. Isochronous mode The mechanisms for synchronization of the internal time levels in master and slave global control (broadcast message), PLL (phase lock loop), as well as the constant bus cycle time (isochronous mode), give the application/control cycles in the master and in the participating slaves a fixed time relationship to one another. Data Exchange Broadcast (internode communication) Efficient data exchange between slaves without delays imposed by the master. Data sent by one slave can be monitored by the slaves that have been requested to do so, allowing them to respond (e.g. actual position values). Motion-synchronous actions> Synchronous actions Multi-axis interpolation (option)On the SINUMERIK 810D powerline/840Di/840D powerline, the number of interpolating axes is expandable. The number of interpolating axes is limited by options and machine data, as well as by the number of axes in the channel. Multi-axis interpolation is not possible for SINUMERIK 810DE powerline/ 840DiE/840DE powerline. Multi-channel displayIn the machine operating area, the M key can be used to select either the single-channel or multi-channel display. In the multi-channel display, only channel information is displayed; the channel can be operated or influenced in the single-channel display. The multi-channel display can, of course, be operated despite this: focus switching, scrollbars and window selection can be operated, but no changes are possible in the NC channel data. The same windows are always displayed together in all channels. The softkeys for switching the windows, therefore, always affect all the channels that are on display. In the multi-channel display, the actual axis value is shown in the top window and the selection menus (T/F/S values, program records etc.) are shown in the bottom window depending on which softkeys are activated. Multi-channel step sequence programming (option)The "Multi-channel step sequence programming" option makes it easier to edit, navigate and time-optimize multi-channel workpiece programs. The steps in a part program can be visualized graphically either in the compensation block editor in the machine/simulation operating areas or in the program editors of all operating areas. The graphics are displayed in the form of icons either without a time reference (standardized display) or with a time reference (the height of the step icons is proportional to the time required by this step). Multiple feedrates in one blockDepending on external digital and/or analog inputs, you can use this function for motion-synchronous activation of up to 6 different feedrates, a dwell time, and a retraction in a single CNC block. The input signals are combined in an input byte with a permanently assigned function. The retraction is initiated by an amount defined in advance within an IPO cycle. Retraction movement or dwell time (e.g., sparking-out time during grinding) lead to deletion of the distance-to-go. Typical applications involve analog or digital calipers or a change from infeed feedrate to machining feedrate via proximity switches. During internal grinding of a ball bearing ring, for instance, in which calipers are used to measure the actual diameter, the feedrate value required for roughing, finishing or smooth-finishing can be activated depending on threshold values. Multipoint interface (MPI)The operator panel and the machine control panel communicate with the CNC via a multipoint interface. Via this interface, several devices can be connected and communicate with the CNC as would be the case in a bus system. On the SINUMERIK 810D powerline, the MPI is located on the front panel of the CCU module. The data signaling rate is 187.5 Kbit/s. On the SINUMERIK 840Di, the MPI is located on the MCI board. The data signaling rate is 1.5 Mbit/s. In addition to the PG MPI interface (187.5 Kbit/s), the NCU modules of the SINUMERIK 840D powerline are also equipped with a high-speed operator panel interface (BTSS) that has a data signaling rate of 1.5 Mbit/s and is used to connect operator panel, machine control panel, hand-held programming unit, and pushbutton panel. NCU-independent setpoint linkage (option)> Link axis This functionality permits coupled axes beyond NCU limits as an extension to the "Link axis": the master axes and the following axis can execute on different NCUs. This option can be used as a setpoint linkage for the following coupled axes: master value coupling (plus simulated master value), coupled motion, synchronous spindle, electronic gear unit and tangential control. Applications include e.g. multi-spindle turning machines, or transfer controls of presses. Number of subprogram repetitionsIn order to execute a subprogram several times in succession, the desired number of program repetitions can be programmed in the block with the subprogram call at address P (range of values: 1 ... 999). Parameters are transferred only when the program is called or in the first pass. The parameters remain the same for all repetitions. If you want to change the parameters between passes, you should make the relevant declarations in the subprogram. Offline ISO dialect/CNC program converterThis program converter allows you to convert both external and Fanuc0 programs, as well as workpiece programs for the SINUMERIK 800 controls into the format for the SINUMERIK 810D powerline/840Di/840D powerline. Online ISO dialect interpreter (option)With the online ISO dialect interpreter, part programs in other ISO dialects (for example, G codes from other manufacturers) can be read into the SINUMERIK 810D powerline/840Di/840D powerline, edited, and processed. Operating modesIn the "Machine" operating area, you have a choice of three operating modes:
In the operating modes MDI and AUTO, you can modify the sequence of a program using the following "program control" functions: SKP Skip block (up to 8 skip levels) DRY Dry run feedrate ROV Rapid traverse override SBL1 Single block with stop after sets of machine functions SBL2 Single block with stop after every block SBL3 Stop in cycle M01 Programmed stop DRF Differential resolver function PRT Program test Oscillation functions (option)
Oscillation functions With this function, an axis oscillates at the programmed feedrate between two reversal points. A possible application is a grinding machine. Asynchronous oscillation across block boundaries Several reciprocating axes may be active. During reciprocating movement, other axes can interpolate at will. The reciprocating axis can be the input axis for the dynamic transformation or the master axis for gantry or coupled-motion axes. Block-related oscillation
Behavior of the reciprocating axis in the reversal point:
The spindles can also perform reciprocating movement. Pair of synchronized axes (gantry axes) (option)
Gantry axes (pair of synchronized axes X/X1) With the "gantry axes" function, the axes of up to eight pairs of mechanically coupled axes can be traversed simultaneously without mechanical offset. The actual values are continuously compared and even the smallest deviations corrected. During both operation and programming, the axes defined in a gantry grouping are treated like machine axes. A gantry grouping consists of a master axis and up to two synchronized axes. Two master axes can be coupled using curve table interpolation. Up to three gantry groupings can be defined per control system (up to three gantry groupings with NCU 571.5). Part program managementPart programs can be organized according to workpieces. This permits clear allocation of programs and data to the respective workpieces. The size of the user memory determines the number of programs and the amount of data that can be managed. Each file (programs and data) can be assigned a name comprising up to 23 alphanumeric characters. Path length evaluation (option)> Synchronous actions With the option "Path length evaluation", with the SINUMERIK 810D powerline/840D powerline from software version 6, data can be backed up in the controller that allows conclusions to be drawn about the service status of the machine. In the first stage, the following data are acquired:
These data are stored in the SRAM but are retained beyond Power On/Off and can be read using the operator panel interface. Using an external utility, consistent data can, therefore, be achieved for the complete life cycle of a machine. These data can also be read through system variables in the part program and in synchronous actions. Path-velocity-dependent analog output (option)"Tool-path velocity-dependent analog output" makes it possible to output the current path velocity in the interpolation cycle. This value can, for example, be made available via a module "DMP Compact 1 A analog" on the NCU terminal block (on the SINUMERIK 840Di, via PROFIBUS DP and S7-300 output modules). The function is programmed via synchronous actions. One application is laser power control. PC card/CF card as additional program memoryWith PCU 20, the existing PC card plug-in unit can be used with a PC card or CF card (through PC card adapter) as an additional external program memory. Programs can be copied in both directions between the PC card and the part program memory of the controller. The programs can also be written onto the PC card from the external PC via Ethernet or from the connected floppy disk drive. The function "processing from external source" enables direct processing of programs present on the PC card. Plain text display of user variables> High-level CNC language In addition to the predefined variables, programmers can define their own variables and assign values to them. The variables are displayed in plain text format (e.g., definition: DEF INT NUMBER/Display: NUMBER or definition: DEF REAL DEPTH/Display: DEPTH). PLC areaSINUMERIK 810D powerline In the SINUMERIK 810D powerline, a PLC 314C-2 DP that is compatible with SIMATIC S7-300 is integrated into the CCU 3.4. PROFIBUS I/O components can be operated on the PLC 314C-2 DP. As I/O modules, you can use either SIMATIC S7-300 components or single I/O modules. SINUMERIK 840Di On the SINUMERIK 840Di, a SIMATIC S7-300-compatible PLC 317-2DP is integrated on the MCI board. The SIMATIC DP ET 200 with 12 Mbaud capability can be connected to the PROFIBUS DP as I/O. SINUMERIK 840D powerline On the SINUMERIK 840D powerline, a SIMATIC S7-300-compatible PLC 317-2 DP is integrated in den NCUs 561.5/571.5/572.5 and NCU 573.5. The same components as on the SINUMERIK 810D powerline can be used as I/O modules. PLC programming (STEP 7) The PLC in the SINUMERIK is programmed using the user-friendly STEP 7 software. The STEP 7 programming software is based on the Windows operating system, and combines the proven STEP 5 programming functions with innovative further developments. The STL (statement list), FBD (function block diagram), and LAD (ladder diagram) programming languages are available. The user can switch from one to the other using STEP 7 pull-down menus. The following blocks are available for structured programming:
In addition, system function blocks (SFBs) and system functions (SFCs) integrated in the operating system can also be called. The STEP 7 software package (for SIMATIC S7-300) is a standard component of SIMATIC programming devices (e.g., Field PG). A software package for standard industrial PCs is also available. The PLC can also be programmed in other SIMATIC S7 high-level languages, such as S7 HiGraph and S7 Graph. PLC/NCK interface A number of functions can be executed via the NCK and PLC interface, ensuring excellent machining flexibility. Some of these are:
The PLC basic program, which is part of the toolbox, organizes the exchange of signals and data between the PLC user program and the NCK, PCU and machine control panel areas. In the case of signals and data, a distinction is made between the following groups:
PLC programming with HiGraphThe HiGraph method is used for describing technical systems and converting these descriptions into PLC programs. With HiGraph, a machine or plant is seen as a combination of separate functional units. These functional units can be made up of basic mechanical and electrical elements. The HiGraph method is used in the automation of machines and plants where mechanical movement and sequences take priority, e.g. machine tools, transfer lines, and conveyor and transportation systems. The HiGraph method can be used:
Advantages of the HiGraph method:
PLC statusIn its "diagnostics" area, the operator panel allows you to check and modify PLC status signals. This makes it possible for you to take care of the following right on site:
The status of the following data items can be displayed separately on the operator panel:
For test purposes, you can also change the status of the above-listed signals. Signal combinations are also possible, and as many as 10 operands can be modified simultaneously. PLC user memoryIn the PLC user memory of the PLC CPU, the PLC user program and the user data are stored together with the PLC basic program. The memory of the PLC CPU is divided up into load memory, work memory and system memory. Load memory is retentive, and takes the form of either integrated RAM or a RAM module (plug-in memory card). It contains data and program and decompiling information. The load memory and the high-speed work memory for execution-relevant program tests provide sufficient space for user programs. Polar coordinatesProgramming in polar coordinates, it is possible to define positions with reference to a defined center point by specifying the radius and angle. The center point can be defined by an absolute dimension or incremental dimension. Polynomial interpolation (option)
Polynomial interpolation With this function, curves can be interpolated for which the CNC axes follow the function: f(p) = a0 + a1p + a2p2 + a3p3 (polynomial, up to 3rd degree) or from software release 6 onwards: f(p) = a0 + a1p + a2p2 + a3p3 + a4p4 + a5p5 (polynomial, max. 5th degree) The coefficient a0 is the end point of the previous block, a1 is calculated as the end point of the current block, a2, a3, a4, and a5 must be calculated externally and then programmed. With polynomial interpolation, it is possible to generate many different curve characteristics, such as straight line, parabolic and exponential functions. Tool radius compensation can be used as in linear and circular interpolation. 5th degree polynomials, in contrast to 3rd degree polynomials, permit further approximation of defined contours. However, polynomial interpolation primarily serves as an interface for programming externally generated spline curves. 5th degree polynomials can optionally be used if the coefficients are obtained directly from a CAD/CAM system ("closer to the surface"). A prerequisite for efficient utilization of this polynomial interpolation is therefore a corresponding CAD/CAM system. Position monitoringSINUMERIK controls provide extensive monitoring mechanisms for axis monitoring:
The "positioning monitor" is always activated following "setpoint-based" termination of traversing blocks. To ensure that an axis is in position within a specified period of time, the timer configured in the machine data is started when a traversing block terminates; when the timer expires, a check is made to ascertain whether the following error fell below the limit value (machine data). When the specified "fine exact stop limit" has been reached or following output of a new position setpoint other than zero (e.g. after positioning to "coarse exact stop" and subsequent block change), the positioning monitor is deactivated and replaced by the zero-speed monitor. Position monitoring is effective for linear and rotary axes as well as for position-controlled spindles. In follow-up mode, position monitoring is not active. Position switching signals/cam controller (option)> High-speed CNC inputs/outputs Position-dependent interface signals for the PLC can be set using position switching signals. The position values at which the signal output and a derivative action/hold up time are to be set can be programmed in the part program and entered via the setting data. The function can be controlled via the PLC. The function is used for applications such as activating protection areas or position-dependent triggering of movements (e.g. hydraulic reciprocating axes during grinding). 32 position signal pairs are available (with SINUMERIK 810DE powerline: 16 signals). The position signals are output in the IPO cycle. They can also be output with the function "high-speed digital CNC inputs/outputs" as switching outputs in the position control cycle. Positioning axes and spindles via synchronous actionYou can position axes or spindles in dependence on conditions (the actual values of other axes, high-speed inputs, etc.) with a special feedrate or speed to a specific setpoint via synchronous actions. Synchronous actions are executed in the interpolation cycle, are carried out in parallel with the actual workpiece machining procedure, and are not limited to CNC block boundaries. These so-called command axes and command spindles can be started in the IPO cycle direct from the main program. The path to be traversed is either predefined or is calculated from real-time variables (with expanded arithmetic functions) in the IPO cycle. Spindles can be started, stopped or positioned asynchronously depending on input signals without PLC intervention. Positioning axes/auxiliary spindlesPositioning axes can execute movements simultaneously with machining, thus reducing non-productive times considerably. They can be used to advantage when controlling workpiece and tool feeders or tool magazines. They can be programmed with an axis-specific feedrate in the part program. Axis movement beyond block boundaries is also possible. Positioning axes can also be controlled by the PLC. This means that axis movements can be started independently of the part program without using up an additional machining channel. Auxiliary spindles are speed-controlled spindle drives without an actual-position sensor, e.g., for tool drives. PresetWith the "preset function", you can redefine the control zero in the machine coordinate system. The preset values affect machine axes. "Preset" does not cause the axes to move, but a new position value is entered for the current axis positions. After new actual values are set, protection zones and software limit switches, only reactivated after a new reference point approach! PROFIBUS DPPROFIBUS DP is the protocol for the distributed I/O, and is based on the international open fieldbus standard as laid down in European fieldbus standard EN 50170 Part 2. PROFIBUS DP is optimized for high-speed, time-critical data exchange at the field level. This fieldbus is used for cyclic and non-cyclic data transfer between a master and its assigned slaves. Master, active bus nodes Devices which control the data traffic on the bus are referred to as masters. They send requests in the form of control words and setpoint values. Masters are divided into two classes:
Slaves, passive bus nodes These are devices which receive, acknowledge, and forward messages to the master at the master's request (SIMODRIVE 611 universal HR, POSMO SI/CA/CD, SIMATIC I/O). They send responses in the form of status words and actual values. Transfer PROFIBUS supports data transfer in accordance with RS 485 and Optical Link. Baud rates 9.6 kbaud, 19.2 kbaud, 45.45 kbaud, 93.75 kbaud, 187.5 kbaud, 500 kbaud, 1.5 Mbaud, 3.0 Mbaud, 6.0 Mbaud, 12 Mbaud. A maximum of 1.5 Mbaud for optical link plugs (OLP). PROFIBUS tool and process monitoring (option)Using the "PROFIBUS tool and process monitoring" function, the digital drive data for torque, active power and actual current are made directly available for evaluation via the PROFIBUS DP interface. One or two PROFIBUS slaves can be connected. Program preprocessing (option)The execution time of a CNC program can be reduced considerably by the preprocessing of cycles. The programs in the directories for standard and user cycles are preprocessed at "power on" with set machine data. Especially in the case of programs containing portions written in a high-level language and of compute-bound programs (e.g. programs containing check structures, motion-synchronous actions or cutting cycles), execution times can be reduced by up to 1/3. Programmable accelerationWith the function "programmable acceleration" it is possible to modify the axis acceleration in the program in order to limit mechanical vibration in critical program sections. The path or positioning axis is then accelerated at the programmed value. The acceleration value set in the machine data can be exceeded by up to 100 %. This limitation is active in AUTOMATIC mode and in all interpolation modes. As part of intelligent motion control, this function provides a more precise workpiece surface. Programming languageThe CNC programming language is based on DIN 66025. The new functions of the CNC high-level language also contain macro definitions (combined sequences of instructions). Protection zones 2D/3D
Protection zones Protection zones allow you to protect various elements on the machine and its equipment, as well as the workpiece to be created, from incorrect movements. Some of the elements that can be protected are, for example:
For the elements to be protected, 2D or 3D protection zones are defined in the part program or via system variables. These protection zones can be activated and deactivated in the part program. Protection zones must always be divided into workpiece-related and tool-related zones. During machining in JOG, MDA or AUTOMATIC mode, a check is always made to see whether the tool (or its protection zones) violate the protection zones of the workpiece. Monitoring of the protection zones is channel-based, that is, all active protection zones for a channel are mutually monitored for collisions (protection zones not channel-specific with NCU system software for 2/6 axes). A maximum of 10 protection zones and 10 contour elements which describe a protection zone are available (with NCU 561.5 and NCU 571.5: max. 4 protection zones and 4 contour elements). Punching/nibbling (option)The punching/nibbling functions are implemented essentially via the language commands, stroke control and automatic path division.
Quadrant error compensation
Quadrant transitions without compensation 
Quadrant transitions with quadrant error compensation Quadrant error compensation (also referred to as "friction compensation") ensures a much higher degree of contour precision, particularly when machining circular contours. At the quadrant transitions, one axis traverses at the maximum path velocity while the second axis is stationary. The different friction conditions can cause contour errors. Quadrant error compensation virtually eliminates this problem and produces excellent results, without contour errors, in the very first machining operation. In operator-controlled quadrant error compensation, you set the intensity of the correction pulse as per an acceleration-based characteristic. This characteristic is determined and parameterized on startup with the aid of the circularity test. During the circularity test, deviations of the actual position from the programmed radius (particularly at the quadrant transitions) are recorded by measurement and graphically represented while the circular contour is being retracted. Quadrant error compensation, automatic (option)To simplify startup, the compensation characteristic for "Quadrant error compensation" with a neural network need no longer be set manually by the commissioning engineer. It is automatically determined during a learning phase, and saved in the buffered user memory. The neural network can simulate the compensation characteristic far better, achieving an improved accuracy, and permits simple and automatic subsequent optimization on site at any time. Reference point approachWhen using a machine axis in program-controlled mode, it is important to ensure that the actual values supplied by the measuring system agree with the machine coordinate values. Reference point approach (limit switch) is performed separately for each axis at a defined velocity either using the direction keys, in a sequence that can be defined in the machine data, or automatically via program command G74. If length measuring systems with distance-coded reference marks are used, reference point approach is shorter, as it is necessary to approach only the nearest reference mark. Reference point approach of an axis with absolute-value encoders is carried out automatically when the control is switched on (without movement of axis), if the corresponding axis is recognized as being calibrated. ReposFollowing a program interruption in AUTOMATIC mode (e.g., to take a measurement on the workpiece and correct the tool wear values or because of tool breakage), the tool can be retracted from the contour manually after changing to JOG mode. In this case, the control stores the interruption point coordinates and displays the differential travel of the axes in JOG mode in the actual-value window as a Repos (repositioning) offset. The contour can be reapproached:
Representation (2D) of 3D protection zones/work areas> Working area limitation; protection zones You can use protection zones to protect various elements on the machine, their components and the workpiece against incorrect movements. The three-dimensionally programmed protection zones are displayed two-dimensionally.. This also applies to the programmed working area limitations. Rotary axis, turning endlesslyDepending on the application, the working area of a rotary axis can be limited via a software switch (e.g., working area between 0° and 60°) or to a corresponding number of rotations (e.g., 1000°), or it can be unlimited (endlessly turning in both directions). This function can also be used with absolute-value encoders. Safety Integrated (option)
Safety functions> Safety Integrated (option) SINUMERIK Safety Integrated provides integrated safety functions that support the implementation of highly effective personnel and machine protection. The safety functions comply with the requirements of Category 3 according to EU standard EN 954-1 and safety integrity level SIL 2 of DIN EN 61508. Consequently, important functional safety requirements can be implemented easily and economically. Available functions include, among others:
Sag compensation, multi-dimensional (option)
Example: Sag compensation Multidimensional compensation is also possible for the effects of physical influences and manufacturing tolerances such as sag or leadscrew pitch errors. The compensation tables can be switched from the PLC. When the reference axis and the compensating axis are identical, leadscrew pitch errors can be compensated. By transferring weighting factors (PLC interface), stored compensating characteristics can be adapted to different conditions (e.g., tools). The most important features of interpolation and compensation using tables are as follows:
Limited functionality on the SINUMERIK 810DE powerline/840DiE/840DE powerline: The correctable tolerance band is limited to 1 mm (0.039 in) (for SINUMERIK 810D powerline/840Di/840D powerline to 10 mm (0.39 in)). Scratching, determining work offsetA work offset can also be determined through "scratching", taking into consideration an (active) tool and, where applicable, the base offset, by moving the axis to the workpiece, entering the desired setpoint position (e.g. "0"), and the controller calculates the work offset. Screen blankingWhen screen blanking is activated, both the screen and backlighting of the operator panel go blank under PLC control or after a programmable period of time has elapsed. This increases the service life of the screens. Separate path feed for corners and chamfersTo optimize solutions for machining tasks, a separate path feed can be programmed with FRCM (modal) or FRC (non-modal) for the "corner" and "chamfer" contour elements. Feed reduction thus makes it possible to achieve the desired geometrically precise definition of corners and chamfers. Serial interface (RS 232 C)A serial interface (RS-232-C) is provided for data input/output on the PCU. This interface can be used to load and archive programs and data. The interface can be operated and initialized menu-driven on the operator panel. Series machine startupFiles called series machine startup files can be generated to enable transfer of a particular configuration, in its entirety, to other controls that use the exact same software version, for example, controls that are to be used for the same machines. Series machine startup thus means bringing a series of controls to the same initial state as regards their data. You can archive/read selected CNC, PLC and PCU data for series machine startup. Compensation data can be optionally saved. The drive data are stored as binary data, and cannot be modified. Series machine startups can even be performed readily and easily without a programming device. Simply create a startup file in the PCU, save it on a PC card in the control, insert this card in the next control, and begin the series machine startup procedure. Set actual valueThe "set actual value" function is provided as alternative to the "preset" function. To use this function, the control must be in the workpiece coordination system (WCS). With "set actual value", the workpiece coordination system is set to a defined actual coordinate and the resulting offset between the previous and a newly entered actual value computed in the WCS as 1st basic offset. The reference points remain unchanged. Setpoint exchangeThe "setpoint exchange" function is used on milling machines with special milling heads on which, for example, the spindle motor is used both for driving the tool and for orientation of the milling head. In this case, the spindle and the milling head axes are defined as independent axes, but are traversed only in succession by one motor. It is possible to connect up to four axes to one motor. The axes, between which a setpoint exchange takes place, can be assigned to different channels or mode groups. Simulation
Simulation of drilling/milling with HMI-Advanced 
Simulation of turning with HMI Advanced Machining simulations, with emphasis on drilling/milling and turning technologies, can be executed on the controller's HMI in the workpiece coordinate system for certain machine kinematics depending on the active operating software and its versions: HMI Advanced
HMI Embedded
ShopMill ShopMill uses SINUMERIK's high computing performance to achieve intelligent simplification of the programming of milling work. It also respects the knowledge that the solving of complex tasks (e.g. 3D surface sections) is reserved for appropriate CAD/CAM software. Therefore particular value has been placed on easy programming of simple workpieces, as encountered in the majority of parts for machining.
ShopTurn ShopTurn contains a simulation for the produced program for horizontal turning machines. The simulation for machining on vertical turning machines is displayed horizontally. A differentiation is made with ShopTurn between "Simulation" (simulation prior to machining) and "Simultaneous recording" (real-time simulation during workpiece machining). The machining with the tool cutting edge is displayed in both cases: the required data are obtained from the tool list, separate input of tool data for the simulation is unnecessary. Since the tool data are read directly from the NC memory, it is guaranteed that current data are used. The machining time is displayed in both simulation modes. The dimensions of the unmachined part are entered in the program header of ShopTurn programs. If DIN/ISO programs are simulated, the unmachined part is not displayed.
Skip blocksCNC blocks which are not to be executed in every program pass (e.g. execute a trial program run) can be skipped. Skip blocks are identified by placing a "/" character in front of the block number. The instructions in the skip blocks are not executed and the program resumes with the next block that is not skipped. As many as 8 skip levels (level 0 to level 7) may be programmed. The individual skip levels can be activated via a data block in the PLC interface. Spatial error compensation (SEC 3D) (option)In addition to the "leadscrew error compensation", "sag compensation" and "temperature compensation" functions, "SEC 3D" provides a further static compensation which allows the machine manufacturer to improve the machine accuracy. The compensation data for SEC 3D are not based on an error model. Errors are measured with the aid of an external measuring instrument (e.g., a laser tracker) on spatial grid points dimensioned for the relevant machine. The control interpolates these compensation values while the machine moves within its working area limits. Spindle functionsSpindle modes are:
Functions of the spindle modes:
1) Prerequisite: actual-position sensor (measuring system) with corresponding resolution (mounted directly on the spindle). Spindle speed limitation> Spindle functions Spline interpolation (option)Using "spline interpolation" it is possible to obtain a very smooth curve from just a few defined interpolation points along a set contour. The intermediate points are connected by polynomials. The compressor converts linear motions (e.g., from CAD) at block transitions to splines of constant speed (COMPON) or splines of constant acceleration (COMPCURV). This yields soft transitions that reduce wear on the mechanical parts of the machine tool. However, if the intermediate points are placed close together, quite sharp edges can also be programmed. The "spline interpolation" function also considerably reduces the number of program blocks required. Extremely "smooth" workpiece surfaces are often extremely important with mold and tool making, both optically and technologically, e.g. for rubber gaskets. With the COMPCAD compressor, "smooth" curves can be approximated within the boundaries of compressor tolerance (parallel tool paths) and surfaces of a high optical quality can also be obtained in the case of large tolerances. Tool radius compensation is possible in spline interpolation, as it is in linear or circular interpolation. Every polynomial can represent a spline. Only the algorithm determines the type of spline.
Spline interpolation for 3-axis machining is suitable for simple applications and for the JobShop area. Standstill monitoring> Position monitoring "Standstill monitoring" represents one of the most comprehensive mechanisms for monitoring axes. The monitor checks to see whether the following error has reached the "zero speed tolerance" limit following the elapse of a programmable time period. Upon termination of a positioning action, standstill monitoring takes over from position monitoring, and checks to see whether the axis moves further from its position than stipulated in the machine data's "zero speed tolerance" field. The zero speed monitoring function is always active following expiration of the "zero speed delay time" or upon reaching the "fine exact stop" limit as long as no new traversing command is pending. When the monitor responds, an alarm is generated and the relevant axis/spindle brought to standstill with rapid stop via a speed setpoint ramp. Standstill monitoring is effective for linear and rotary axes as well as for position-controlled spindles. Standstill monitoring is inactive in follow-up mode. Start-up support for SIMODRIVE 611 digitalFor fast, user-friendly initial start-up of the SIMODRIVE 611 digital drives and for optimizing the control loops, start-up software is available for standard industrial PCs/PGs with an MPI card. The start-up software is integrated in the PCU 50/PCU 70. With this software, the drive configurations can be entered and the drives can be parameterized. The configuration of motor and drive module determines which standard data records are loaded. The drive and control parameters can also be archived on the PG/ PC. Additional tools are available for optimization and diagnostics. Time range measuring functions
Frequency range measuring functions
The measurement diagrams can be archived and are suitable for documenting the machine settings. They are an excellent means of quickly optimizing the current, speed and position control. In addition to conventional means of recording in the time range (step response of the speed and position control loop is a familiar method), it is also possible to analyze the behavior of the drive and machine in the frequency range using FFT (fast Fourier transformation). Start-up trace No additional oscilloscope is required for axis optimization with SINUMERIK 810D powerline or SINUMERIK 840D powerline, as the implemented installation and start-up software can be used to record up to 4 servo signals per position control cycle. The control system response can be specifically measured, for example on a block change and in the event of a change in the level of digital signals. Trigger conditions and measuring duration for measured-value recording are freely selectable. Subprogram levels and interrupt routinesSubprograms can be called not only in the main program, but also in other subprograms. Subprograms can be nested to a depth of 12 levels, including the main program level. That means that a main program may contain as many as 11 nested subprogram calls. Three levels are needed when you are using Siemens machining and measuring cycles. If such a cycle is to be called from a subprogram, the call can be nested at a depth of no more than 9. Starting with software release 6, programs can also be called event-controlled following resetting of the part program start or end, or following booting of the controller. Users can then make the basic function settings or carry out initializations using a part program command. A system variable can be used to scan the event, which activated the associated program. Synchronized actions stage 2 (option)More than 16 synchronous actions can be active in the CNC block. As many as 255 parallel actions can be programmed in each channel. Technology cycles can be combined into programs using synchronous actions, making it possible, for example, to start axis programs in the same IPO cycle by scanning digital inputs. Limited functionality on the SINUMERIK 810DE powerline/840DiE/840DE powerline: The number of simultaneously traversed axes is limited to 4 (path and positioning axes). Synchronous actions> Cross-mode actions Even in its basic configuration, a SINUMERIK control allows you to initiate up to 16 actions synchronous to the axis and spindle movements. These actions execute in parallel with workpiece machining, and their inception can be determined on the basis of conditions. The starting of such motion-synchronous actions (or synchronous actions for short) is, therefore, not restricted to CNC block boundaries. "Synchronous actions" are always executed in the interpolation cycle. Several actions can even be carried out in the same IPO cycle. Synchronous actions without validity identifier are active non-modally only in automatic mode. Synchronous actions with validity identifier ID are modal in the subsequently programmed blocks in AUTOMATIC mode. Statically effective synchronous actions with the identifier IDS remain active in all operating modes (see "Mode-independent actions"). The "synchronous actions" provide you with an excellent tool which allows you to respond very quickly to events in the interpolation cycle. Here are some typical applications:
Limited functionality on the SINUMERIK 810DE powerline/840DiE/840DE powerline: Only one active synchronous function (SYNFCT) is possible at a time. The number of simultaneously traversed axes is limited to 4 (path and positioning axes). Synchronous spindles/multi-edge turning (option)
Examples for synchronous spindles/multi-edge turning True-to-angle synchronization of one leading and one or more following spindles enables on-the-fly workpiece transfer, particularly for turning machines, from spindle 1 to spindle 2, for example for the purpose of finishing, without experiencing the non-productive times normally associated with rechucking. In addition to the speed synchronism, the relative angular position of the spindles to one another, e.g., on-the-fly, position-oriented transfer of edged workpieces, is also specifiable. On-the-fly transfer:
Finally, specification of an integer transformation ratio between the main spindle and a "tool spindle" provides the prerequisites for multi-edge machining (polygon turning). Multi-edge turning: n 2 = T · n1 Configuring and selection take place either via the CNC program or operator panel. Several pairs of synchronous spindles can be implemented. Tangential control (option)
Representation of a rotatable tool axis and die during punching/nibbling Tangential control makes it possible to correct a rotary axis in the direction of the tangents of two path axes. The two leading axes and the corrected axis lie in the same channel. Applications:
Tangential control is effective in all interpolation modes. On punching and nibbling machines with a rotatable punching tool and associated lower tool, the following functions may be used to ensure universality of the tool:
Tapping with compensating chuck/rigid tapping> Spindle functions Teach-in with HT 6 handheld terminal"Teach-in" is generally taken to mean the transfer of current positions to the CNC program. When teaching with the HT 6 handheld terminal in AUTO mode, it is possible not only to transfer the program but also to test and correct it immediately. The program is stopped and the axes are moved into the desired position with the JOG keys. This position is transferred to the program as a traversing block and can then be started again at any point. A reset is not required. Positions already taught in the program can be corrected, and new positions can be inserted. Other program statements can be modified as required. Temperature compensation (option)Heat causes machine parts to expand. This expansion depends, among other things, on the temperature and on the thermal conductivity of the machine parts. The actual positions of the individual axes, which change on the basis of variations in temperature, have a negative effect on the precision with which workpieces are machined. These actual value modifications can be corrected using temperature compensation. At a specific temperature, measure the actual-value offset over the positioning range of the axis to obtain the error curve for this temperature value. Error curves for different temperatures can be defined for each axis. In order to ensure proper compensation of thermal expansion in changing temperatures, the temperature compensation value, reference position, and linear angle of lead parameters must be transferred from the PLC to the CNC via function blocks each time the temperature changes. Abrupt changes in these parameters are automatically smoothed by the control in order to prevent machine overload and avoid triggering watchdog monitors unnecessarily. Thread cutting> Spindle functions Tool and process monitoring system> PROFIBUS tool and process monitoring 'Detect errors before they happen'. This is the motto for our SINUMERIK 840D powerline, a control-integrated tool and process monitoring system. Active power monitoring functions keep an eye on such things as breakage, wear, and missing tools. Precise operating status recognition and process optimization are also possible. Tool carrier with orientation capability
Kinematics type T 
Kinematics type M 
Kinematics type P For machine tools, which have tool carriers with settable tool orientation, the user of a SINUMERIK control can freely configure these kinematics without using 5-axis transformation. The "tool carrier with orientation capability" functionality enables 2?-D/3-D machining with permanent spatial orientation of the tool/workpiece table. Vectors l1 to l4 represent the geometrical dimensions of the machine. The rotary axes need not move in parallel to the Cartesian axes, but instead can be inclined at any angle (e.g. cardan milling head with 45° inclination). The angles ?1 and ?2 can be either specified or computed from the active frame and assigned to the tool carrier with orientation capability or to the workpiece table. The following kinematics can be configured flexibly:
Tool change via T numberIn chain, rotary-plate and box magazines, a tool change normally takes place in two stages: A T command locates the tool in the magazine, and an M command inserts it in the spindle. In circular magazines on turning machines, the T command carries out the entire tool change, that is, locates and inserts the tool. The tool change mode can be set using machine data. Tool identification systems (option)Within the framework of the tool loading and unloading dialog in the Siemens tool management system for SINUMERIK 810D powerline/ 840D powerline with HMI-Advanced, you are provided with a link to an automatic tool identification system. This allows you to replace manual input of the tool data with automatic reading and writing of the tool code carrier. During unloading, the data block for the tool is saved on the HMI-Advanced; during loading, it is read from the HMI-Advanced via the code carrier and entered in the tool management system. In the interim, the tool data can be re-edited as during tool selection from the tool catalog (offset data, etc.). Using an editable description file containing precisely defined tool and cutting data, the code carrier data are converted during loading into dialog data, which can be read by the tool management. During unloading, the dialog data are converted back into code carrier data with the aid, once again, of the description file. Tool management (option)"Tool management" ensures that at any given time the correct tool is in the correct location and that the data assigned to the tool are up to date. Tool management is used on machine tools with circular magazines, chain magazines or box magazines. It also allows fast tool changes and avoids both scrap by monitoring the tool service life and machine downtimes by using spare tools. The most important functions of tool management are:
HMI-Advanced, the most user-friendly and most sophisticated configuration, makes it possible to utilize the tool management function to the limit of its capability, but HMI-Embedded also provides you with the most essential task-related functions. Missing tools can be loaded based on a decision made by the operator. Tools with similar wear characteristics can be combined into wear groups. Tool management also takes tool length compensations for adapters that are permanently mounted at certain magazine locations and fitted with different tools into account. With MCIS TDI, the SINUMERIK 810D powerline/840D powerline with HMI-Advanced provides an upgrade to its tool management function which includes such things as tool balance and an online link to a tool presetting station. Tool offsets
Tool offsets By programming a T function (5-figure integer number) in the block, you can select the tool. Every T number can be assigned up to 12 cutting edges (D addresses). The number of tools to be managed in the control is set at the configuration stage. A tool offset block comprises 25 parameters, e.g.:
The wear and the tool base dimension are added to the corresponding offset. When writing the program, you need not take tool dimensions such as cutter diameter, cutter position or tool length into account. You program the workpiece dimensions directly, following the production drawing, for example. When a workpiece is produced, the tool paths, depending on the relevant tool geometry, are controlled so that the programmed contour can be produced with every tool used. You enter the tool data separately in the control's tool table, and in the program you call only the required tool with its offset data. During program execution, the control fetches the required offset data from the tool files and corrects the tool path for various tools automatically. Tool offset D can be programmed with reference to tool number T (when the Siemens tool management is active, e.g., with monitoring functions and management of sister tools) or without internal references to existing tools. You can define as many as 32,000 D values per control. D numbers can be freely assigned, checked, renamed, ascertained with the associated T number, invalidated, and activated on a site-dependent basis during programming. Tool offsets, grinding-specific> Grinding wheel surface speed Grinding-specific tool offsets are available (minimum wheel radius, maximum speed, maximum surface speed, etc.). When a cutting edge is created for grinding tools (tool type 400 to 499), these are stored automatically for the tool in question. Tool types are: 400: Surface grinding wheel 401: Surface grinding wheel with monitoring 403: Surface grinding wheel with monitoring and without tool base dimensions for grinding wheel surface speed 410: Facing wheel 411: Facing wheel with monitoring 413: Facing wheel with monitoring and without tool base dimensions for grinding wheel surface speed 490 - 499 Dressers With the TMON command, you can activate geometry and speed monitoring for grinding tools (type 400 to 499) in the CNC part program. Monitoring remains active until deactivated in the part program with TMOF. The current wheel radius and the current wheel width are monitored. The speed setpoint monitoring is monitored cyclically in relation to the speed limit value, taking into consideration the spindle override. The speed limit value is the smaller of the values resulting from comparison of the maximum speed with the speed computed from the maximum grinding wheel surface speed and the current wheel radius. Tool orientation interpolation> Transformation, generic Interpolations of tool orientations supplement generic transformation: The tool orientation can be programmed in a plane as large circle interpolation (ORIPLAN program command), on the outside surface of a taper in the clockwise or counterclockwise direction (ORICONCW/ORICONCCW), or even with free definition of the tool curve orientation (ORICURVE). Tool radius compensation
KONT for behind the contour 
Bypassing the outside corners with transition circle/transition ellipse When "tool radius compensation" is activated, the controller automatically computes the equidistant tool paths for different tools. To do so, it requires the tool number T, the tool offset number D (with cutting edge number), the machining direction G41/G42, and the relevant working plane G17 to G19. The path is corrected in the programmed level depending on the selected tool radius. You can match the approach and retract paths to the required contour profile or rough-part forms, for example:
In the part program it is also possible to select the strategy with which the outside corners of the contour are to be bypassed:
For soft approach to/retraction from the contour, i.e., tangential approach and retraction irrespective of the position of the starting point, various strategies are available: Approach and retract from left or right, on a straight line, on a quadrant or semicircle, in space or in the plane. The controller automatically adds a circle or straight line to the block with the "Tool radius compensation" if no point of intersection is possible with the previous block. Compensation mode with the "Tool radius correction" may only be interrupted by a certain number of successive blocks or M functions which do not contain motion commands or positional data in the compensation level. This number of successive blocks (or M commands) can be set using machine data (standard 3, max. 5). 3D tool radius compensation (option)Inclined surfaces can be machined with 3D tool compensation or tool compensation in space. The 3D tool compensation function enables contour milling and face milling with a defined path. The inclined tool clamping position on the machine can be entered and compensated. The control computes the resulting positions and movement automatically. The radius of a cylindrical milling cutter at the tool insertion point is included in the calculation. The insertion depth of a cylindrical milling cutter can be programmed. The milling cutter can be turned not only in the X, Y and Z planes, but also by the lead or hitch angle and the side angle. Tool types
Geometry of turning tool 
Geometry of slotting saw The tool type determines the geometry specifications required for the tool offset memory, and how they are to be used. Entries are made for the relevant tool type in tool parameter DP. The control combines these individual components to produce a result variable (e.g., total length, total radius). The relevant overall dimension goes into effect when the offset memory is activated. The use of these values in the axes is determined by the tool type and current machining plane G17, G18 or G19. The following tool types can be parameterized: Group 1xy: milling cutters (from spherical head cutter to bevel cutter) Group 2xy: drills (from twist drill to reamer) Group 4xy: grinding tools (from surface grinding wheel to dresser) Group 5xy: turning tools (from roughing tool to threading tool) Group 700: slotting saw The saving of all tool offsets is supported by input screens. For wood, the "slotting saw" tool is available as tool type. Transformation package Handling (option)
Transformation package Handling The "transformation package for handling devices" contains the so-called standard transformation block, with whose help typical 2-axis to 5-axis handling devices such as gantries or SCARAs can be operated. This coordinate transformation package converts the axis-specific actual values for the axes (e.g., A1 to A4) into Cartesian values (e.g., X, Y, Z, A) and the programmed Cartesian setpoints back into axis-specific values for the handling devices. Thanks to this coordinate transformation, the movements of the handling device become simpler and more user-friendly. The handling device can be set up, that is, manually traversed not only in the axis-specific coordinate system, but also in the handling device's own Cartesian coordinate system, using, for example, the jog keys on the handheld programming unit. Adaptation of the respective kinematics is carried out via machine data. A 6-axis transformation for defined applications is also available (please consult your local Siemens sales office). Transformation, genericThe function "Generic transformation" is used to define any tool orientation in the space with the initial setting of the axes, and not just according to the Z-direction. It can then be used much more flexibly and universally. It is then possible to also control machine kinematics by the CNC where the orientation of the rotary axes is not exactly parallel to the linear axes. Starting with software release 6 (SINUMERIK 840D powerline), the generic 5-axis transformation was extended to the 3-axis and/or 4-axis transformation, i.e. it is also possible for machines with only one rotary axis (rotatable tool or workpiece). TRANSMIT/peripheral surface transformation (option)
Face machining with TRANSMIT 
Tool-center-point path through the pole The "TRANSMIT" function is used for milling external contours on turned parts, e.g. square parts (linear axis with rotary axis). As a result, programs become much more simple and complete machining increases machine efficiency. Turning and milling can be performed on one machine without rechucking. 3D interpolation with two linear axes and one rotary axis is possible. The two linear axes are mutually perpendicular and the rotary axis lies at right angles to one of the linear axes. "TRANSMIT" can be called up in different channels simultaneously. The function can be selected and deselected with a preparatory function (straight line, helix, polynomial and activating tool radius compensation) in the part program or MDA. With TRANSMIT, the area of the transformation pole is reached when the tool center can be positioned at least to the turning center of the rotary axis entering the transformation. TRANSMIT through the pole is implemented in different ways:
Peripheral "surface transformation" is used on turning machines and milling machines, and enables peripheral surface transformation, e.g., for turned parts. The TRACYL peripheral surface transformation or cylinder surface transformation can be used to manufacture grooves of any shape on the surface of cylindrical bodies with or without groove side offset. The shape of the grooves is programmed in reference to the plane cylinder surface processed. Travel to fixed stop (option)With this function, tailstocks or sleeves, for example, can be traversed to a fixed stop in order to clamp workpieces. The pressure applied can be defined in the part program. Several axes can be traversed to a fixed stop simultaneously and while other axes are traversing. The "extended travel to fixed stop" function can be used to adapt torque or force on a modal or block-related basis, travel with limited torque/limited force (force control, FOC) can be initiated, or synchronous actions can be used at any time to program traversing functions. Traversing rangeThe range of values for the traversing ranges depends on the selected computational resolution. The following ranges of values can be programmed when the default value is specified in the machine data field "computational resolution specified in the table for linear or angular position" (1,000 increments per mm or degree):
If the computational resolution is increased/decreased by a factor of 10, then the value ranges change accordingly. The traversing range can be restricted by software limit switches and operating ranges. Universal interpolator NURBSInternal motion control and path interpolation are performed using NURBS (non-uniform rational B splines). This provides a uniform method for all internal interpolations that can also be used for future complex interpolation tasks. The following input formats are available irrespective of the internal structure: Linear, circular, helical, involute interpolation, splines (A, B, C) and polynomials. User interfaceThe user interface has a clear layout with 8 horizontal and 8 vertical softkeys. The targeted use of Windows-type technology permits simple and user-friendly operation of the machine. The interface is subdivided into 6 operating areas:
In this way, it is possible, for example, to create another part program while parts production is in progress and to transfer data from an external storage unit at the same time. On changing the operating area, the last active menu is always stored. There are two hotkeys for switching between operating areas. User interface expansionThe "user interface expansion" functionality allows SINUMERIK users to design their own user interfaces to visualize either machine-manufacturer or end-user functional expansions or simply their own screen form layouts. User environments configured by Siemens or non-Siemens machine manufacturers can be modified or replaced. This function is implemented via an integrated interpreter and via configuring files containing the description of the user interface. The interpreter is available for HMI-Advanced, HMI-Embedded, ManualTurn, ShopMill, ShopTurn and HT 6. The screen forms can be designed directly on the control itself. A graphic tool is required to create graphics and pictures. Part programs can be processed with newly created user interfaces. Configuring examples for new screen forms, which can also be used as the basis for the user's own new screen forms, can be found in the supplied toolbox. You can implement the following functions with "expand user interface":
With the integrated editor, even the basic version of the user interface can be expanded at predefined softkeys by up to 20 pictures (more than 20 pictures with OA copy license). User machine dataThe NCK makes machine data available for configuring the PLC user program. These user machine data are stored in the NCK-PLC interface during control power-up, prior to PLC power-up. The PLC basic program reads these data from the NCK-PLC interface during its initialization phase. This means that specific machine configurations, machine expansions and user options can be activated. Variables and arithmetic parametersUsing variables in place of constant values permits the development of flexible programs. Variables make it possible to respond to signals, e.g. measured values. If variables are used as a setpoint value, the same program can be used for different geometries. Variable types
Variable types
VelocityThe maximum path and axis velocity and spindle speed are affected by the machine and drive dynamic response and the limit frequency of actual-value acquisition (encoder limit frequency and limit frequency of the input circuit). The resulting velocity from the programmed path lengths in the CNC block and interpolation cycle (IPO cycle) is always limited to the maximum velocity or, in the case of short path lengths, reduced to the velocity that can be travelled during one IPO cycle. The minimum velocity must not go below 10-3 units/IPO cycle. The minimum and maximum axis velocities are dependent on the selected computational resolution. The maximum velocity of the axis is generally limited by the mechanics or by the limit frequency of the encoder or actual-value acquisition. The velocity value range is not limited by the CNC (max. 300 m/s). Vibration extinction VIBXThe function is implemented as a loadable compile cycle and supports the axis-specific damping of machine vibrations. Up to 8 axes can be parameterized in the CNC, each with two machine data for the filter frequency and the required damping factor. Work offsets> Frame concept 
Coordinate system ?According to DIN 66217, clockwise, rectangular (Cartesian) coordinate systems are used in machine tools. The following coordinate systems are defined:
Thus, you use work offsets to transform your machine zero point into the workpiece zero point in order to simplify programming. You can choose from among various work offsets:
Working area limitation> Work offsets Working area limitations describe the area in which machining is permitted. These limitations refer to the basic coordinate system. A watchdog checks to see whether the tool tip has penetrated the protected working area (also taking into account the tool radius). One value pair (plus/minus) per axis may be used to describe the protected working area. The upper and lower working area limits, which can be set and activated via setting data, may be modified using the G25/G26 commands. Working area limitations restrict the traversing range of the axes in addition to the limit switches. Protective zones are thus set up in which tool movements are prohibited and which protect equipment such as tool revolvers, measuring stations, etc., from damage. Working plane> Tool radius compensation When specifying the working plane in which the desired contour is to be machined, the following functions are defined at the same time:
When calling the tool path correction G41/G42, the working plane must be defined so that the control can correct the tool length and radius. In the basic setting, the working plane G17 (X/Y) is preset for drilling/milling, and G18 (Z/X) for turning.
|
||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||||
| Каталог 2018 | Каталог 2017 | Каталог 2016 | Каталог 2015 | Каталог 2014 | Каталог 2013 | Каталог 2012 | Сертификат | Контакты | Карта сайта | Поиск |