 |
GO2cam Pascal API
|
A post-processor is made up of two parts:
Processing of a part with a post-processor:
PARAMETER_STANDARD procedure, to manage specific parameters input.POINT, LINE, ...The interpreter processes only one file made of the following files, as listed:
TYPE used:
TR3 = array[0..2] of real;TR9 = array[0..8] of real;TC255 = array[0..254] of char;TC500 = array[0..499] of char;TC80 = array[0..79] of char;TC16 = array[0..15] of char;CONST for calling functions:
OUTPUT_NC_ : write NC blocksWRITE_NC_ : write NC statesREAD_NC_ : read NC statesREAD_PATH_ : read information on toolpath elementREAD_PART_ : read information on current cycleREAD_PROF_ : read information on profile element (can)is : test on cycle or toolpath elementPPLOAD_ : load a cycle, profile, ...util : various utilitiesREAD_DPP_ : access to DPP file parameters.SPI_GEN, SPI_CAL, SPI_LOC, SPI_FIL, SPI_WINCONST access keys and toggle values
B... TOGGLE access keyE... INTEGER access keyR... REAL access keyS... character string access keyCONST_ toggle valueA model is used to process each machining plane. This model is defined in the DPP file. It notably specifies keys used for each coordinate. It also specifies the processing carried out on coordinates, as well as the positioning mode. The model must be selected with WRITE_NC_init_plane before any utilization. A default model is selected at the beginning, according to the type of post-processor and DPP file. The default model associated to the plane can be selected: WRITE_NC_init_plane_db
WRITE_NC_init_plane, WRITE_NC_init_plane_db, TEST_change_plane, READ_PART_cycle_plane_type, READ_PART_rot_angles, READ_PART_origin_no, READ_PART_ori_coord, OUTPUT_NC_primary, OUTPUT_NC_secondaryREAD_PART_memo_plane_type, READ_NC_plane_no, READ_PART_plane_name, READ_PART_plane_no, READ_PART_plane_mat, TEST_plane_fictiv, TEST_exist_start_planePositioning on plane processing is defined in the DPP model.
READ_PART_rot_angles, READ_PART_subroutine_angles, READ_PART_rotcal_angles, OUTPUT_NC_primary, WRITE_NC_primary, READ_NC_primary, OUTPUT_NC_secondary, WRITE_NC_secondary, READ_NC_secondaryPlane origin processing is defined in the DPP model, by the plane processing type and the origin expression.
READ_PART_origin_no, READ_PART_ori_coord, WRITE_NC_origin_no, WRITE_NC_origin_coord, READ_PART_plane_ori, READ_PART_plane_ori_no, WRITE_NC_plane_origin, READ_NC_origin_validate, WRITE_NC_plane_translateInformation on coordinates processing can allow modification of cycle processing.
TEST_paxis3_orthogonal, TEST_paxis3_recalculate, TEST_pplane_recalculateThe machining plane list used by the machining operations list can be accessed by the FILE_BEGIN procedure. Warning, "imaginary" planes obtained in A/B/C Rotation subprogram do not appear in this list. Moreover, it is important to use WRITE_NC_init_plane properly, to obtain correct information.
READ_PART_plane_radius, READ_PART_plane_cone, READ_PART_inter_plane, UTIL_init_dev_decomposed, UTIL_init_dev_flank, UTIL_init_dev_shift, UTIL_init_dev_rot4, UTIL_point_dev_calculate, UTIL_calc_point_rot4, UTIL_point_dev_offset, UTIL_point_dev_flankThe subprograms are numbered according to the DPP parameters. The GO2cam subprograms occupy the first numbers. The MULTIPASSES-Z and MULTI-HOLES subprograms then follow. The subprograms will be generated according to their numbers order. The MULTIPASSES-Z subprograms can include Z movements.
Different procedures are used, according to subprogram or blocks call processing.
WRITE_NC_program_no (necessary for relative numbering).When a subprogram uses only one tool, the OPERATION_BEGIN procedure is called before the first subprogram call. This allows to output the subprogram tool call, as well as the plane positioning and spindle start. TEST_spm_call=CONST_YES (or TEST_cycle_spindle) can be tested. In this case, movements must be avoided in OPERATION_BEGIN.
The OPERATION_BEGIN procedure is also called twice at the beginning of each subprogram:
1) to properly initialize the plane and the tool. Blocks output is deactivated.
2) to generate necessary blocks
The ABC rotation subprograms use OPERATION_BEGIN between each call with TEST_plane_fictiv!=CONST_YES. The other non-decomposed subprograms use TRANSFO... procedures.
First key position after N: 6
INTERPRETER procedures called by GO2cam. The absence of a non-optional procedure will cause an error. The procedure identifier can be accessed by ICALL(PPI_CALL).
Machine Types:
Version: 5.1
Procedure called before processing PPs V5 (if it exists). In this case PARAMETER_STANDARD is only called by editing machine.
Version: 4.4
Procedure called before operations list processing to define configuration page.
Version: 4.4
Procedure called to process user actions in configuration page. Updating is automatic if this procedure is missing. When it is present, it must process all types of data (integer, real, etc.).
First procedure called after modifiers processing. Avoid NC blocks output in this procedure. It is in this procedure that the processing flags must be updated according to modifiers values.
Procedure called to split the program according to DPP parameters: number of blocks, characters, etc. This procedure can generate a special code for the DNC, or carry out a clearance and open a new file.
OUTPUT_NC_cut_programProcedure called at the beginning of each program. This procedure will output program number (ie: O0001). It will be called several times in case of 1 program per turret.
Example:
Machining operation start procedure, allowing to process the machining plane, tool change, spindle start, coolant start, etc.
Example:
Version: 6.5
Change of tool for Sister tools without changing operation. Use TEST_change_tool to make difference between new tool or replace tool.
Version: 5.5
Change of plane angles without changing operation. This procedure allows to change the rotary angles of a plane without changing operation. It will be called on hole cycles and macros with orientation change on the same sub-cycle. It will only be called if the DPP is configured for this. When it is absent, the operation is broken, meaning OPERATION_END then OPERATION_BEGIN will be called.
Version: 4.4
Operation end procedure, allowing to carry out a retraction. This procedure is called at the end of each sub-cycle, and between each A,B,C ROTATION subprogram call.
Change diameter compensation.
Change length compensation. This procedure is called for shovel tools with 2 pilot points in turning.
"Techno" cycle start procedure.
Specific techno functions processing.
Probe techno functions processing.
READ_PART_probing_touch_number, READ_PART_probing_touch_point, READ_PART_probing_touch_vector"Techno" cycle end procedure, allowing to carry out a retraction. This procedure is called at the end of each "techno" cycle.
RETURN or REWORKING techno function.
READ_PART_z_part_returnNC subprogram beginning procedure.
Procedure calling a NC subprogram.
NC subprogram end procedure.
Blocks sequence start procedure to call.
Blocks sequence call procedure.
Blocks sequence end procedure to call.
NC Rotation before a subprogram call.
READ_PART_subroutine_rotNC Translation before a subprogram call.
NC Translation and Rotation before a subprogram call.
READ_PART_subroutine_transrotNC Symmetry before a subprogram call.
READ_PART_subroutine_symNC Rescale before a subprogram call.
READ_PART_subroutine_homEDM techno parameters before a subprogram call.
READ_PART_subroutine_tecedmProgram end procedure. This procedure will output end program M code (ie: M30). It will be called several times in case of 1 program per turret.
Example:
End of NC file.
Version: 4.4
This procedure is optional. It is called after closing the ISO file. It can be present in a specific file: "pp.PPI". It can use the READ_PART_cut_file_name function. It can be used to adapt files for a customer DNC.
Canned SIMPLE DRILLING type cycle procedure (ie: G81).
Canned CHIP-BREAKING DRILLING type cycle procedure (ie: G82).
Canned DEBURRING DRILLING type cycle procedure (ie: G83).
Canned COUNTERBORING cycle procedure.
Version: 4.5
Canned reaming cycle procedure. Use INTEGER_MILL_CYCLE_NO to choose a NC cycle. The old REAMING1,2,3,4 procedures have priority when they are present to ensure compatibility.
Canned TAPPING cycle procedure (ie: G84).
Positioning, retraction or rapid approach for drilling, counterboring, tapping and reaming cycles. (POINT (MILLING-LATHE) is never called on these cycles).
Version: 5.6
Canned cycle on HOLE machining by circular Interpolation.
READ_PATH_radius, READ_PART_boolean_tec, READ_PART_integer_tec, READ_PART_real_tec, TEST_CYCLE_HOLE_TOOLPATH (MILLING-LIVETOOL)Version: 5.7
Canned cycle on HOLE Threading.
Version: 5.7
Canned cycle on HOLE back machining.
Canned cycle on milling profile. This cycle was used to generate NURBS on a SIEMENS.
Version: 4.5
Canned DRILLING, COUNTERBORING, REAMING or TAPPING cycle procedure. This procedure, if present, is called when the cycle special number (INTEGER_MILL_CYCLE_NO) is negative. This allows to perform specific processing in a customer post-processor, while preserving standard processing.
Canned CONST_CENTERING centering cycle.
READ_PATH_safety_distance, READ_PATH_altitude_return, READ_PART_drill_depth, READ_PART_dwell, READ_PATH_feedRTT_DIAMETRE_MAXI, BOOLEAN_TURN_MACHINING_DIRECTIONCanned CONST_DRILLING drilling cycle. Use BOOLEAN_TURN_DRILLING_TYPE.
READ_PATH_point, READ_PATH_safety_distance, READ_PATH_altitude_return, READ_PART_drill_depth, READ_PART_dwell, READ_PATH_feedBOOLEAN_TURN_OFFSET, BOOLEAN_TURN_MACHINING_DIRECTIONCanned pecking cycle. CONST_PECKING PP cycle. GO2cam CONST_TOOL_PECKING, CONST_SIMPLE_PECKING cycles. READ_PATH_point : with approach distance.
READ_PATH_point, READ_PATH_angle, READ_PATH_point_end, READ_PART_turn_canned_safety_dist, READ_PART_dwellBOOLEAN_TURN_MACHINING_DIRECTION, BOOLEAN_TURN_PILOTED_POINT, REAL_TURN_DWELL_DEPTH, RTT_ANGLE_PIQUAGECanned CONST_TAPPING tapping cycle. BOOLEAN_TURN_MACHINING_DIRECTION for reworking and return.
READ_PATH_point, READ_PATH_safety_distance, READ_PATH_altitude_return, READ_PART_drill_depth, READ_PATH_feedBOOLEAN_TURN_MACHINING_DIRECTIONCanned CONST_GROOVING grooving cycle. This cycle is rarely canned.
READ_PATH_point (middle of profile at maximum stock), READ_PART_profile_itn_no, READ_PART_turn_canned_depth, READ_PART_turn_canned_overlength, READ_PART_turn_canned_safety_dist, READ_PART_dwell, READ_PART_feedBOOLEAN_TURN_PILOTED_POINTS_NUMBER, BOOLEAN_TURN_PILOTED_POINT, BOOLEAN_TURN_FINISH_TYPE, BOOLEAN_TURN_TOOLPATH, BOOLEAN_TURN_ALLOWANCE_MANAGECanned CONST_PARTING parting off cycle.
READ_PATH_point, READ_PATH_point_end, READ_PART_dwellREAL_TURN_SAFETY_DISTANCE_Z, REAL_TURN_Z_ALLOWANCE, REAL_TURN_FEED_2Canned CONST_ROUGHING roughing cycle without pocket. It is the only roughing cycle that can be canned according to NCs. When the cycle contains pockets, this procedure will only be called if the pocket roughing is also canned. READ_PATH_point: maximum stock, profile reference point.
READ_PATH_point, READ_PART_profile_itn_no (1..8), READ_PART_turn_canned_depth, READ_PART_turn_canned_overlength, READ_PART_turn_canned_safety_dist, READ_PART_feed, READ_PATH_feedBOOLEAN_TURN_MACHINING_DIRECTION, BOOLEAN_TURN_TOOLPATH, BOOLEAN_TURN_OFFSET, BOOLEAN_TURN_RETRACT_TYPE, BOOLEAN_TURN_BACK_MOVE_POINT, BOOLEAN_TURN_CORNER_ROUNDING, BOOLEAN_TURN_ALLOWANCE_MANAGEPocket part of Canned CONST_ROUGHING roughing cycle. CONST_POCKET_ROUGHING PP cycle. This cycle is never canned.
READ_PATH_point, READ_PART_turn_canned_depth, READ_PART_turn_canned_overlength, READ_PART_turn_canned_safety_dist, READ_PART_feedBOOLEAN_TURN_RETRACT_TYPE, BOOLEAN_TURN_BACK_MOVE_POINTCanned parallel roughing cycle. This cycle is never canned.
READ_PATH_point, READ_PART_profile_itn_no, READ_PART_turn_canned_depth, READ_PART_turn_canned_overlength, READ_PART_turn_canned_safety_dist, READ_PART_feedBOOLEAN_TURN_MACHINING_TYPECanned CONST_THREADING threading cycle. Either a NC cycle generating all passes, or a NC cycle generating only one pass can be used (ie: G33).
READ_PART_thread_pass_nb, LOAD_thread_pass, READ_PROF_point, READ_PATH_point (approach distance included), READ_PATH_point_end (clearance distance included), READ_PATH_angle (element angle), READ_PART_turn_canned_safety_dist (only Rdsz is useful), READ_PART_turn_canned_depthBTT_TYP_PLONGEE, BOOLEAN_TURN_PULL_MACHINING, REAL_TURN_PITCH, REAL_TURN_PASS_DEPTH, REAL_TURN_CONE_LENGTH, RTT_RAPPORT_SOMMET, RTT_RAPPORT_FOND, RTT_ANGLE_FILET, INTEGER_TURN_THREADS_NUMBER, INTEGER_TURN_PASSES_NUMBER, INTEGER_TURN_EMPTY_PASSES_NUMBERCanned CONST_PROFILE_THREADING threading cycle. This cycle is on profile.
READ_PART_profile_start_point, READ_PART_profile_elt_number, LOAD_profile_eltRapid positioning (ie: G0 X10 Y0). CYCLE_DRILLING_CANCEL (MILLING-LIVETOOL) is called for drilling, counterboring, tapping, reaming milling cycles.
Example:
Rapid positioning in rotary tools.
Rapid positioning in straight or taper cut.
Rapid positioning in pocketing.
Rapid positioning in 4 axes EDM.
Output working linear movement (ie: G1 X10 Y0).
Example:
Output working linear movement for live tools.
Output working linear movement in straight or taper cutting.
Output working linear movement in EDM pocketing.
Output working linear movement in 4 axes EDM.
Output working linear movement in decomposed threading.
Version: 4.5
Output working linear movement with accelerated feed rate. This procedure is notably used for sloping grooves cycles in turning. When it is missing, LINE (MILLING-LATHE) procedure is used with the rapid feed rate machining of machine file.
Output working linear movement with accelerated feed rate for rotary tools.
Version: 5.5
LINE (MILLING-LATHE) with change on G41/G42/G40 mode. This procedure allows to enable and disable radius compensation during toolpath, elsewhere than in APPROACH_PLANE (MILLING-LATHE) or RETURN_PLANE (MILLING-LATHE). It will be called to process finishing on pocket cycles. Its absence will be reported by a message when it needs to be used.
Output working circular movement (ie: G02 X10. Y0. R 5).
Example:
Output working circular movement for live tools.
Output working circular movement in straight or taper cut.
Output working circular movement in pocketing.
Output working circular movement in 4 axes EDM.
Output working circular movement in decomposed threading.
Machining toolpath approach in 3 axes milling.
Machining toolpath approach in 3 axes for rotary tools.
Machining toolpath approach in machining plane.
READ_PATH_cutcomMachining toolpath approach in rotary tools plane.
READ_PATH_cutcomMachining toolpath approach in plunging.
Machining toolpath approach in rotary tools plunging.
Machining toolpath approach in straight or taper cut.
Machining toolpath approach in pocketing.
Machining toolpath approach in 4 axes EDM.
3 axes machining toolpath return in milling.
3 axes machining toolpath return for rotary tools.
Machining toolpath return in plane.
Machining toolpath return in plane for rotary tools.
Retraction after machining toolpath in milling.
Retraction after machining toolpath for rotary tools.
Machining toolpath return in straight or taper cut.
Machining toolpath return in pocketing.
Machining toolpath return for 4 axes EDM.
Version: 5.9
Add a synchro on toolpath. Synchro on approach, return points or between other movements.
Version: 5.5
This function is called to validate or not READ_PATH_point_5axis. This procedure is called just before OPERATION_BEGIN and after OPERATION_END. It is only called when the toolpath and DPP configuration require its use. It is only used on toolpaths with different normal vectors. It is used according to the DPP configuration (5-axis position or 5-axis canned). PPFRA_V5.LIB and PPTOUR_V5.LIB are modified to process this procedure: It activates and deactivates the LIB_MULTAX global when necessary. The procedure parameter is used for this. This global is then tested by the USINAGE_CONTINUE function, which results in the use of READ_PATH_point_5axis, OUTPUT_NC_primary, OUTPUT_NC_secondary.
Version: 4.4
Procedure allowing to authorize or not processing of a 4 axes EDM cycle, element by element, without segmentation. If this procedure is missing, the guide and part altitudes are compared. The DPP flags allow to accept arcs and to have different types of top and bottom elements always tested.
Version: 5.6
Procedure allowing to invalidate Canned processing CYCLE_HOLE_TOOLPATH (MILLING-LIVETOOL) to type of use when the DPP is canned.
Version: 5.7
Procedure allowing to invalidate Canned processing CYCLE_HOLE_THREAD (MILLING-LIVETOOL) to type of use when the DPP is canned.
Version: 5.7
Procedure allowing to invalidate Canned processing CYCLE_HOLE_BACKMACHINING (MILLING-LIVETOOL) to type of use when the DPP is canned.
Procedure allowing to invalidate Canned processing according to type of use when the DPP is canned. If this procedure is missing, the Canned is invalidated when REAL_TURN_DRILLING_DIAMETER > REAL_TOOL_DIAMETER or BTT_COTE_DECALAGE <> CONST_CENTER.
BOOLEAN_TURN_DRILLING_TYPE, BOOLEAN_TURN_PILOT_SIDE, REAL_TURN_DRILLING_DIAMETER, REAL_TOOL_DIAMETER, CYCLE_TURN_DRILLING (LATHE)Procedure allowing to invalidate Canned processing according to type of use when the DPP is canned.
Procedure allowing to invalidate Canned processing according to type of use when the DPP is canned.
Procedure allowing to invalidate Canned processing according to type of use when the DPP is canned.
READ_PART_under_axe_overcut, READ_PART_boolean_tec, CYCLE_TURN_ROUGHING (LATHE)Procedure allowing to invalidate Canned processing according to type of use when the DPP is canned.
Procedure allowing to invalidate Canned processing according to type of use when the DPP is canned.
Procedure allowing to invalidate Canned processing according to type of use when the DPP is canned.
READ_PART_integer_tec (INTEGER_TURN_THREADS_NUMBER), CYCLE_TURN_THREADING (LATHE)Procedure allowing to invalidate Canned processing according to type of use when the DPP is canned.
Version: 5.13
At the beginning of simulation, like PP_BEGIN for nc output. This procedure is called at the beginning of machine simulation. It allows to initialize parameters, like the PP_BEGIN procedure when outputting nc blocks. It also allows to position axes at the start, using PPMTE_... functions.
Version: 5.13
At the end of simulation, like PP_END for nc output. This procedure is called at the end of machine simulation. It allows to perform clearances, using PPMTE_... functions.
Version: 5.13
Before each cycle, allowing to carry out a retraction if tool or plane change. This retraction must be similar to retraction in OPERATION_BEGIN before tool call. This procedure is called at the beginning of each cycle, to perform necessary clearances when changing tool or plane. The tests are the same as in OPERATION_BEGIN, and similar movements must be generated. For this, common variables can be used.
Version: 6.01
After each cycle, allowing to carry out a retraction if tool or plane will change. This retraction must be similar to retraction in OPERATION_END. This procedure is called at the end of each cycle, to perform necessary clearances (if the tool will be changed, if the plane will change, etc.). The tests are the same as in OPERATION_END, and similar movements must be generated. For this, common variables can be used.
Version: 5.13
At the beginning of each cycle. First move after tool or rotary axis change, if necessary. This procedure is called at the beginning of each cycle. It allows to perform a first approach movement, if necessary.
Version: 5.13
Rapid positioning, like POINT (MILLING-LATHE) when outputting nc file. If this procedure does not exist, the movement is done automatically. If this procedure exists, it must output the movement. You can make some tests on specific type. This procedure performs rapid positioning, like the POINT (MILLING-LATHE) procedure when outputting nc blocks. If it is absent, the movement is generated automatically. But if it exists, it must generate the movement. It allows to perform tests and filter certain movements, such as clearances generated at program origin in database, which will be replaced by those of MTE_OPERATION_BEGIN (MTE).
Version: 5.13
Return part. It will be done automatically if this procedure does not exist. This procedure manages part return. It will be done automatically if it is absent.
Version: 5.13
Parameters:
Rework spindle moving to get part. It will be done automatically if this procedure does not exist. This procedure manages counter-spindle movements to grab the part. When there is a parting off, it is called twice, before and after it. A standard management is done if the procedure is absent.
Version: 5.13
Called on techno function, like TECHNO_FUNCTION for nc file output. You can add specific order to simulation. This procedure is called on techno functions, like the TECHNO_FUNCTION procedure when outputting nc blocks. It allows to give specific orders to the simulation.
Version: 6.08
This optional procedure is called by tooling module. You can define your own rule to define the compensation number. All the parameters used by the procedure can be modified to modify the value in the tool table in MTE.
Parameters:
int_LComp [in,out]: The current length compensation number defined for the toolint_LComp2 [in,out]: The current length compensation number 2 defined for the toolint_DComp [in,out]: The current diameter compensation number defined for the toolstr_SpecificID [in,out]: The current specific ID defined for the toolUTILMTE_ASM_tool_mounted, UTILMTE_ASM_tool_mounted_trihedral, UTILMTE_ASM_tool_mounted_cycleVersion: 6.09
This optional procedure is called by tooling module. You can define rule to put channels and block positions. All the parameters used by the procedure can be modified to modify the value in the blockaxis table in MTE.
Parameters:
zblock [in,out]: Zaxis block valuexblock [in,out]: Xaxis block valueyblock [in,out]: Yaxis block valuechannel [in,out]: channel numberchannel2 [in,out]: second channel numberFunctions called directly and which do not require use of PCALL or ICALL.
Writes NC buffer block in blocks file. Identical to PUNCHB with Itype defined by WRITE_NC_block_format. Blocks numbering is carried out according to .DPP:
POST PROCESSOR GENERALITIES
Example:
WRITE_NC_block_format, WRITE_NC_block_noSyntax: PUNCHB(Itype)
Writes NC buffer block in blocks file. Format: starting char. / block number address / block / ending char. See additional tools: dpp_punchb()
Itype values:
Example:
WRITE_NC_block_no, WRITE_NC_block_formatSyntax: GO2CAMID(Sclef)
Read constant value in RES_IPPG_GO2CAM.DAT with string value in order to use it with PCALL function.
Remark: Useful for using GO2cam parameters in a .DAT file
Example:
TRUE if an axis key is activated in progress NC block. TRUE also after function WRITE_NC_testmove.
Example:
WRITE_NC_testmove, OUTPUT_NC_paxis1, OUTPUT_NC_paxis2, OUTPUT_NC_paxis3, OUTPUT_NC_primary, OUTPUT_NC_secondaryTolerance for movement axes.
Remark: Useful for testing a real null value
This is the tolerance below which we consider that there is no movement.
Example:
WRITE_DPP_tolerppVersion: 4.4
All SPI_GEN, SPI_CAL, SPI_LOC, SPI_FIL functions can be used. See SPI documentation.
The SPI_WIN_write.. and SPI_WIN_read.. functions can also be used to manage PP parameters.
The SPI_WIN_new_panel and SPI_WIN_call_panel functions allow to display again a new input panel during execution.
SPI_WIN_new_panel** - init panel parametersSPI_WIN_write_...** - create parametersSPI_WIN_call_panel** - display panelSPI_WIN_read_...** - read parameters valuesFunctions to write into ISO file.
Functions to write NC states.
These procedures allow to complete the NC states, so as to retrieve some information later with READ_NC_... procedures. OUTPUT_NC_... procedures automatically complete the concerned NC states.
Functions to read NC states.
The PPG never directly completes the NC states: only WRITE_NC_... and OUTPUT_NC_... procedures can complete these states.
Note: However, the PPG initializes these states before the FILE_BEGIN call.
Functions to change DPP parameters.
Functions to read DPP parameters.
User dialog and display functions (old post-processors).
The INPUT functions display the question and input is made through the keyboard or, according to flag completed by PPG, they read in the .CFG file.
Tests for complementary information in DB reading.
No parameters are passed in most cases. A CONST_YES/CONST_NO toggle is recovered.
Syntax:
Read toolpath information.
The transformations linked to planes or techno subprograms have already been carried out by PPG by moving the starting point and the point in progress.
Read information about cycles, etc.
Various utilities:
Functions to load a profile in memory, in order to perform a "canned cycle" in the .PAS.
Read geometry information about profiles for canned cycles.
These functions allow the PP to write in Data Base.
Functions to read pp.CFG (old post-processors).
Functions to change PP processing.
1.10.0