Drawing assembly & views 2

[Berserk]

Hello,

I am using NX9 and I have a drawing with a model added as a component.
Whenever I try to make a base view, UG adds another component to the assembly.
Is there a way to turn this off?

Thanks!

UGNX 8 / 8.5 / 9 - Windows 7 64bit
Productive Design Services

http://www.productivedesign.com

 

[Jaydenn]

Are you sure it's adding a component?
Is it possible that it's just a link in the navigator?

The icons will be slightly different in the tree. See attached photo.

J

NX 6.0.5.3

 

[Berserk]

Yes, it looks like that.
I have other drawings that does not add those when I create views.
There must be a setting somewhere.

UGNX 8 / 8.5 / 9 - Windows 7 64bit
Productive Design Services

http://www.productivedesign.com

 

[Jaydenn]

I don't think it's a setting, but I could certainly be wrong.

I believe it has more to do with whether or not you're using the "master model concept".

If your drawing and model reside within the same file, you won't see the links in the tree.
If your model is a separate file, and your drawing a separate file, you'll see links in the tree.

You said that you "added the model as a component"; that sounds to me like you're using the master model approach. If this is true, you will see the components in the tree as you make views, etc.

J



NX 6.0.5.3

 

[cowski]

If your model is a separate file, and your drawing a separate file, you'll see links in the tree.

This is not true; you will only see the "drafting components" if you add a view from a part other than the drawing. If you do not want to use drafting components, I think there is a setting to turn it off (PhoeNX mentions it in thread561-375323, but I can't see his image as the site is blocked here).

www.nxjournaling.com

 

[Jaydenn]

Here's that setting Cowski is talking about.

NX 6.0.5.3

 

[cowski]

That's not the setting I had in mind; I thought there was one that would make base views default to the drawing file rather than the model file. I can't seem to find it now; perhaps it never existed.

I don't recommend turning off the setting shown in Jaydenn's screenshot; if you do, it will simply hide the fact that you are using a drafting component. Ultimately, you need to choose the correct part when adding a base view. The "select part" seems to default to the model part (if you are using the master model method) rather than the drawing. If you want the drawing to behave like older versions of UG/NX, make sure you have the drawing file selected when adding base views.

www.nxjournaling.com

 

[Arkance/PhoeNX]

@cowski, there is no default, it's a variable. The default is the views come from the drawing part. The variable switches it back to the model part.

Anthony Galante
Senior Support Engineer


NX3 to NX10 with almost every MR (21versions)

 

[cowski]

Which variable would that be?

The default is the views come from the drawing part.

That's not been my experience. But then again, I'm not surprised that our settings differ.

www.nxjournaling.com

 

[Arkance/PhoeNX]

Ok, the one Jaydenn refers to is what I alluded to in the other thread that Cowski has pointed to (I can't see the image, I must have forgotten to add it).

When you add a view from a model, the setting will add a drafting component if the setting is turned on.

For what I referred to Cowski previously:

From NX8.5, there was a change for what views are being selected when you have create a base view.
Pre NX8.5 views were from the drafing part.
Post NX8.5 views are from the model part.

The variable will swap that behaviour back .

Anthony Galante
Senior Support Engineer


NX3 to NX10 with almost every MR (21versions)

 

[cowski]

Ok, the one Jaydenn refers to is what I alluded to in the other thread that Cowski has pointed to

Try saying that five times fast!

The variable will swap that behaviour back .

So if I want my views to default to the drawing, what variable do I change?

www.nxjournaling.com

 

[Arkance/PhoeNX]

As always, I caveat a variable with, it works at the moment, don't be surprised if it's removed in the future.

Here's what I keep in my env file to remind what it is and does:

#Siemens' best practice recommendation for creating drawings is to create
#master model drawings. This means the master model resides in one part file
#while the drawing resides in another part file. The drawing file references
#the data in the master model file. Prior to NX 8, when a base view was added
#to the drawing, the referenced view would default to the model view from the
#current drawing file. This is counter to the master model best practice. So
#a change to the base view dialog was made in NX 8 to default to the views in
#the master model. Users should be aware of this change and understand the
#referenced views and geometry are now of the master model and not what is in
#the drawing file. If users want the pre-NX 8 behavior, they can change the
#part option to use the current drawing file and not the master model file or if
#they wish to have this as the default for the system they can set the
#environment variable:
NX_MASTER_MODEL_DWNG_DEFAULT_TO_ROOT_PART=1

Anthony Galante
Senior Support Engineer


NX3 to NX10 with almost every MR (21versions)

 

[cowski]

Good info, thanks Anthony.

www.nxjournaling.com