drawing is looking for a part that's gone.

Use SolidWorks explorer to correct the references

Kman

Tried that you get an error "you can not change file type"

I couldn't get the SW explorer to do it??????????? It won't let you change from one file type to the other.

Although it would be handy to be able to replace a drawing reference with a part (in place of an assembly), the fact is that SolidWorks does NOT allow it.

In order for you to re-associate the sheetmetal part with your existing drawing, you'll have to create a new assembly. Even if the sheetmetal part is the only component in that replacement, the drawing reference can be linked to that new assembly.

If the draw> I couldn't get the SW explorer to do it??????????? It won't let you change

The kludge fix is to make an assembly whose only component is your part, then change the reference in the drawing to the kludge assembly. Maybe if we send in enough enhancement requests we'll be able to replace assemblies with parts and vice-versa in drawings the way we can in assemblies. It took a long time for SolidWorks to allow the switch in assemblies.

Jerry Steiger Tripod Data Systems "take the garbage out, dear"

Marty,

Just for reference -

In future you may want to add extruded boss features to your sheetmetal part as representations of the PEM inserts (rather than having to manage multiple parts in an assembly).

I have been able to model such representative bosses and (even when merged to become one with the sheetmetal part's single solid body) without compromising the ability of SolidWorks to unfold it.

Per O. Hoel

Jerry, LOL this was what I ended up doing and it's ok but it's a bit annoying to me to have a sub assy when in an assembly that only has on part in it and is really only a sheetmetal part.

Thanks a bunch,

Marty

O. Hoel,

I was just sitting here thinking of a good way to do this. (Could be a better way) I have a customer that does this and I have emailed him about it. I don't have any of his files here and I can't really remember but they were some sort of a inserted feature or something like that. That way he didn't have to give it the correct heights etc.

Any thoughts???

-Marty

Marty,

I'm not sure of what you have in mind, but what I tried to describe earlier is to simply model the PEM inserts as features (boss-extrude) in place on the 3D (bent-up) sheetmetal part.

If the boss features are merged with the sheetmetal solid body, then (when flattened) they will be carried to their respective positions on the flat pattern.

If those same features are not merged, but are created as separate bodies, then they will be left in 3D space when the sheetmetal solid is flattened.

Either way, you can create a drawing of the part with a reference to ONLY the part file. There is no need for an assembly.

If you don't want the PEM bosses to show in one or more of the views of the drawing, then they can simply be selected (from within the Feature Manager of the drawing view) and specified as hidden.

H> O. Hoel,

The assembly for the drawing doesn't have to be in the actual assembly with the part. Just make a separate assembly for drawing purposes only. It's a kludge, but not a really ugly one.

Jerry Steiger Tripod Data Systems "take the garbage out, dear"