how do i remove external references from part file

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