cancel
Showing results for 
Search instead for 
Did you mean: 

Disable post output for some tool paths

Hello all,

 

Can we ask the post processor to not to post some of the tool paths?

 

I ask because in NX Probing (Hole Probing Operation), there's no simulation for the probe path motion. 

 

So I add some "point to point" operations into my probing operation as sub-ops to simulate how the probe actually moves. But these point-to-point operations will be read by PostBuilder and G01/G00 or G65P9810 will be output. But in reality, the probe motion will be realized by the cycle call, G65P9814. So I would like to disable the output for all those "auxiliary" point-to-point operations.

 

Thanks in advance,

 

Steph

13 REPLIES

Re: Disable post output for some tool paths

Esteemed Contributor
Esteemed Contributor

One option...

Use a # variable, set to 0 for simulation, 1 for posting (you can tell if post is being run for sim or not - I just don't remember the variable off-hand)

 

Then around each op you want to skip

IF[#1234EQ1]GOTOn

 

Depending on how you do block numbers, the may be able to be pre-computed, else you'll have to post & reproccess the posted output to figure out.

 

Ken

Ken Akerboom Sr CAx Systems Engr, Moog, Inc.
Production: NX10.0.3.5 MP5 + patch/TC11.2
I'd rather be e-steemed than e-diseaseled


Re: Disable post output for some tool paths

Hello Ken,

 

If I am not mistaking you, the code I can get from the post will be something like this

 

N1    G00 X Y Z       (move to hole pos)

N5    G01 Z F          (move to target z pos)

N10  G65P9814D  (macro for hole meas.)

N15  IF[#123EQ1] GOTO50  (simulation related)

N20  G01 X

N25  G01 X

N30  G01 X

N35  G01 Y

N40  G01 Y

N45  G01 Y

N50  G00 Z             (Retract) 

 

But what I want to do is eliminate the output of the line N15 to N45 all together, so the NC code is clean and looks like this

 

N1    G00 X Y Z       (move to hole pos)

N5    G01 Z F          (move to target z pos)

N10  G65P9814D  (macro for hole meas.)

N15  G00 Z             (Retract) 

Re: Disable post output for some tool paths

I am open to use APIs too if there's any...

 

And I am running NX9.0.3.

Re: Disable post output for some tool paths

Legend
Legend

Why APIs?
Edit your tcl-postprocessor. Create some flag when you output the cycle's call G65P9814D, and then use the condition "if { $flag}" not to output next point-to-point motions.

Re: Disable post output for some tool paths

Esteemed Contributor
Esteemed Contributor

I would add an attribute or UDE to the operations to indicate that there needs to be no output for the regular post run.

You can access operation attributes without problems in the post and they should be reliably reset for the next operation. Use the review tool to check this.

You can then use MOM_skip_handler_to_event MOM_start_of_path in the start_of_path of the P2P operation to skip the entire output of the P2P operations. You need to do some testing of what gives you the most reliable work-flow.

Stefan Pendl, Systemmanager CAx, HAIDLMAIR GmbH
Production: NX10.0.3, VERICUT 8.0, FBM, MRL 3.1.4 | TcUA 10.1 MP7 Patch 0 (10.1.7.0) | TcVis 10.1
Development: VB.NET, Tcl/Tk    Testing: NX12.0

How to Get the Most from Your Signature in the Community

Re: Disable post output for some tool paths

Genius
Genius

I think the variable that Ken is referring to is mom_post_in_simulation, I have used it before for outputting a tool change command for use in simulation but then outputting an M00 and comment to manually change the tool in the actual post because the machine did not have an automatic tool change option.

Mike Diamond, CNC Programmer, Orizon Aerostructures Inc.


Production: NX10.0.3.5, Vericut 7.4.1, ICAM V21

Development: VB.NET, Tcl/Tk Testing: NX11

Re: Disable post output for some tool paths

Thank you for your information, Stefan!

 

I am looking exactly for this. 

Re: Disable post output for some tool paths

Legend
Legend

Sinec we are on the subject of this...

 

What about getting the post to ignore Instanced or "paste with reference" toolpaths. For example I have a horizontal program to run 24 pieces of a part built with paste with reference or instanced operations. When I do a new setup I only want to post out enough to build 1 part so I can dial the setup in. Right now I open the file, save as a new name, delete everything I dont need and post it. Then when its done I delete that file so I dont have multiple files to manage.

 

NX11.0.1

Re: Disable post output for some tool paths

Esteemed Contributor
Esteemed Contributor

Have you checked with the review tool if there is any MOM variable indicating that the tool path is a reference?

Usually the variable names indicate their usage very well.

Stefan Pendl, Systemmanager CAx, HAIDLMAIR GmbH
Production: NX10.0.3, VERICUT 8.0, FBM, MRL 3.1.4 | TcUA 10.1 MP7 Patch 0 (10.1.7.0) | TcVis 10.1
Development: VB.NET, Tcl/Tk    Testing: NX12.0

How to Get the Most from Your Signature in the Community

Learn online





Solution Information