Cancel
Showing results for 
Search instead for 
Did you mean: 

Recognition of looping toolpathes in milling-operations

Valued Contributor
Valued Contributor

Hello! A few years ago we made an ER for recognition of looping toolpathes in milling-operations. NXCAM should detect if toolpathes are looping to give the Postprocessor a chance to output a looping-structure.

Example:

2016-01-22 12_47_25-NX 10 - Fertigung - [zyklen_test2.prt (Geändert) ].png

 

The Output of the Post could be:

 

N10960 G90 G64 X199.997 Y193. M8 M54
N10970 Z30.
N10980 ; LOOP start
N10990 R3=20. ; whole depth
N11000 R4=5. ; depth per cut
N11010 NN1:R3=R3-R4
N11020 IF R3>0 GOTOF ZZ1
N11030 R3=0
N11040 ZZ1: X199.997 Y193.
N11050 Z=-20.+R3
N11060 G1 Y190.
N11070 Y-40.
N11080 Y-43.
N11090 G0 Z=30. ; clearanceplane
N11100 X165. Y193.
N11110 Z=-20.+R3
N11120 G1 Y190.
N11130 Y-40.
N11140 Y-43.
N11150 G0 Z=30. ; clearanceplane
N11160 IF R3<>0 GOTOB NN1
N11170 M01 ; LOOP end
N11180 G0 Z30.

 

I can't believe that no other company wants to have this enhancement. In shopfloor it's pretty easy to change the toolpath if the "depth per cut" is not good because of bad material. In this case the worker only has to change the R4-Parameter. Another benefit is if you have casting-material and the oversize is different from the expected. In this case the worker only needs to change the R3-Parameter.

 

The input for the post should be the start and end of the loop and the 3 parameters as defined.

 

If anyone want's to push this ER: The ER is 1904369

 

Thanks a lot.

 

Werner

 

4 REPLIES

Re: Recognition of looping toolpathes in milling-operations

Valued Contributor
Valued Contributor

You could also only machine the floor surface and write out a loop containing the R4. If you put in a UDE you can also provide a depth per cut for instance. 

 

So writing out the loop is something you have to make in the postprocessor. But this is something you can also switch on and off with the UDE. 

W10 NX11.0.1 almost NX12.0.0.27

Re: Recognition of looping toolpathes in milling-operations

Esteemed Contributor
Esteemed Contributor

DJS wrote:

You could also only machine the floor surface and write out a loop containing the R4. If you put in a UDE you can also provide a depth per cut for instance. 

 

So writing out the loop is something you have to make in the postprocessor. But this is something you can also switch on and off with the UDE. 


Note if you do this, toolpath & cut times will be wrong, as will internal toolpath verification.

G code simulation should be correct.

If you can live with those limitations, it can be done.

Otherwise you'll have to wait for Siemens.

 

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: Recognition of looping toolpathes in milling-operations

Valued Contributor
Valued Contributor

Hello!

 

This is exactly what we do since we work with NXCAM. To work with an UDE and only create one toolpath on the floor. The cut times I have new calculated with the really number of cuts in the Post. This works correct.

 

Our problem is the IPW. If the cutlength of the milling-tool is lower than the total cutdepth we have a IPW whitch is not correct.

 

Ken, you write "you'll have to wait for Siemens". Are there plans to have a function like we want?

 

Thanks for pushing the ER Smiley Wink

 

Werner

Re: Recognition of looping toolpathes in milling-operations

Creator
Creator

This is something that I has had in my mind for a long time, my first thought was to customize the post and work with a UDE as @jobe but due to my limited knowledge about postbuilder/TCL so haven't I done it yet.

We work almost exclusively with large castings and if Siemens would make this possible so would our daily lives get a lot easier.

I will definitely push this ER!

 

 

 

Learn online





Solution Information