Showing results for 
Search instead for 
Do you mean 
Reply
Solved! Go to solution

CAM MCS change & options

I think it's a bug ... or a bad setting.

 

If you have generated operations in one group and later change the MCS for the whole group, its not recognised as “change”. When trying to generate whole group again, it gives you the “warning” that paths are already up to date and not needed to be generated. And the operations are not generated. I don’t think this is a good “solution”??

You can go to settings and choose “force generate”, so there is no warning. But that’s not the same.

 

2nd. Is it possible somewhere to make the settings, that e.g. when selecting MCS e.g. “inferred” would stay at next selection. Or the least used would be remembered at next time?

 

3rd. Good function in “Fixed contour” => Area Milling Drive Method, where you can select “Method => Steep and Non-steep.

Would it be possible to add “Connection” options (e.g. Ramp on part, stagger ramp on part) in “Steep Cutting”? It would be very useful.

 

Best

Opl.

NX 10.0.3.5

7 REPLIES

Re: CAM MCS change & options

Changing the MCS does not need a path regenerate, since the path is usually independent from the MCS, it is only used to map the positions for output.

 

Some things are related to the MCS, like cut levels in level based operations like cavity and z-level milling, which need to be regenerated.

 

For the rest it is best to create enhancement requests at GTAC and post them here to allow others to request being added to the ER, so it gets more weight.

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: NX11.0 EAP, NX12.0 EAP

How to Get the Most from Your Signature in the Community

Re: CAM MCS change & options

MCS is important since it’s the origin for the program/operations (in the group) when post-processing the operations.

If you generate toolpath with different MCS (e.g. origin) … as it should be (or changed) and post-process the operations … well you will have the problem… the operations will be wrong.

Re: CAM MCS change & options

[ Edited ]

The MCS is not influencing the internal tool path, it will just tell the post-processor the origin compared to the absolute origin the internal tool path is located in.

 

The position values of the internal tool path are always in absolute origin, the post-processor will get positions transformed by the MCS to convert them to NC code.

 

Moving an operation from one MCS to another is not changing the tool path, just its location.

 

Changing the MCS is more like using a different preset on the machine, the tool path is the same the location is different.

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: NX11.0 EAP, NX12.0 EAP

How to Get the Most from Your Signature in the Community

Re: CAM MCS change & options

Stephan is correct but there are times when the path will need to be regenerated.  Tool axis vector changes or clearence height changes would warrent an updated toolpath.  

Jeff Sauers, Lead CNC Programmer, Oberg Industries

Production: NX 10.0.3.5, Vericut 8.0


Re: CAM MCS change & options

We need to know what the differences between the two MCS are!

 

A difference in origin coordinates does not trigger an operation to get invalid, which is correct.

A difference in orientation of the CSYS axis is applicable for the operation to be marked as invalid.

A different tool axis will have to mark an operation as invalid too.

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: NX11.0 EAP, NX12.0 EAP

How to Get the Most from Your Signature in the Community
Solution
Solution
Accepted by topic author opl
‎01-27-2016 04:42 AM

Re: CAM MCS change & options

If you are only changing the MCS CSYS, there is no need to regenerate the path. The status should change to repost.

 

To see this, list your tool path, change the MCS, and list your tool path again - you will see different coordinates.

Mark Rief
Retired Siemens

Re: CAM MCS change & options

Hay

 

@Mark Rief

Yes it’s true if you move the MCS, you do not need to re-generate operation for post-processing.

 

Best

Opl

Learn online





Solution Information