how do i remove external references from part file

hi everyone,
this is a rather simple question for someone who deals with assemblies on
everyday basis, but for me - I cant seem to figure it out although I
searched the help.

I've got a solidworks part file which was used in some assembly part by
someone. I need to remove the external references from it - how do I do it?
(naturally, I don't mean locking or breaking them)

thanks,
Gil

 

The only way is to manually go through the sketches and feature
definitions to remove in-context references. In sketches, use the
eyeglasses tool and sort by "defined in context", then hit the "delete
all" button. For features you'll have to redefine end conditions for
things like "up to vertex" where the vertex was from another part.

Alternately, if all you're looking to do is to create new in context
relations in a different assembly, and you're not very particular about
"best practice" type issues when they will cost you a lot of time, you
might try just going to Tools > Options > External references > Allow
multiple contexts. This is obviously not a great way to work, but
sometimes you just need to "git 'er done", and this will allow you to do
it. I've tried to get SolidWorks to make this a document property
rather than a global property, but no luck yet. I think it would make
more sense as a doc prop.

Matt

 

Simple answer: one at a time. Features using external references are
marked with "->". Go through each feature and replace with local
references.
-If the reference is an external plane, create a new one in the model.
-In sketches, you can isolate all external references in the constraint
manager and delete them. Then proceed to replace new references.

 

Thanks Matt, I seem to understand what you mean, and I'll try it on that
file I've got.

 

Thanks, you gave me a short and simple answer, which serves me well.

 

Gill,

Here is some more that kind of rolls together Matt's and Tick's answers
and adds something else.

First, in the part with external references:

1. Look for features wth the -> symbol in the feature tree.
2. Starting with the first sketch as in 1. above enter the sketch.
3. Use the Display/Delete Relationships tool from the RMB
4. From the drop down list pick Defined in Context and delete all those
references.
5. Fix missing references so that the sketch is defined.
6. Exit the sketch.
7. RMB on the sketch in the feature tree and Edit Sketch Plane
8. Make sure the sketch is referencing a sketch plane in the current
part.
9. Repeat 1 through 8 till done with the part.
Note: On step 8 you may want to reorient the first sketch so your
drawing views come out right. This may require a bit of fixing but is
worth it for consistencies sake.

Still not done yet.

Now, go into the assembly in which the part was defined.

1. Look for InPlace mates referencing the part fixed above.
2. Delete those InPlace mates.
3. Remate the part.

Now both the assembly and the part should act as if there were no
external references. Sorry, this is always going to be a manual
procedure because creating a part in context will create the first
sketch in "global space" which means the first sketch will likely not
be centered on the origin very well.

Sometimes it is a good idea to delete references and remate right after
creating the part and then continue with it with the first sketch on
the correct plane and centered.

This is a PITA just to use external references so I only create them
when I have to and I only leave them when absolutely necessary.

 

thanks TOP, for the detailed explanation, it will sure be helpful to me.
I either consider external references as a PITA mainly because I do mostly
part modeling with little assembly work or small scale assemblies only.

Gil

 

And just to be complete there are certain external references that
can't be gotten rid of easily. Mirror parts, Derived parts and Cavities
come to mind.

And to top it off there are external design tables. I haven't found a
really good way to track these.

 

Great discussion-

By default, I keep the "No External References" clicked on, in assembly
mode. In this mode, sometimes you can't "convert" faces, or edges, so I
temporarily turn it off, convert, and then switch it back on. Then I'll
immediately remove the external reference in the part file.

Best Regards,
Devon T. Sowell
www.3-ddesignsolutions.com