Showing results for 
Search instead for 
Do you mean 
Reply

CSE - NX9 with custom milling tools - Heidenhain

[ Edited ]

Hello everybody,

 

I've got following problem:

 

- custom milling tool is generated
- Heidenhain PP output is correct with RL/RR

- ISV is correct
- in CSE the tool moves on the central axis through the workpiece and the contact points are ignored

 

Are there any problems with NX9 and custom milling tools?

 

Thanks!

8 REPLIES

Re: CSE - NX9 with custom milling tools

Sounds like a tracking point problem unless there is a known bug.  Maybe you can edit the tool's tracking points to something wild and see if it makes a visual difference.  If you're in INCH mode there might be a metric conversion issue for that type of tool.  I've discovered that with CYCLE800 the linear displacements are divided by 25.4 in inch mode.  So 3" becomes .1181".

 

Just a few thoughts to get you started until the Thomases check it out.

 

Good luck.

George

 

George Bennett
All NX versions
W7 Ultimate
Dell Precision M6700
Spirit of Innovation

Re: CSE - NX9 with custom milling tools - Heidenhain


VikP wrote:
- ISV is correct

- in CSE the tool moves on the central axis through the workpiece and the contact points are ignored


 

The above doesn't make sense, since CSE is the simulation engine for ISV.

Is there any error listed in the NX syslog file for the cutter compensation?

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: CSE - NX9 with custom milling tools - Heidenhain

Hi VikP,

 

do you get the radius correctin value, with getRadCorrection(), after the toolchange?

 

ThomasF

Re: CSE - NX9 with custom milling tools - Heidenhain

Hello,

 

I assume too you don't get the Radius reported/transferred to CSE.

 

Since NX903 MP1 you can check if you switch on these setting:

ISV --> Simulation Settings --> Other Options --> Use Tool Radius for Cutter Compensation

 

Does the operation have the output set correctly for

NCM --> More --> Output Contact/Tracking Data --> Contact Point

 

Which controller you are using?

 

Thomas Schulz
Siemens PLM
Manufacturing Engineering Software

Re: CSE - NX9 with custom milling tools - Heidenhain

[ Edited ]

Thank you for the commitment!

 

I use the Heidenhain iTNC Controller from NX9. 

 

This option is set:

ISV --> Simulation Settings --> Other Options --> Use Tool Radius for Cutter Compensation

 

The operation have the output set correctly for:

NCM --> More --> Output Contact/Tracking Data --> Contact Point

 

Anyway, getRadCorrection() is still zero...

Re: CSE - NX9 with custom milling tools - Heidenhain

When you wrote "custom milling tools" is that a user defined milling tool?

I am afraid these tool types do have a radius object stored int eh database, because only a contour is described.

 

Could you simply check if that is a problem of the tool?

Thomas Schulz
Siemens PLM
Manufacturing Engineering Software

Re: CSE - NX9 with custom milling tools - Heidenhain

There ist no entry of the diameter in the tool database, only in the trackpoint database.

Re: CSE - NX9 with custom milling tools - Heidenhain

Please go in contact with GTAC and file a PR, so that we can improve the system. From my view it should be possible to calculate a radius based on the defined tracking information.

 

Thomas Schulz
Siemens PLM
Manufacturing Engineering Software

Learn online





Solution Information