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Feature Recognition from STEP or IGES files with NX8

Creator
Creator

Hi,

 

I need to test for my thesis "Feature-Recognition" of some CAD-Softwares. Now I have just found in Siemens NX 8 the Feature-Recognition for CAM. Siemens NX8 detects the Features just for the CAM process but I need to change the parameters (lenght, witdth...) of the Feautures.
Feature-Recognition means for me that I open a neutral file like a 3D-STEP-file or a 3D-IGES-file and the CAD-Software finds or extracts manually or automatically the Features (Holes, Chamfer...) from the 3D-Model so that I can change the 3D-Model in the construction history.

Is there a function in NX8 which has Feature-Recognition like the way I need it?

 

In this video e.g. you can see what I mean:https://www.youtube.com/watch?v=ZsGsqijRwQE

 

Best Regards

Emre

18 REPLIES

Re: Feature Recognition from STEP or IGES files with NX8

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

Just use the "synchronous" tools in NX; they are faster and easier than whatever was happening in that video.

Re: Feature Recognition from STEP or IGES files with NX8

Siemens Phenom Siemens Phenom
Siemens Phenom

In addition to the ability to make the changes faster, the thing with feature recognition is that does not understand design intent.

 

Scott

Re: Feature Recognition from STEP or IGES files with NX8

Siemens Phenom Siemens Phenom
Siemens Phenom

As I'm sure you know, the decomposition of a given object into parameterized "features" is not unique. And the decomposition found by a recognition algorithm may or may not be suitable for the editing operation you have in mind.

 

The basic point of NX "synchronous technology" is that there is no one feature structure that's suitable for all editing operations. So, "features" should be fabricated on the fly, after you have told the system what sort of editing you want to do and what faces will be involved.

山田
yamada

Re: Feature Recognition from STEP or IGES files with NX8

Creator
Creator

I have to do a research about Feature-Recognition techniques. It does not matter if it understands the design intent. The designer has to say for what he wants to use the features!

For example I have designed a pad with 6 holes (see foto) for "company A " and save the 3D-Model as STEP to send it to "company B" which has another CAD-System. "Company B" opens the STEP-file and just see a 3D-model wich cannot be edited. So "Company B" uses Feature-Recognition technique to extract Features like holes or chamfers. After extracting you can edit the 3D-Modell as if you have constructed by yourself (but without contraints and dimensioning).
For NX8 I just want to know if it can recognize features from a STEP-file.

One foto shows the STEP-file and the other one shows the NX-Part file. After Feature-Recognition the STEP-file has approx. look like the Part-File. 

 

Re: Feature Recognition from STEP or IGES files with NX8

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

""Company B" opens the STEP-file and just see a 3D-model wich cannot be edited."

 

It seems that you have completely missed the point of the synchronous commands. With these commands, you can edit the geometry directly; it does not have to first be recognized as a particular feature type. You can operate on the topology of the model directly. Need to resize or delete one of those holes? no problem. Need to add a new hole? Copy faces from one of the existing holes or create a new one with traditional commands.

Re: Feature Recognition from STEP or IGES files with NX8

Creator
Creator

Thanks, but I really couldn't edit the diameter of my holes. I just could edit the pad. I watched some videos to understand it but if you have a good video you can post it here.

Re: Feature Recognition from STEP or IGES files with NX8

Creator
Creator

I have added a foto of the "Feature-Recognition in NX8". In NX8 it is called "Find Features" in CAM. But can I edit the Features which are found?

Re: Feature Recognition from STEP or IGES files with NX8

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

If you import geometry to NX, I'd recommend running either "heal geometry" and/or "optimize face" right away. These commands can clean up the face and edge geometry to make it easier to work with (changes are more reliable and predictable). After that, if you want to resize one of the holes, you can use the "resize face" command and directly enter the desired diameter; or you can use one of the offset functions (offset face or offset region) to resize the hole based on an offset distance. Don't like the location of the hole? use "move face" to get it in the desired place.

 

If you search this site and/or youtube, I'm sure you will find some interesting videos featuring the synchronous commands.

Highlighted

Re: Feature Recognition from STEP or IGES files with NX8

Siemens Phenom Siemens Phenom
Siemens Phenom

Emre, you can use the Resize Face command to change hole sizes. I include a short movie that has a dumb solid, I did a Resize Face and then I rename the feature to something would make sense for my use. Once I have this I can now edit this feature. That is the best part of synchronous is that it lets you control the changes. 

 

Using the NX CAM Feature recognition is used to pick the tools needed to drill the holes. I do not believe that is creating any kind of modeling feature that can be edited. 

 

Scott

 

(view in My Videos)