Creating an outer layer with specified thickness.

[nkamins]

Hi, I am somewhat of a novice with Creo so I apologize for any deficiencies. I am using creo 2.0 and essentially what I want is an outer layer of my current model. So I have a complex model and would like the same shape but extending from the outer surface to, let's say, 1 inch beyond that. If there is not a method of doing this directly, I could make a scaled up version of my model and then "subtract" my model from that. But I don't know how to cut a part from another part. Is there a method of getting this outer skin that I am looking for? Thanks.

[DeanLong · Accepted solution]

A couple ways you could do that.

1. Create a Copy/Paste of the Solid Geometry by setting the Filter (lower right corner) to Geometry. Pick on your part so it highlights a face, then right click and select Solid Surfaces. Then do a Copy/Paste (Cntr C, Cntr V). Then set the filter to Quilt, pick the copy and offset it the distance you want. Then Solidify that offset. Then use Solidify again, only this time you are going to use your first copied quilt at the original size as a remove material. You should get a "hollow" solid part part".

2. Scale your model to the offset size you want, they use Shell at the thickness you want. This method is quickest, but it assumes all the geometry can shell and offset properly.

[nkamins]

Dean, I appreciate the response and the level of detail. I tried method #1, and looked over the "as a remove material" in the last step. Was confused but when I caught it, it worked like a charm. Thanks!

Edit: Follow up: on my actual part, the offset fails. Are certain parts not adequately suited for offset operations?

[Patriot_1776]

Yes.  If surfaces get inverted or eliminated, or if a curve radius goes to zero, it will fail.  There are any number of reasons for failure, ESPECIALLY if you're offsetting it a large distance like an inch.  You MAY be able to offset some of the surfaces, and patch it together.

[DeanLong]

Typically if something fails to offset it just means something in its geometry went to mathematical zero (became degenerate) or inverted. Stated simply, a 1.0mm inner radius cannot offset 2.0mm. But, Creo has gotten better over the years with ignoring the degenerate surface(s) and then extending and trimming the adjacent surfaces during the offset. It doesn't do it successfully in every instance but most times it will.

If you across that situation again you can copy surfaces individually without the failing feature(s), extend the boundaries, merge them and stitch it all back together, then solidify.

Glad I could help