The APT source generated by the V5 Manufacturing applications is regularly enhanced to:
support new functionalities
obtain the same level of APT source generated by the Version 4 Manufacturing applications in order to ensure upward Post-Processor compatibility.
Following information applies to customers upgrading from previous V5 levels. As the current level includes all the following changes through service packs of previous releases, this information should be read carefully in order to identify modifications compared to their current CATIA level.
Special Notice Regarding Circular Interpolation
General Modifications Introduced with V5R7
General Modifications Introduced with V5R7 SP1
General Modifications Introduced with V5R7 SP5
General Modifications Introduced with V5R8 SP2
General Modifications Introduced with V5R12
General Modifications Introduced with V5R13 GA and V5R12 SP2
Axial Operation Modifications Introduced with V5R7
Axial Operation Modifications Introduced with V5R7 SP1
Axial Operation Modifications Introduced with V5R7 SP5
Axial Operation Modifications Introduced with V5R8 SP1
Axial Operation Modifications Introduced with V5R9 SP3
Lathe Machining Modifications Introduced with V5R7 SP5
Lathe Machining Modifications Introduced with V5R8 SP2
Lathe Machining Modifications Introduced with V5R8 SP5
Lathe Machining Modifications Introduced with V5R10 SP5
In Part Operation (at machine tool definition stage), Minimum and Maximum Interpolation radius values are defined for the generation of circular interpolation in APT output. These two parameters are used at two different times: at toolpath computation and at the generation of output file.
The user should check and possibly modify these values before creating Machining operations. Otherwise circular interpolation may not appear in the APT source.
Please note that if value is modified after machining operation creation and generation of toolpath, then the toolpaths should be recomputed (using Right button on Program: Compute Tool Path in Force computation mode) before generation of the output file.
1. The displacement to the tool change point is generated
before the CUTTER.
Note that the TLAXIS is also moved up.
2. Duplicate points (that is, consecutive points that have the same coordinates) must not be eliminated in the case of cycles for axial operations. In particular, it is necessary to keep these points when the approach clearance is equal to zero.
Previous Situation
RAPID
GOTO/ 0.00000, 0.00000, 0.00000
CYCLE/DRILL, 20.000000, 0.000000, 1000.000000,MMPM
CYCLE/OFFCurrent Situation
RAPID
GOTO/ 0.00000, 0.00000, 0.00000
CYCLE/DRILL, 20.000000, 0.000000, 1000.000000,MMPM
GOTO/ 0.00000, 0.00000, 0.00000
CYCLE/OFF
3. Version 4 Compatibility: TLAXIS before CATIA0.
The TLAXIS is given in the old reference axis system before CATIA0 generation.
Previous Situation
PPRINT OPERATION NAME : Machining Axis face at 0 degrees
$$*CATIA0
$$
$$ -1.00000 0.00000 0.00000 25.00000
$$ 0.00000 0.00000 1.00000 200.00000
$$ 0.00000 1.00000 0.00000 243.50000
PPRINT OPERATION NAME : Tool Change.7
TLAXIS/ 0.000000, 0.000000, 1.000000
$$ TOOLCHANGEBEGINNING
RAPIDCurrent Situation
PPRINT OPERATION NAME : Machining Axis face at 0 degrees
TLAXIS/ 0.000000, 1.000000, 0.000000
$$*CATIA0
$$
$$ -1.00000 0.00000 0.00000 25.00000
$$ 0.00000 0.00000 1.00000 200.00000
$$ 0.00000 1.00000 0.00000 243.50000
PPRINT OPERATION NAME : Tool Change.7
$$ TOOLCHANGEBEGINNING
RAPID
4. Addition of CENIT Post-processor for Lathe Machining: CENIT_LATHE.pptable.
5. New version of the CENIT Post-processor by DLL.
1. Cutter format is now exactly the same as in V4 (parameters are written with format f10.6 and positions of parameters and commas are consequently modified on the 2 lines of the statement).
2. The seventh parameter of the CUTTER statement is now valuated with the cutting length and not like before with the total length of the tool. Please note that if the cutting length is not valuated for a given tool, the seventh parameter of the CUTTER statement will be valuated with the total length.
3. GOTO format is modified from GOTO/ to
GOTO / as in V4 (2 blank characters are added between the word GOTO and
the slash).
Previous Situation
PPRINT OPERATION NAME : Tool Change.1
TLAXIS/ 0.000000, 0.000000, 1.000000
$$ TOOLCHANGEBEGINNING
RAPID
GOTO/ 0.00000, 0.00000, 100.00000
CUTTER/ 40.000000, 20.000000, 0.000000, 20.000000, 0.000000$
, 0.000000, 100.000000
TOOLNO/1, 40.000000
TPRINT/T1 End Mill D 10
LOADTL/1
PPRINT OPERATION NAME : Profile ContouringCurrent Situation
PPRINT OPERATION NAME : Tool Change.1
TLAXIS/ 0.000000, 0.000000, 1.000000
$$ TOOLCHANGEBEGINNING
RAPID
GOTO / 0.00000, 0.00000, 100.00000
CUTTER/ 40.000000, 20.000000, 0.000000, 20.000000, 0.000000,$
0.000000,100.000000
TOOLNO/1, 40.000000
TPRINT/T1 End Mill D 10
LOADTL/1
PPRINT OPERATION NAME : Profile Contouring
4. INTOL and OUTTOL statements are written before the first circular statement definition, and before other circular statements each time the discretization tolerance is modified. The discretization tolerance used to generate the INTOL statement is read on the machining operation. The value associated to the OUTTOL statement is always equal to zero.
5. AUTOPS and PSIS statements become modal, that is, the statements are generated only if the plane containing the circle is modified.
6. The point coordinates that are used to define the PSIS statement are the those of the center of the circle, and not those of the end point of the circle, as before.
7. The Circle and Cylndr statements are written exactly as in V4 (see the example below).
INTOL / 0.02500
OUTTOL/ 0.00000
PSIS/(PLANE/(POINT/ 0.00000, 0.00000, 0.68000),PERPTO,$
(VECTOR/ 0.000000, 0.000000, 1.000000))
INDIRV/ 0.47943, 0.87758, 0.00000
TLON,GOFWD/(CYLNDR/ 0.00000, 0.00000, 0.68000,$
0.00000, 0.00000, 1.00000, 3.79375),ON,$
(PLANE/PERPTO,$
(PLANE/(POINT/ 0.00000, 0.00000, 0.68000),PERPTO,$
(VECTOR/ 0.000000, 0.000000, 1.000000)),$
(POINT/ 0.00000, 0.00000, 0.68000),$
(POINT/ -3.32933, 1.81882, 0.68000))
8. New version of the CENIT Post-Processor.
1. TLAXIS instruction
Previous Situation
The TLAXIS statement is generated for each machine rotation (between ROTABL and $$*CATIA0 statements).
Coordinates of TLAXIS instruction are defined in the current axis system ($$*CATIA0).Current Situation
Coordinates of TLAXIS instruction are defined in the first axis system definition ($$*CATIA0) of the machining program. (V4 compliant)
Coordinates of rotation matrix and machining axis matrix are defined in absolute axis system. (V4 compliant)
The TLAXIS statement is generated only if the tool axis orientation is modified after a head rotation. This means that if the program only includes ROTABL instructions, there is only one TLAXIS statement at the beginning of the APT source file. (V4 compliant)
The TLAXIS are generated if no table rotation statement is defined between machining operations with different tool axis.
2. Clearance motion (at the beginning of machining operation)
If a clearance macro is defined on the machining operation, the clearance macro
motion is generated before the Approach macro motions.
Previous Situation
When no tool motion is generated by the clearance macro (example: distance motion set to 0.0), Feedrate statement (of the Clearance macro) is not generated.Current Situation
The value of Clearance feedrate (it can be set to RAPID) defined on the macro is generated at the beginning of the operation.
3. Minimum and Maximum interpolation radius defined on Machine.
Previous Situation
The minimum and maximum interpolation radius defined on the Machine are not taken into account for tool path computation of macro motions.Current Situation
The minimum and maximum interpolation radius defined on the Machine are used for all tool motions at the output file generation.
When circular interpolation is needed (depends on the machine defined on the Part Operation and/or options set for generation of APT source) CIRCLE or CYLNDR instruction is generated according to the following rule:
generation of CIRCLE instruction when circular motion axis is parallel to the Z axis of the machining axis system
generation of CYLNDR instruction in the other case.
One Rule is added for the generation of circular interpolation in order to match V4 behavior.
Previous Situation
Circular interpolation is possible even if the circular motion axis is not parallel to the tool axis and the above mentioned rule is applied.Current Situation
Circular interpolation is generated only when circular motion axis is parallel to the tool axis. Used syntax (CIRCLE or CYLNDR) will follow the above mentioned rule. If circular motion axis is not parallel to the tool axis, no circular interpolation is performed, only GOTO statements will be generated.
1. The management of point coordinates after machine rotations has been improved for APT and NC code generation and tool path replay. For APT files, the CATIA0 matrices following ROTABL statements also benefit from these improvements.
2. Duplicated points are now eliminated according to the final coordinates of the point: any transformations are taken into account.
Change made in computation of Machine Home Position parameters.
Previous Situation
%MFG_X_HOME_POS, %MFG_Y_HOME_POS and %MFG_Z_HOME_POS parameters were computed
in absolute axis system.
Current Situation
%MFG_X_HOME_POS, %MFG_Y_HOME_POS and %MFG_Z_HOME_POS parameters are computed in
current axis system (defined by last CATIA0 matrix)
1. On BoringAndChamfering, Chamfering2Sides, CounterSinking and SpotDrilling operations, computation errors on MFG_DETAIL_DEPTH and MFG_TOTAL_DEPTH parameters have been corrected.
2. Previously the MFG_PLUNGE_TIP and MFG_PLUNGE_VAL parameters were output as negative are now output as positive.
3. Previously the MFG_DWELL_TIME and MFG_DELAY_VALUE parameters were output in integer format (INT) are now output in real format (REAL).
4. The rules for cycle interruptions are modified.
Previous Situation
Operation broken down into several CYCLE instructions if
(Entry distance at point n or Exit distance at point n-1) > Approach ClearanceCurrent Situation
Operation broken down into several CYCLE instructions if
(Entry distance at point n or Exit distance at point n-1) > Approach Clearance AND > JumpDistance
5. New Parameter for CYCLE syntaxes: MFG_JUMP_DIST (Jump Distance) accessible for all axial operations.
6. Tool compensation parameters are modified for Version 4 compatibility.
Previous Situation
MFG_TL_COMP: Length number of first corrector
MFG_TL_COMP_2: Length number of second corrector
MFG_TOOL_COMP: Distance between position of first corrector and tool tip
MFG_TOOL_COMP_2: Distance between position of second corrector and tool tip.Current Situation
MFG_TOOL_COMP and MFG_TL_COMP (compatibility V4): Length number of current corrector
MFG_TOOL_COMP_1: Length number of first corrector
MFG_TOOL_COMP_2: Length number of second corrector
MFG_TOOL_COMP_DIST: Distance between current corrector position and tool tip
MFG_TOOL_COMP_DIST_1: Distance between first corrector position and tool tip
MFG_TOOL_COMP_DIST_2: Distance between second corrector position and tool tip.
7. NC compensation instructions are output in the APT file for BoringAndChamfering and Chamfering2Sides operations when the corrector length number is modified during the operation.
8. Cycle syntax can now be output for BackBoring and T-Slotting operations.
9. Linking between pattern points is now always done by horizontal paths.
10. Different Cycle syntaxes are generated when two consecutive positions do not have the same depth.
1. Machining operations using a Boring Bar tool respect the defined hole depth.
2. Tool Cutting Length is no longer used for chamfering operations (Spot Drilling, Countersinking, Boring&Chamfering, Chamfering2Sides) when Depth mode is set to 'by Diameter'. The defined diameter is now taken into account for tool path computation.
3. Correct valuation of MFG_EFFCT_DEPTH for Drilling Break Chips and Drilling Deephole operations. Note for CAA2 usage: GetEffectDepthCut method of CATIMfgAxialOperation interface returns the correct valuation.
4. New Parameters for CYCLE syntaxes:
MFG_DIAMETER (Diameter of machined hole) accessible for all axial operations.
MFG_THREAD_DIAMETER (thread diameter of machined hole) accessible for Tapping,
Reverse Threading, Thread without Tap Head, and Thread Milling operations.
MFG_BCK_BORE_VAL (Back Bore Depth) for Back Boring operation.
On Back Boring operation, tool path computation errors and invalid valuation on MFG_TOTAL_DEPTH parameter have been corrected.
1. New Parameters for CYCLE syntaxes on Circular Milling
operation
MFG_CIRCULAR_MODE: Circular mode (1: Standard / 2: Helical)
MFG_HELIX_MODE: Helix mode (1:by Pitch / 2: by Angle)
MFG_PITCH: Helix Pitch
MFG_HELIX_ANGLE: Helix angle
2. New Parameter for CYCLE syntaxes on Thread Milling operation
MFG_PITCH_WAY_OF_ROT: (1: Left hand / 2 Right hand). This new parameter
replaces the MFG_PITCH_SENS parameter.
3. New valuation of MFG_DIAMETER and MFG_THREAD_DIAMETER for Circular Milling and Thread Milling operations. Offset on contour is now taken into account for the valuation of MFG_DIAMETER and MFG_THREAD_DIAMETER parameters.
Tool Compensation distance (between P1 and current tool compensation point) is taken into account for X, Y, Z coordinates of CYCLE location points (V4 compliant).
The lathe context of Drilling and Point to Point operations is now fully managed. The lathe context is determined if the following conditions are satisfied:
A lathe machine is defined on the Part Operation.
Operation machines along the spindle axis of the lathe machine.
Operation uses a fixed tool assembly.
As a result, some modifications have been done to integrate these cases.
1. SPINDL/OFF statement is no longer automatically output after a lathe operation.
Previous Situation
PPRINT OPERATION NAME : Threading.1
$$ Start generation of : Threading.1
CYCLE/THREAD, 3.175000
CYCLE/OFF
$$ End of generation of : Threading.1
SPINDL/OFF
$$ ------ SPINDLE OFF END OF LATHE ------Current Situation
PPRINT OPERATION NAME : Threading.1
$$ Start generation of : Threading.1
CYCLE/THREAD, 3.175000
CYCLE/OFF
$$ End of generation of : Threading.1
2. A Lathe Tool Change is now automatically created before a lathe context operation instead of a Mill Tool Change.
Note: For programs created before V5R7 SP5, you must delete the previous Mill Tool Change to allow the automatic creation of a new Lathe one.
Previous Situation
PPRINT OPERATION NAME : MILL Tool Change
$$ Start generation of : MILL Tool Change
$$ TOOLCHANGEBEGINNING
RAPID
GOTO / 200.00000, 0.00000, 300.00000
CUTTER/ 25.400000, 0.000000, 12.700000, 7.332348, 30.000000,$
0.000000,228.600000
TOOLNO/4, 25.400000
TPRINT/T5 drill 1.0dia
LOADTL/4
$$ End of generation of : MILL Tool ChangeCurrent Situation
PPRINT OPERATION NAME : LATHE Tool Change
$$ Start generation of : LATHE Tool Change
$$ TOOLCHANGEBEGINNING
RAPID
GOTO / 200.00000, 0.00000, 300.00000
CUTTER/ 25.400000
TOOLNO/4,TURN
$$ End of generation of : LATHE Tool Change
3. For Drilling and Point to Point used in lathe context, the SPINDL statement output is the value of the NC_SPINDLE_LATHE NC command.
Previous Situation
PPRINT OPERATION NAME : Drilling Deep Hole along the Spindle axis
$$ Start generation of : Drilling Deep Hole along the Spindle axis
TLAXIS/ 0.000000, 0.000000, 1.000000
SPINDL/ 70.0000,RPM,CLW
RAPID
GOTO / 0.00000, 0.00000, 196.98060
CYCLE/DEEPHL, 199.947948, 5.000000
GOTO / 0.00000, 0.00000, 191.98060
CYCLE/OFF
$$ End of generation of : Drilling Deep Hole along the Spindle axisCurrent Situation
PPRINT OPERATION NAME : Drilling Deep Hole along the Spindle axis
$$ Start generation of : Drilling Deep Hole along the Spindle axis
TLAXIS/ 0.000000, 0.000000, 1.000000
SPINDL/ 70.0000,RPM
RAPID
GOTO / 0.00000, 0.00000, 196.98060
CYCLE/DEEPHL, 199.947948, 5.000000
GOTO / 0.00000, 0.00000, 191.98060
CYCLE/OFF
$$ End of generation of : Drilling Deep Hole along the Spindle axis
4. Minimum and Maximum interpolation radius defined on Machine
Previous Situation
The minimum and maximum interpolation radius defined on the Machine, are not taken into account for tool path computation of macro motions.Current Situation
The minimum and maximum interpolation radius defined on the Machine, are used for all tool motions at the output file generation.
When circular interpolation is needed (depends on the machine defined on the Part Operation and/or options set for generation of APT source) CIRCLE or CYLNDR instruction is generated according to the following rule:
generation of CIRCLE instruction when circular motion axis is parallel to the Z axis of the machining axis system
generation of CYLNDR instruction in the other case.
One Rule is added for the generation of circular interpolation in order to match V4 behavior.
Previous Situation
Circular interpolation is possible even if the circular motion axis is not parallel to the tool axis and the above mentioned rule is applied.Current Situation
Circular interpolation is generated only when circular motion axis is parallel to the tool axis. Used syntax (CIRCLE or CYLNDR) will follow the above mentioned rule. If circular motion axis is not parallel to the tool axis, no circular interpolation is performed, only GOTO statements will be generated.
1. When circular interpolation is needed, the following behavior has been modified for lathe operations to ensure compatibility with V4 behavior:
Previous Situation
2D circular interpolation is requested : No CIRCLE orders are generated.
3D circular interpolation is requested : CYLNDR orders are generated if the machining working plane is ZX. Otherwise, GOTO statements will be generated.Current Situation
2D circular interpolation is requested : CIRCLE orders are generated whatever machining working plane (ZX, XY, YZ).
3D circular interpolation is requested : CIRCLE orders are generated if the machining working plane is XY. Otherwise, CYLNDR orders are generated .Note: If machining operation is already computed, the computation must be forced to initialize the tool path.
2. TLAXIS order is no more output for lathe tool change
Previous Situation
PPRINT OPERATION NAME : Lathe Tool Change.1
$$ Start generation of : Lathe Tool Change.1
TLAXIS/ 1.000000, 0.000000, 0.000000
$$ TOOLCHANGEBEGINNING
RAPID
GOTO / 254.00000, 0.00000, 508.00000 CUTTER/ 0.400000 TOOLNO/0,TURN
$$ End of generation of : Lathe Tool Change.1Current Situation
PPRINT OPERATION NAME : Lathe Tool Change.1
$$ Start generation of : Lathe Tool Change.1
$$ TOOLCHANGEBEGINNING
RAPID
GOTO / 254.00000, 0.00000, 508.00000
CUTTER/ 0.400000
TOOLNO/0,TURN
$$ End of generation of : Lathe Tool Change.1
3. TLAXIS order is no more output for lathe operations
Previous Situation
PPRINT OPERATION NAME : Roughing.1
$$ Start generation of : Roughing.1
TLAXIS/ 1.000000, 0.000000, 0.000000
SPINDL/ 70.0000,RPM
RAPID
GOTO / 159.86681, 0.00000, 234.57181Current Situation
PPRINT OPERATION NAME : Roughing.1
$$ Start generation of : Roughing.1
SPINDL/ 70.0000,RPM
RAPID
GOTO / 159.86681, 0.00000, 234.57181
CUTTER statement has been modified to output the diameter of the insert nose according to APT definition.