cancel
Showing results for 
Search instead for 
Did you mean: 

Recognizing Features Even When Configuration File is Set as cam_general.dat

Valued Contributor
Valued Contributor

Hello there,

 

I am creating operations (e.g. hole making) for my workpiece. I set both Configuration File and Template Set File as cam_general in Manufacturing Preferences. 

 

When I create the operation, I go to Specify Feature Geometry, then I select a feature (e.g. a hole). After that, the status line shows that "Recognizing Feature". Then I hit OK, and go to Machining Feature Navigator. I can find a machining feature is created there. 

 

We are using NX 10.0.3.5 MP4. I am wondering if this is new in NX 10.

 

Thanks,

Kai

4 REPLIES

Re: Recognizing Features Even When Configuration File is Set as cam_general.dat

Esteemed Contributor
Esteemed Contributor

The new drilling operations introduced with NX 9 are utilizing the same machining features as FBM does.

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: Recognizing Features Even When Configuration File is Set as cam_general.dat

Siemens Phenom Siemens Phenom
Siemens Phenom

Hi Kai,

 

You are probably experiencing the following use case:

- You change the CAM configuration using the Preference -> Manufacturing menu

- You select a feature

- You perform Create Feature Process

- The software recognizes additional features (you don't expect this as part of the Create Feature Process command).

 

The basic, as-designed, behavior is that you can use Create Feature Process (typically the command from the ribbon) to do a 1 button click workflow (find the features and create the operations for them).

 

There is an obscure (incorrect) behavior in the software where features get de-selected (only once) after you change the CAM configuration (there is a known PR for that). As a result, no features are selected and the software performs this single button process and does feature recognition first.

 

The simple workaround is to:

- Change the CAM configuration

- Start the Create Feature Process command (notice that the previously selected feature was deselected) but don't execute it yet

- Re-select the feature(s) in the Machining Feature Navigator

- Click OK on the Create Feature Process dialog

 

I hope this helps.

 

Tom van 't Erve

NX CAM Development

Re: Recognizing Features Even When Configuration File is Set as cam_general.dat

Valued Contributor
Valued Contributor

Hi Tom,

 

We are just trying to create an operation manually without FBM, but the software still tries to recognize the feature that I select in the operation as an FBM machining feature, and added a new machining feature in the Machining Feature Navigator.

 

That is basically what happened. Please see the attached video.

 

Thanks,

Kai

Re: Recognizing Features Even When Configuration File is Set as cam_general.dat

Siemens Phenom Siemens Phenom
Siemens Phenom

Kai,

 

Please ignore my previous post; I completely misunderstood what you were explaining. The AVI helped to get me back on track. The feature recognition that you see happening in the back-ground is by design !!

 

There are 3 basic Feature Based Machining workflows:

  1. "Maximum" automation: as a user, you do Find Features followed by Create Feature Process
  2. "Medium" automation: as a user, you do Find Features followed by Group Features. You than have to manually add your operations under the feature groups
  3. "Minimum" automation: here you create both your feature groups (optional hole_boss_geom) and your operations manually. But even in this last workflow all the operations from the hole_making template are still "feature based". When you select geometry, the software will first check if there already is an existing machining feature that it can re-use, if not, then it will perform feature recognition (limited to the STEPPED feature types) and it will create a feature for you if it can.

I hope that explains what you are seeing.

Note that this is independant from your CAM configuration. This is the build-in behavior for the hole_making operations.

 

Tom van 't Erve

NX CAM Development

 

Learn online





Solution Information