[allenp]

1) bug report: when you add different tool diameter for specific tool (to work with two diameters in G41), the G code will make an error in first line of new toolpath creation for second radius adding
DXX before lowering tool in position. instead of:
G01 Z-1
you will get
G01 D1 Z-1


2) how to make/obtain machine simulation file for haas vf2 tr?

[imachining-6061]

It's a misplaced compensation call in your post processor . Check your gpp file for compensation calls.

For machine simulation there is already a lot of posts here ! Do a search!

[allenp]

sorry but i did search entering
solidcam machine simulation

but the search results were less than satisfactory so can you please point out to which earlier posts can i refer to?
it only says that you must make an assembly yourself which is impossible for me right now.

[allenp]

yes it is but i feel like it isn't shown in the gpp file, I mean, like some code is missing from it, I've checked out the entire post and the only place I feel like this bug might be is here:

@compensation
; Handle setting of Diameter Compensation Gcode
; We not use this procedure to output code
; We create our own procedure for this so that we..
; have can control placement during @line,@arc
if side eq COMP_LEFT then
iDiametercomp = 41
if bDiameterCompOutputD
change(iDiameteroffset) = true
endif
endif
if side eq COMP_RIGHT then
iDiametercomp = 42
if bDiameterCompOutputD
change(iDiameteroffset) = true
endif
endif
if side eq COMP_OFF then
iDiametercomp = 40
change(iDiameteroffset) = false
endif
endp

@usr_compensation_output
; Handle output of Diameter Compensation Gcode
if change(iDiametercomp)
if iDiametercomp eq 40 or !bDiameterCompOutputD
{'G'iDiametercomp' '}
else
{'G'iDiametercomp, ' D'tool_number''}
endif
endif
endp

;-------------------

but I don't see the culprit.

also I've tried turning on trace mode for postprocessing and found nothing, but here's the whole story so you can see it for yourself:
Sendvid - Instant video upload

please any hint would be helpful, I need to use this post as it perfectly suits my needs for now, but this little bug is so annoying and most of the time I am using at least 2 tool diameters.

[partur]

You must change the varitable tool_number on d_offset

before:

@usr_compensation_output
; Handle output of Diameter Compensation Gcode
if change(iDiametercomp)
if iDiametercomp eq 40 or !bDiameterCompOutputD
{'G'iDiametercomp' '}
else
{'G'iDiametercomp, ' D'tool_number''}
endif
endif
endp

after:

@usr_compensation_output
; Handle output of Diameter Compensation Gcode
if change(iDiametercomp)
if iDiametercomp eq 40 or !bDiameterCompOutputD
{'G'iDiametercomp' '}
else
{'G'iDiametercomp, ' D'd_offset''} ;<-- line to change
endif
endif
endp

the same problem will be at the G43 Hxx. Here is a new variable h_offset. But it will not solve all the problems with automatic correction H. When creating a T-slot operation, we can choose two adjustments for both sides of the saw, but postprocessor does not print the correct G code. If this is also a problem for you, I can write how to fix it.

Enjoy

[imachining-6061]

1) bug report: when you add different tool diameter for specific tool (to work with two diameters in G41), the G code will make an error in first line of new toolpath creation for second radius adding
DXX before lowering tool in position. instead of:
G01 Z-1
you will get
G01 D1 Z-1

@usr_rapid
; Handle output for Rapid Move (G00)
; Note: XYZ not allowed together on a single line

if change(iDiameteroffset)
change(iDiameteroffset) = false
endif

if change(iDiametercomp)
change(iDiametercomp) = false
endif

Add those two if statements to your @usr_rapid function . this should correct the issue

cheers