tool tolerances on postbuilder Tolint and Tolext

[berri2]

Hello,

I want to put, a custom code that change with tool tolerances from NX CAM to the NC code.

For example: On NXCAM I have Tolint: 0.03 Tolext: 0.12,
if there isn't any code on postbuilder is the same I change this tolerances or not. But if is a MOM valiable or some code on the postpro,the int and out tool tolerances are change.

I think that, one MOM variable is, global mom_inside_outside_tolerances.

Which are the variables to put inside a postpro?

Thanks.

 

[berri2]

Hi,

I have added, new MOM variable and some programming.

But I don´t understand so well how it works after the post.

global mom_inside_outside_tolerances

set tol [expr $mom_inside_outside_tolerances(0)+$mom_inside_outside_tolerances(1)]
set tol [format "%.6f" $tol]
set intol [format "%.3f" $mom_inside_outside_tolerances(0)]
set outtol [format "%.3f" $mom_inside_outside_tolerances(1)]

MOM_output_literal ";------------------------------------------------- "
MOM_output_literal "; mom_inside_outside_tolerances "
MOM_output_literal ";------------------------------------------------- "

 

[cadcamnx]

hi igor

this possible !!!


depends where you would
and what if the command iTNC 530 manages def cycle 32

can only be placed in the function def cycle 32 ...

you can do so

thinning INTOL 00:12 00:03 outtol put the media in the cycle def
just pre INTOL 00:05 00:05 outtol the same thing
just INTOL 00:01 12:01 outtol also

if you want I ride for you and send you

Andre ....

I'll be online after 20:00 hours of Brazil


specialist and multi axis
development of IS & V
and postprocessors
member committee nxcam plm world
skype:andrenxcam7

 

[cadcamnx]

sorry format numerical wrong !!

specialist and multi axis
development of IS & V
and postprocessors
member committee nxcam plm world
skype:andrenxcam7

 

[markrief]

I am not sure what you are trying to do, but if you want to provide these NX CAM tolerances as variables to your CNC control, take a look at the Sinumerik 840D posts in the mach\postprocessor folder. These output the tolerances for the control to use in special cycles.


Mark Rief
Product Manager
Siemens PLM

 

[berri2]

Hi Mark,

I want to take tool tolerances, I have attached a photo before, to my CNC control, for example Heidenhain:

T0.03 tool tolerance or it can be changed to T0.01 etc.

18 TOOL CALL 4 Z S0
19 CYCL DEF 32.0 TOLERANCIA
20 CYCL DEF 32.1 T0.03
21 CYCL DEF 32.2 HSC-MODE:1 TA5

Thanks.

 

[markrief]

I want to take tool tolerances, I have attached a photo before, to my CNC control,

That is exactly what the Sinumerik posts do. For example:

...
N200 ;Intol : 0.000040
N210 ;Outtol : 0.000040
N220 ;Stock : 0.000000
N230 _camtolerance=0.000080
N240 _X_HOME=0.0 _Y_HOME=0.0 _Z_HOME=0.0
N250 _A_HOME=0 _C_HOME=0
N260 ;
N270 ;
N280 ;Operation : HSM_CYCLE832_POCKET
N290 ;
N300 TRAFOOF
N310 SUPA G0 Z=_Z_HOME D0
N320 SUPA G0 X=_X_HOME Y=_Y_HOME A=_A_HOME C=_C_HOME D2
N330 ;First Tool
N340 T="MILL"
N350 M6
N360 MSG("MILL_FINISH")
N370 TRAFOOF
N380 SUPA G0 Z=_Z_HOME D0
N390 SUPA G0 X=_X_HOME Y=_Y_HOME A=_A_HOME C=_C_HOME D2
N400 ;
N410 ;Initial Move
N420 CYCLE832(_camtolerance,1,1)
N430 TRAFOOF






Mark Rief
Product Manager
Siemens PLM

 

[berri2]

Hello Mark,

Thanks for the Siemens NC code.

I am not familiar with Siemens controls yet. I know

Heidenhain, I have added cycle32 (cycle832 Siemens) on

postbuilder for my custom post. It runs pretty well now, and

the machine doesn't goes jerky, as before without cycle 32.

Thanks.

 

[berri2]

Hi again,

I attach some heidenhain code here with cycle32.

15 TOOL CALL 2 Z S0
16 CYCL DEF 32.0 TOLERANCE
17 CYCL DEF 32.1 T0.03
18 L X32.686 Y-13.315 R0 FMAX
19 L Z2. FMAX
20 L Z-18.8 FMAX
21 L Z-25.257 M3 F250