Redirect external references

[ztraina]

I made a part in the context of an assembly. Now I want to reuse that part in the context of a different assembly. How do i redirect the references in the part so that they point at the new assembly?

here's my specific situation:

I made a part at home in the context of an assembly. now i'm bringing the part into work, and I need to transfer it to the version of the assembly they have in the office (essentially the same assembly save file name). I expected the part to search for a new context if i removed the original, but when i get it to the office it just appends "->?" to everthing, and I never get a chance to redirect the references.


help?


help?

 

[TheTick]

Make a scratch copy where the file names match. If the assembly structures and internal ID's of the files, faces, etc. match, then the references should transfer.

"Great ideas need landing gear as well as wings."--C. D. Jackson

http://www.EsoxRepublic.com

 

[APPENG]

Basically when you create a part in context like that it references the assembly for the things that you used to help define it.

What you need to do is open the part in its own window and edit the features of the part to eliminate the external references. This will make that part stand on its own two feet (if you take my meaning)

Lets use a simple example...

I have a plate in an assembly and I created a new part in the assembly by starting a sketch on the face of the existing plate, converting the outside edges, and the holes in the plate as well. Then I extruded it to some thickness.

What we have just done is create some external references that refer to assembly for information.

1 The sketch entities have external references to the outside perimiter of the model edges, and also the edges of the holes.

2 (possibly) the sketch plane refers to a face of the plate in the assembly... (note this would only happen if we inserted the model on the origin, and then while in edit part mode, picked the face of the existing plate then opened a new sketch)

Lets say that both items 1 and 2 are true.

To get rid of the external references we would open the part and right click in the feature manager and select "List External references". This will launch a dialog box that will list every in-contect reference we have along with its status, and what type of feature it references.

Pay attention to what features, and entities are being reffered to.

Next (in the case of the above model)

We edit the features to eliminate those references.

Case 1: we edit the sketch and remove the "On Edge" relationships on all of the sketch entities. A quick way to find external relations is to use the display/delete relations tool, and set the filter up top to say "defined in context" Then delete the relations. Next we need to "rebuild" the relations in the sketch locally, by creating new relations via dimensions or geometric relations, etc.

Case 2: We need to re-define the sketch plane and use one of the system planes, or perhaps a user defined plane. to take the place of the face of the original plate we sketched on while in the assembly.

As you follow this procedure, you will notice that you will have less and less "->" signs showing. Ideally we want those to go away. Edit the part as you need to, to eliminate all of them. Now the part will stand on its own.

Hope that helps


Regards,
Jon
jgbena@yahoo.com

 

[ztraina]

Jon -

I would like to make the part "stand alone" as you said. However, the part i'm modelling is a cable that has to dynamically update based on the orientation of parts in the assembly.

If i wanted to make it independent, i think i could break all the references? but then when the assembly changes shape, the cable will not update.

 

[APPENG]

Yeah thats a bit of a problem.

What generally do in the case of "routing" things like that is to create a 3d sketch of points in context and then open that part in its own window and model the rest in there... that way the only thing in context is that sketch.

What you can try is to replace that part in the assembly. Accept the notice that you get about internal ID's and then reattach the relationships by editing the sketch's or the features in question. I certainly can be done. either way



Regards,
Jon
jgbena@yahoo.com

 

[SBaugh]

There is however one Option you might investigate. I was told by SW that this option can be very dangerous so be careful and Good luck because I have never needed or have seen a use for it.

Under Tools\Options\System Options\External References - 3rd box from the top

Allow multiple contexts for parts when editing in an assembly You can create external references to a single part from more than one assembly context. However, any individual feature or sketch within the assembly may only have one external reference.

Regards,


Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376

 

[APPENG]

Yeah I thought about that option but yes it's a bit dangerous.. not too mention after a lot of usage the tangled web of references HOY VEH!



Regards,
Jon
jgbena@yahoo.com