Using a Drawing Component vs an Assembly Component in Drafting 2

[SDETERS]

We have an issue with one of our parts/drawing that got migrated from I-Deas to NX. The drawing is now no longer associated with the 3D model. So the user instead of adding the part as a component back into the drawing he added the part as a drawing view component. My Terminology may be a bit off here. What is the downside of adding the drawing view component into you drawing instead of creating the views from the assembly component?

I guess I am looking for pro's and cons to using drawing views components vs adding the part as a component and making the view from this?

Thaks

 

[Toost]

Here's a few differences that i can think of now.
A "drawing component" * will not be reported in parts lists.
A drawing component cannot (Can no longer !) be substituted/ replaced.
"derived views" works fine on drawing components but in case you want another base ( such as a TRI-view ) view you need to add the component again.
- this makes the ANT look a bit weird but has no real downside since the Drawing Comp anyway will not be reported in a partslist.
In case there are multiple D.C.'s , it can be tricky to identify which one is shown in which view. - There is no cross-highlighting
* I don't think that there is an official name/term for "drawing components". I have used the term "drawing specific component" which is kind of equivalent.

Regards,
Tomas

 

[SDETERS]

Thomas thanks for the feedback. Sounds like it is a not the end of the world. So we will keep it and move on. Have a good weekend.

 

[cowski]

In addition to what Toost mentioned:
For exploded views to work correctly, they must be created in the drawing file. If the drawing were of an assembly, exploded views and the parts list would not work correctly.

The customer defaults uses the term "drafting component", so I guess that's the official term for them. If you are using a recent version of NX with the out of the box settings, you are probably already (and unwittingly) using them. When you add a base view, NX defaults to selecting the master model file instead of the drawing file. Depending on your settings, NX may not show a "drafting component" in the navigator, even though you are using one. You can use "information -> object" then select a drawing view to see where it is being pulled from (check the reported "part name").

I asked a similar question a while back either here or at the Siemens' community site: "if you are creating a drawing of a single part (not an assembly), why bother adding it as a component of the drawing file, why not just pull in the desired view?" I can't seem to find a link to the thread right now, but I don't remember getting any sort of substantive answer.

www.nxjournaling.com

 

[SDETERS]

Cowski. thanks. For the exploded views we do not use this function. We use assembly Arrangements to display our exploded views. I feel the exploded view function does not work well for us. We have 30 or so arrangements in one of our base assemblies. Exploded views and arrangements do not play nicely with each other.
I think I remember that thread you are talking about. I will search and see if I can find it. We usually point to the model to create the views from instead of using the drawing component.

thanks again and enjoy the weekend.

 

[Toost]

"For exploded views to work correctly, they must be created in the drawing file. If the drawing were of an assembly, exploded views and the parts list would not work correctly."
- Which cannot (?) be done since the D.C.'s are invisible outside the drawing ?!?

"The customer defaults uses the term "drafting component", so I guess that's the official term for them."
- Thank's , did not know that.

/ Tomas

 

[Dave K]

About a year or so ago, I was on a call with GTAC, and the topic of views from the drawing, or views from the model came up. I was given the impression that even internally, there is some debate as to which is the better way to do it. I think the OOTB default has gone back and forth on that too.

-Dave

NX 9, Teamcenter 10