Cancel
Showing results for 
Search instead for 
Did you mean: 

Tool Compensation in Variable contour (Mill-turn)

Solution Partner Creator Solution Partner Creator
Solution Partner Creator

Hi,

 

I need help on how to input tool compensation in this process

 

 

I already change the machine control but still the output is same.

 

 

Thank you in advance.

 

tool_compensation.JPG

 

Hope you can help me .  Thanks

 

 

13 REPLIES

Re: Tool Compensation in Variable contour (Mill-turn)

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

You can use UDE "Cutter Compensation". In this case, on CNC controller you must set tool diameter to zero and use only "tool wear" for compensation.

 

Marek Pawlus, NCmatic

Production: NX 11.0.2
Development: C#, Tcl/Tk, CSE

Re: Tool Compensation in Variable contour (Mill-turn)

Solution Partner Creator Solution Partner Creator
Solution Partner Creator

cutter.JPG

 

 

Hi Marek,

 

Are you talking about this in machine control?

 

Thanks for replying.

 

regards,

 

Joy

 

 

Re: Tool Compensation in Variable contour (Mill-turn)

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

Yes, this is the UDE to add in NX.

But it is importatnt to remember that toolpath is not generated with "contact contour output".

That is why on real machine controller, tool should have diameter set to zero (or to tool wear value)

Marek Pawlus, NCmatic

Production: NX 11.0.2
Development: C#, Tcl/Tk, CSE

Re: Tool Compensation in Variable contour (Mill-turn)

Solution Partner Creator Solution Partner Creator
Solution Partner Creator
but the NC data is still the same with no cutterm compensation machine control set up

Re: Tool Compensation in Variable contour (Mill-turn)

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom
Yes, coordinates will not change. You should only get extra G41/G42 or RR RL commands to activate compensation. That is what I mean, that you will not achieve "contact contour output".
But still you are able to use cutter compensation.

If you didn't get G41/G42 in your NC output - ask author of your postprocessor. It should work with OOTB postprocessors.
Marek Pawlus, NCmatic

Production: NX 11.0.2
Development: C#, Tcl/Tk, CSE

Re: Tool Compensation in Variable contour (Mill-turn)

Solution Partner Creator Solution Partner Creator
Solution Partner Creator
Hi Marek,

There was no G41/42 in NC output.

I'll ask the author of the post-processor.

Thank you so much,

regards,

Joy

Re: Tool Compensation in Variable contour (Mill-turn)

Pioneer
Pioneer

Excuse me and my English (may be I not understand it..).... How you can use Tool Radius Compensation for multi-axis milling!? I know, it possible, but - you must to use 3D-compensation, and postprocessor must to output more complex then just G40\41\42.... It not so easy, I did it for Siemens, MAZAK, Heid.

Re: Tool Compensation in Variable contour (Mill-turn)

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

As you already mentioned Mazak, you can check G41.5/G42.5

 

mazak_cutcom.jpg

Marek Pawlus, NCmatic

Production: NX 11.0.2
Development: C#, Tcl/Tk, CSE

Re: Tool Compensation in Variable contour (Mill-turn)

Pioneer
Pioneer

No. For Mazak-ISO I did it like

X[-1.66+[#820*[0.0155980]+#821*[0.2215462]]+[#825*[-0.9907477]]] Y[-6.692+[#820*[0.0858307]+#821*[0.9751499]]+[#825*[0.1357155]]] Z[250.+[#820*[-0.0000076]+#821*[-0.0001062]]+[#825*[0.0004555]]] B89.974 C167.2
X[-1.838+[#820*[0.0197264]+#821*[0.2683858]]+[#825*[-0.9830375]]] Y[-5.329+[#820*[0.0849835]+#821*[0.9633115]]+[#825*[0.1834022]]] Z[250.001+[#820*[-0.0000006]+#821*[-0.0000458]]+[#825*[0.0008935]]] B89.949 C164.432
X[-1.945+[#820*[0.0237431]+#821*[0.3138884]]+[#825*[-0.9732021]]] Y[-3.963+[#820*[0.0839406]+#821*[0.9494599]]+[#825*[0.2299475]]] Z[250.001+[#820*[0.0000035]+#821*[-0.0000183]]+[#825*[0.0013316]]] B89.924 C161.706

Learn online





Solution Information