NX 8 modeling/drafting problem

[ducy]

Hello

I have NX 8 and I have a problem
here is the thing:
I start a new file from template, with "model template".
In file I have a e.g. solid body, for example on layer 5.
Than I make drawing of that body.
Go back to model environment.
Then make an extraction of that body on a different layer which is also no need to be active or work.
Than if I go back to the drawing (with new layer / body inactive in layer controls) I got drawing with that new body included, which is not OK of course and very irritating because all drawing made before are useless.
Also that thing happen if I import any body (instead of extracting) to the part with existing drawings, the drawings also includes that new body.

All that thing is not happening if I make new part file with "blank" from template.

Anybody know the solution to the problem?

Thank you
D.

 

[cowski]

The recommended solution is to use the "master model method", this means that your model and drawing are in separate files. The model is added as a component to the drawing file, then you can control what is shown in the drawing file with reference sets.

If you really want to keep the model and drawing in the same file, that is also supported (but not recommended). In this case you can control what is shown in views by using layers. You can use the "layer visible in view" command to control which layer(s) are shown in a given view.

www.nxjournaling.com

 

[ducy]

Thank you cowski for answer

I'm aware of using layers.
But in this case like I described, even if you put the extracted or imported model to a part, and have it on a different layer wont help. The object is displayed in drawing that you made previously.
Check by your self.

 

[cowski]

I'm running NX 8.0.1.5 and tried extracting bodies and making a drawing. I was unable to duplicate your problem. Note: when I extracted the bodies, I had the options "fix at current timestamp" checked and "use display properties of parent object" unchecked.

www.nxjournaling.com

 

[ducy]

do you have model started in "modeling" template or "blank"?

 

[cowski]

I used the siemens supplied "model" (inch) template as was mentioned in your opening post.

www.nxjournaling.com

 

[cowski]

What is the exact version of NX 8 that you are running (Help -> About NX)?

www.nxjournaling.com

 

[Toost]

Ducy,
Do you have the drawing in a separate file or not ?
- In case the drawing is a separate file, the model is a "component" and can be "layer managed", Right click the component in the assembly navigator - Properties - assembly tab - Layer option :
- Set to original layers original body resides in the drawing file on same layer as in model file and the copy etc etc.
- Set to Specified layer all objects from this model file will reside on a single layer in the drawing file.

Regards,
Tomas

 

[ducy]

Hay

Thank you all for help.

But I do know how layers work.
I do have drawing in same part as model.
I use NX for many years and this did not happen in previous versions.
I tried to duplicate this error on different machine and also get the same error. Maybe you did not follow the procedure exactly ...
My version of NX 8.0.1.5
I assume that there are some settings in file or user environment, because, like I said when using blank template, this error is not happening. But I cannot find those settings.

 

[Arkance/PhoeNX]

The problem is that the 'Model' template you are using has all the layers turned on by default. The 'Blank" template is not a template as such but a new NX part file created when you select it.
The attached image shows the layers turned on for both templates if you set the 'Show' to 'All'. Simplest way to fix is to open the template file stored in UGII\templates (model-plain-1-inch-template.prt or model-plain-1-mm-template.prt) and only activate the layers you want, then save it.
The better way is to make your own template & then create your own PAX file to point to that file. There are plenty of posts on ENG-TIPS that explain how to do that.


Anthony Galante
Technical Resource Coordinator

NX4.0.4MP10, NX5.0.6, NX6.0.5, NX7.0.1, NX7.5.0-> NX7.5.5 & NX8.0.0 -> NX8.0.2, NX8.5p21

 

[Arkance/PhoeNX]

Also when in Drafting, you should look at Format -> Layer Visible in View to set/reset the layers that are shown for the drawing sheet & views.

Anthony Galante
Technical Resource Coordinator

NX4.0.4MP10, NX5.0.6, NX6.0.5, NX7.0.1, NX7.5.0-> NX7.5.5 & NX8.0.0 -> NX8.0.2, NX8.5p21

 

[ducy]

@ namdaci45
Thank you that is the solution.
It's only "problem" that I cannot (I think) resolve the issue in parts already made in past, but OK...