Acceleration characteristic, knee-shaped

SINUMERIK 802S base line

When operating stepper drives, it is necessary to reduce the acceleration above a certain speed to utilize the motor characteristic of stepper motors optimally. Path and single-axis interpolations can then be performed taking into account the specific acceleration curve of stepper drives. The acceleration can be reduced linearly or hyperbolically. By utilizing the steeper characteristic in the lower speed range, an optimum start/stop response can be obtained for the stepper motor at these low speeds.

The axis dynamics is also optimized for the Look Ahead function. When the stepper motor characteristic is utilized in this manner for rapid traverse movements, non-productive time is reduced.

The knee-shaped acceleration characteristic is also effective in setup mode, with superimposed motion and in the case of threads.

Acceleration with jerk limitation

SINUMERIK 802D

To 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 Security

Access to programs, data and functions is protected in a user-oriented hierarchical system of 8 access levels.

These are subdivided into 4 password levels (protection level 0 to 3) for Siemens, machine manufacturer and end user.

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 1 to 3 are preprogrammed by default through Siemens.

Access rights for protection levels 4 to 7 can be altered by the machine manufacturer or end user.

Actual-value system for workpiece

The term "actual-value system for workpiece" is used to designate functions, which allow the SINUMERIK user to:

• begin machining in a workpiece coordinate system defined via machine data in JOG and AUTOMATIC mode without any additional manipulations after powering up the control
• retain the valid settings relating to active level, settable frames (G54-G59), kinematic transformations, and active tool compensation at the end of the part program for use in the next part program
• toggle between the workpiece coordinate system and the machine coordinate system
• change the workpiece coordinate system (e.g., by changing the settable frames or tool offset)

Alarms and messages

All "alarms and messages" are output on the operator panel in plain text with a graphic symbol indicating the clear criterion. The alarm texts are stored on the control.

"Alarms and messages" from the machine can be displayed in plain text from the PLC program. A distinction is made between status messages and error messages. Whereas the display of a status message is immediately deleted when the condition is no longer active, error messages must always be acknowledged.

The control's response to alarms or messages is configurable, and the required texts are stored on the control.

"Alarms and messages" in the part program: Messages can be programmed to give the user information on the current processing status while the program is executing.

Analog spindles

Unipolar or bipolar 10 V interfaces can be operated.

Auxiliary function output

Auxiliary function output informs the PLC when the part program wants the PLC to handle certain machine switching 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:

• Tool selection T
• Tool offset
• Feed F/FA
• Spindle speed S
• H functions (for SINUMERIK 802D/802D base line only)
• M functions

Auxiliary function output may be carried out either with velocity reduction and PLC acknowledgement up to the next block, or before and during travel without velocity reduction and without block change delay. Following blocks are then retracted without a time-out.

Axes/spindles

> Spindle functions

• Axes
  Three of the four simultaneously operating axes are interpolating axes.
• Spindles
  Spindle drives can be speed-controlled or position-controlled.

SINUMERIK 802S base line/802C base line

In SINUMERIK 802S base line/802C base line, the encoder evaluation functions are integrated in the control module.

SINUMERIK 802D/802D base line

In SINUMERIK 802D/802D base line, the encoder evaluation functions are located in the digital drive modules of the SIMODRIVE 611 universal E HRS.

Backlash compensation

With positive backlash (normal case), the encoder actual value is ahead of the true actual value (table): The table does not travel far enough.

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.

Backlash compensation is always active in all modes following reference point approach.

Block search

The block search function allows any point in the part program to be selected, at which machining must start or be continued. The function is provided for the purpose of testing part programs or continuing machining after a program abort.

You have a choice of 3 different search options:

• Block search with calculation at the contour:
  During the block search, the same calculations are executed as during normal program operation. The target block is then traversed true-to-contour until the end position is reached. Using this function it is possible to approach the contour again from any situation.
• Block search with calculation at the block end point:
  this function allows you to approach a target position (such as tool change position). All calculations are also executed here as during normal program operation. The end point of the target block or the next programmed position is approached using the method of interpolation valid in the target block.
• Block search without calculation:
  This method is used for high-speed searches in the main program. No calculations are carried out during the search. The values stored in the control remain the same as they were before the block search.

For a CNC program to execute without errors, the target block must be included as relevant block information.

You can specify the search destination by:

• Directly positioning the cursor on the destination block
• Specifying a block number, a jump label, any character string, a program name, or a line number.

Circle via center point and end point

Circular interpolation causes the tool to move along a circular path in a clockwise or counter-clockwise direction. The required circle is described by:

• Starting point of circular path (actual position in the block before the circle)
• Direction of rotation of circle
• Circle end position (target defined in circular block)
• Circle center

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 point

If 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, the intermediate point, and the end point.

Clamping monitoring

> Position monitoring, standstill monitoring

SINUMERIK 802D/802D base line

"Clamping monitoring" is one of the 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, the clamping monitor replaces the standstill monitor, 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.

CNC program messages

> Alarms and messages

CNC user memory

All programs and data, such as part programs, subprograms, comments, tool offsets, work offsets and program user data can be stored in the shared, battery-backed CNC user memory.

Contour definition programming

"Contour definition programming" enables fast input of simple contours.

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 monitoring

SINUMERIK 802C base line/802D/802D base line

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.

Cycle support

> Technology cycles

Data backup

The following data backup procedures are available to you for system software and user data:

• Integrated FEPROM
• Serial RS-232-C interface
• PC card (for SINUMERIK 802D/802D base line only).

Diagnostics functions

For service purposes, a self-diagnostics program and testing aids have been integrated in the controls. The status of the following is displayed on the operator panel:

• Interface signals between the CNC and the PLC and between the PLC and the machine
• Variables
• PLC bit memories, timers and counters
• PLC inputs and outputs

For testing purposes, signal combinations can be set for the output signals, input signals, and bit memories. Alarms and messages also offer useful diagnostic information. In the "service display" menu, it is possible to call up important information about the axis and spindle drives, such as:

• Absolute position value (for SINUMERIK 802C base line/802D/802D base line only)
• Position setpoint
• Following error (for SINUMERIK 802C base line/802D/802D base line only)
• Speed setpoint
• Actual speed value

Dimensions metric/inches

Depending 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):

• Position data X, Y, Z, etc.
• Interpolation parameters I, J, K and circle radius CR
• Pitch

SINUMERIK 802D/802D base line

• Programmable work offset (TRANS)
• Polar radius RP

With the G700/G710 programming expansion, all feedrates are also interpreted in the programmed measuring system (inch/min or mm/min). In the "Machine" operating area, you can switch back and forth between inch and metric dimensional notation using a softkey.

Display functions

All current information can be displayed on the operator panel's screen, such as:

• Block currently being executed
• Previous and following block
• Actual position value, difference between setpoint and actual value (for SINUMERIK 802C base line/802D/802D base line only)
• Current feedrate
• Spindle speed
• G functions
• Auxiliary functions
• Workpiece designation
• Main program name
• Subprogram name
• All data entered, such as part programs, user data and machine data
• Help texts

Important operating states are displayed in plain text, for example

• Alarms and messages
• Position not reached (for SINUMERIK 802C base line/802D/802D base line only)
• Feed stop
• Program in progress
• Data input/output in progress

Drives

SINUMERIK 802S base line

The SINUMERIK 802S base line has an interface for frequency signals and direction signals for activating power units for stepper motors. Up to three stepper motor power units can be controlled.

SINUMERIK 802C base line

The SINUMERIK 802C base line offers ±10 V interfaces to the SIMODRIVE 611 base line and SIMODRIVE 611 universal HRS converter systems.

SINUMERIK 802D/802D base line

The SINUMERIK 802D/802D base line is equipped with a PROFIBUS interface for the SIMODRIVE 611 universal E HRS converter system.

Electronic handwheels

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 500 kHz.

Execution of large CNC programs

Part programs that are too large for CNC memory can be read in via the RS-232-C interface and executed while the read-in is in progress. The CNC executes the program from circulating buffer. Part programs are automatically reloaded into circulating buffer as soon as free memory space becomes available.

Feedforward control

SINUMERIK 802D/802D base line

Using 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.

For compensation of contour violations, the SINUMERIK 802D/802D base line features velocity-dependent speed feedforward control.

Feedrate override

The programmed velocity is overridden by the current velocity setting via the machine control panel or by the PLC.

0 to 200% for SINUMERIK 802D/802D base line and
0 to 120% for SINUMERIK 802S base line/802C base line.

Follow-up mode

SINUMERIK 802C base line/802D/802D base line

If 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. A new reference-point procedure for the axes is not required when follow-up mode is cancelled.

Frame concept

SINUMERIK 802D/802D base line

With the Frame concept, it is possible to transform rectangular coordinate systems very simply by translating, rotating, scaling and mirroring The following instructions are used to program these options:

• TRANS programmable work offset
• ROT rotation in space or in a plane
• SCALE scaling (scale factor)
• MIRROR mirroring

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
• AROT
• ASCALE
• AMIRROR

If swiveling tools or workpieces are available, machining can be extremely flexible.

Helical interpolation

Helical interpolation: Thread milling with form cutter

SINUMERIK 802S base line/802C base line/802D

The helical interpolation function is ideal for machining internal and external threads using form milling cutters and for milling lubrication grooves. The helix comprises two movements:

• Circular movement in one plane
• Linear movement perpendicular to this plane

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.

High-level CNC language

To meet the various technological demands of modern machine tools, a CNC high-level language has been implemented in SINUMERIK 802D/802D base line and SINUMERIK 802S base line/802C base line that provides a high degree of programming freedom.

Indirect programming (SINUMERIK 802D/802D base line)

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.

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:

• Sine, cosine, tangent
• Arc sine, arc cosine, arc tangent (SINUMERIK 802D/802D base line only)
• Square root
• Absolute value
• Power of 2 (square) (SINUMERIK 802D/802D base line only)
• Integer component
• Round to integer
• Natural logarithm (SINUMERIK 802D/802D base line only)
• Exponential function (SINUMERIK 802D/802D base line only)
• Shift (SINUMERIK 802D/802D base line only)
• Rotation (SINUMERIK 802D/802D base line only)
• Scale change (SINUMERIK 802D/802D base line only)
• Mirroring (SINUMERIK 802D/802D base line only)

Comparison operations and logic combinations

Comparison operations with variables can be used to formulate jump conditions. The comparison functions that can be used are:

• Equal to, not equal to
• Greater than, less than
• Greater than or equal to
• Less than or equal to
• String concatenation (for SINUMERIK 802D/802D base line only)

The following logic combinations are available (for SINUMERIK 802D/802D base line only): AND, OR, NOT, XOR (eXclusive OR). These logic operations can also be performed bit by bit.

I/O interfacing via PROFIBUS DP

SINUMERIK 802D/802D base line

PROFIBUS DP represents the protocol profile for distributed I/Os. It supports extremely fast cyclic communication for data volumes with 12 Mbit/s. The advantages of PROFIBUS DP are also maintained when data is transferred for both I/O and drives: high availability, data integrity and standard message structure.

Intermediate blocks for 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).

Languages/language expansions

The user interface for the SINUMERIK controls is available in almost every required language. The user interface can be switched between two languages when online.

Leadscrew error compensation / measuring system error compensation

The principle of "indirect measuring" on CNC-controlled machines is based on the assumption that the leadscrew pitch 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 situation). 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 caused by the measuring system as well as its installation tolerances on the machine (so-called measuring system errors), plus any machine-dependent 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.

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.

SINUMERIK 802D/802D base line

A second pair of plus/minus software limit switches can be activated via the PLC.

Linear interpolation

SINUMERIK 802D

Up to 4 axes can interpolate linearly.

SINUMERIK 802S base line/802C base line

Up to 3 axes can interpolate linearly.

SINUMERIK 802D base line

Up to 2 axes can interpolate linearly.

Look Ahead

During the machining of complex contours, most of the program blocks describe very short paths and often feature 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.

"Look Ahead" enables the optimum machining velocity to be achieved. 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.

Measuring system error compensation

> Leadscrew error compensation / measuring system error compensation

Monitoring functions

The 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:

• Read in
• Format
• Encoder and drive
• Contour
• Position
• Standstill
• Clamping
• Speed setpoint
• Actual velocity
• Enabling signals
• Voltage
• Temperatures
• Microprocessors
• Serial interfaces
• Transfer between CNC and PLC
• System memory and user memory

Monitoring of tool life and workpiece count (option)

SINUMERIK 802D

This function supports monitoring of the tool life and/or workpiece count. If the life of a cutting edge times out during machining, an alarm is output and a VDI signal transmitted. Tool life monitoring is carried out for the active cutting edge of the loaded tool. Monitoring of the workpiece count registers all the tool edges that are used to produce a workpiece.

Online ISO dialect interpreter

SINUMERIK 802D

With the online ISO dialect interpreter, part programs in other ISO dialects such as G codes from other manufacturers can be read into, edited and processed in the SINUMERIK 802D. Part programs can also be written in the normal manner. G290/G291 can be used to also swap between the two programming languages within a part program.

Operating modes

In the "Machine" operating area, you have a choice of three operating modes:

• JOG
  JOG mode is intended for the manual movement of axes and spindles as well as for setting up the machine. The set-up functions are reference point approach, repositioning, traveling with the handwheel or in the predefined incremental mode, and redefinition of control zero (preset/set actual value).
• MDI
  In MDI mode, you can enter individual program blocks or sequences of blocks, then execute them immediately via CNC Start. The tested blocks can then be saved in part programs.
• AUTO
  In AUTO mode, your part programs are executed automatically once they have been selected from the workpiece, part program or subprogram directories (normal operation). During AUTO mode it is possible to generate and correct another part program.
  The Teach-in submode (with SINUMERIK 802S base line/802C base line only) allows you to transfer motion sequences to the AUTO program by travelling through positions and storing them.

In the operating modes MDI and AUTO, you can modify the sequence of a program using the following "program control" functions:

• SKP skip block
• 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 (with SINUMERIK 802D/802D base line only)
• M01 Programmed stop
• PRT Program test

Part program management

Part programs can be organized according to workpieces. This permits clear allocation of programs and data to the respective workpieces.

PLC remote diagnostics

SINUMERIK 802D/802D base line

This function allows you to monitor your PLC program online, and to transfer the PLC program from the control to a PLC and vice-versa. A modem-to-modem link via the fixed-line network or mobile telephone network is used.

PLC status

In its "diagnostics" area, the user interface allows you to check and/or change PLC status signals.

This allows you to do the following on site without a programming device:

• Check the input and output signals from the PLC's I/Os
• Perform troubleshooting
• Check interface signals for diagnostic purposes

The status of the following data items can be displayed separately on the operator panel:

• Interface signals from/to the machine control panel
• NCK/PLC and MMC/PLC interface signals
• Data blocks, bit memories, timers, counters, inputs and outputs

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 memory

The PLC user program, the user data and the basic PLC program are stored together in the PLC user memory.

Polar coordinates

SINUMERIK 802D/802D base line

When programming 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.

Position monitoring

To protect the machine, SINUMERIK controls provide extensive mechanisms for axis monitoring:

• Motion monitoring:
  Contour monitoring, position monitoring, standstill monitoring, clamping monitoring, speed setpoint monitoring, actual speed monitoring, encoder monitoring
• Monitoring of static limitations:
  limit switch monitoring, working area limiting (for SINUMERIK 802D/802D base line only)

Position control monitoring is always activated after motion blocks have been terminated due to setpoints (for SINUMERIK 802C base line/802D/802D base line only). 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 (SINUMERIK 802D/802D base line only) as well as for position-controlled spindles.

Programmable acceleration

SINUMERIK 802D/802D base line

With the "programmable acceleration" function it is possible, for example, 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 maximum acceleration value stored in the control is not exceeded. 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 language

The CNC programming language is based on DIN 66025.

Reference point approach

When 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.

SINUMERIK 802D/802D base line

Reference point approach for an axis with absolute value encoders is carried out automatically when the control is switched on (without axis motion) if the corresponding axis is recognized as being calibrated.

Repos

Following 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.

Returning to the contour is possible manually in JOG mode using the axis and direction keys. It is not possible to overshoot the interruption point; the feedrate override switch is effective.

Rotary axis, turning endlessly

SINUMERIK 802D/802D base line

Depending on the application, the working area of a rotary axis can be limited via a software limit 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).

Serial interface (RS 232 C)

A serial interface (RS-232-C) is provided for data input/output. 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 startup

In order to transfer a specific configuration as easily as possible to other controls on the same type of machine, you can create so-called series startup files.

Series machine startup is then extremely easy and user-friendly, and can even be accomplished without a programming device by using an IBM-compatible PC.

SINUMERIK 802S base line/802C base line

Simply link two ECUs via the RS-232-C interface and transfer all data (MD, MPF, LEC, etc.) directly from one control to the other to achieve a completely identical control.

SINUMERIK 802D/802D base line

Store a startup file on PC card in the control, plug the PC card into the next control, and start series machine startup there.

Skip blocks

CNC blocks that are not to be executed in every program run, 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.

Spindle functions

Spindle speed

• Analog (± 10 V)
• Digital (SINUMERIK 802D/802D base line only)

Spindle override 0 to 200% (120% for SINUMERIK 802S base line/802C base line);
gear stages preset via:

• Part program (commands M41 to M45)
• Automatically via programmed spindle speed (M40) or
• Oriented spindle stop (positioning mode) with SPOS ¹⁾

Spindle monitoring with the functions ¹⁾

• Axis/spindle stationary (n < n_min)
• Spindle in set range
• Max. spindle speed
• Programmable lower (G25) and upper (G26) spindle speed limitation
• Min./max. speed of the gear stage
• Max. encoder limit frequency
• End point monitoring for SPOS

Constant cutting speed with G96 (in m/min or inch/min) at the tool tip for uniform turning finish and thus better surface quality.

Thread cutting with constant pitch:¹⁾

With G33 you can produce the following thread types: Cylindrical, taper and face threads, single-start or multiple-start, as left-hand or right-hand threads. In addition, multiple-block threads can be produced by concatenating threading blocks.

Tapping with compensating chuck/rigid tapping:

When tapping with compensating chuck (G63), the compensating chuck equalizes differences between spindle movement and drilling axis. A prerequisite for rigid tapping (G331/G332) is a position-controlled spindle with position measuring system.

The traversing range of the drilling axis is therefore not restricted. By using the method whereby the spindle, as a rotary axis, and the drilling axis interpolate, threads can be cut to a precise final drilling depth (e.g., for blind hole threads).

1) Prerequisite: Positional actual-value encoder (measuring system) with corresponding resolution (mounted directly on the spindle).

Spindle speed limitation

> Spindle functions

Standstill monitoring

SINUMERIK 802C base line/802D/802D base line

The standstill monitor checks whether the axis moves further out of its position than the value specified as standstill tolerance in the machine data. 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.

Subprograms

If 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).

Seven subprogram levels are possible in a main program with the SINUMERIK 802D/802D base line and 4 with the SINUMERIK 802S base line/802C base line. Subprograms can be completely protected against unauthorized readouts and displays (cycles). A main program can also be called from within another main program or subprogram.

Tapping with compensating chuck/rigid tapping

> Spindle functions

Teach In

SINUMERIK 802S base line/802C base line

"Teach-in" is generally taken to mean the transfer of current positions to the CNC program.

When teaching-in in AUTOMATIC 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 to the desired positions from the MCP or handwheel 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.

Technology cycles

For frequently repeated machining tasks, technology cycles (standard cycles) are available for the drilling/milling and turning technologies. You can store these technology cycles together with your user cycles in the control as protected subprograms. The parameters are set via graphically supported input screen forms in plain text.

Thread cutting

> Spindle functions

Tool change via T number

In 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. You can preselect the tool changeover mode with machine data.

Tool offsets

Tool offsets

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.

For programming a T function (for SINUMERIK 802D/802D base line: 5-digit integer, for SINUMERIK 802S base line/802C base line: 2-digit integer) the tool is selected in the block. Each T number can be assigned a corresponding tool offset (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.:

• Tool type
• Up to 3 tool length offset values
• Radius compensation
• Wear dimension for length and radius
• Tool base dimension

The wear and the tool base dimension are added to the corresponding offset.

Tool radius compensation

Bypassing the outside corners with transition circle/transition ellipse

When tool radius compensation is enabled, the control 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 two axes depending on the selected tool radius.

The control can also automatically insert a circle or a straight line in the block with the tool radius compensation when no intersection with the previous block is possible.

The offset process of tool radius compensation may be interrupted only by a certain number of successive blocks or M commands containing no motion commands or positional data in the compensating plane.

Tool types

Example: Geometry of turning tool

The tool type determines the geometry specifications required for the tool offset memory, and how they are to be used. The control combines these geometric data into a result value (e.g. total length, total radius).

The calculated 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 5xy: turning tools (from roughing tool to threading tool)

The saving of all tool data is supported by input screens.

Travel to fixed stop (option)

SINUMERIK 802D

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. "Travel to fixed stop" is possible simultaneously for several axes, and parallel to the movement of other axes.

SINUMERIK 802C base line

See function: SIMODRIVE 611.

Traversing range

The range of values for the traversing ranges depends on the selected computational resolution. The default value for "computational resolution for linear or angle positions" in the machine data (1000 increments per mm or per degree) can be used to program the value ranges (see table). The traversing range can be restricted by software limit switches and operating ranges.

User interface

SINUMERIK 802S base line/802C base line

The user interface is divided into five operating areas:

• Machine
• Parameters
• Program
• Services
• Diagnostics

This means that in parallel with part machining, for example, another part program can be created. On changing the operating area, the last active menu is always stored. Five horizontal softkeys and the window system permit simple and user-friendly operation of the machine.

SINUMERIK 802D/802D base line

The user interface is divided into six operating areas:

• Machine
• Offset/Parameters
• Program Manager
• Program Editor
• System
• Alarm
• Custom

This means that in parallel with part machining, for example, another part program can be created.

On changing the operating area, the last active menu is always stored. "Hot keys" are provided for switching from one operating area to another. Eight horizontal and eight vertical softkeys and the window system permit simple and user-friendly operation of the machine.

User machine data

The NCK makes machine data available for configuring the CNC. These data make it possible to activate specific machine configurations, machine expansions, and user "options".

Velocity

The maximum path/axis velocities as well as spindle speed are influenced by the dynamic response of the drive and machine and the limit frequency of the actual-value acquisition system.

The minimum velocity must not fall below 10^-3 units/IPO cycle.

The maximum velocity of the axis is generally limited by the mechanics or by the limit frequency of the encoder.

Work offsets

You can define work offsets, which can then be called in the part programs.

Working area limitation

> Work offsets

SINUMERIK 802D

In addition to the limit switches, "working area limitations" limit the traversing range of the axes. 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.

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.