Using a Drawing Component vs an Assembly Component in Drafting
Using a Drawing Component vs an Assembly Component in Drafting
(OP)
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
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





RE: Using a Drawing Component vs an Assembly Component in Drafting
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
RE: Using a Drawing Component vs an Assembly Component in Drafting
RE: Using a Drawing Component vs an Assembly Component in Drafting
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
RE: Using a Drawing Component vs an Assembly Component in Drafting
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.
RE: Using a Drawing Component vs an Assembly Component in Drafting
- 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
RE: Using a Drawing Component vs an Assembly Component in Drafting
-Dave
NX 9, Teamcenter 10