Magneta outline of feature in drawing mode

Not gonna "sign up" to take a gander but sounds like you've created a surface feature vs a "protrusion".

Clicked the rotatated protrusion button....maybe I'll do "solidify" just for grins.

Sorry for the need for signup....new to this whole flickr thang. This URL will show the image.

What were you doing with this "rotated protrusion" and where: if you'd created it in assembly mode to make a cut, it defaults to surface. Most of these are highly technical questions related to HOW you are making these 'copied' parts ~ what method you've employed (Copy gemometry from other model or Shrinkwrap from other model) come to mind as ways to 'reference' another part. But to avoid guessing the right (or just as often, the wrong) answer, we need to know the how you are doing this and it often doesn't hurt to know WHY ~ what's your goal, what're you trying to accomplish. Then we can tell you some good methods for getting where you're going. And they may not be the ones you originally selected. We do not want to be put in the position of going to great pains to tell you precisely how to do something dumb.

And the magenta goes away when you use the surface to create a solid through 'Edit>Solidify' or 'Edit>Thicken'. Select the quilt first, then the menu item.

Reference this:

So it seems I made a quilt. As to why I did what I did. The large part is a machined casting which gets overlaid with nitrile. I chose "create component in assembly mode" I chose "part" and "create features". At that point I created a revolved protrusion over the thin "lip" (feature on left of aforementioned picture). Then I created a extruded protrution on the bottom surface and finally the revolved protrusion on the right hand surface. That is the one that became the quilt.

The reason I created the overlay using the assembly part as reference is for expediency. I've used the same technique to create welded overlay for seats and valve discs. I've never ran into the problem with quilting until now. Funny it's only the last feature that quilted, none of the other surfaces show that.

I tried to solidify and Pro complains that it has a problem resolving the interesction of the revolved feature and the extruded feature. Thicken works but I get this "hole" in the hatching in the cross section view unless I choose .001 and then there is no cross hatching.

Thanks for the suggestions. Doug

So..if you inadvertently press the "surfaces" button in the dashboard...you make a surface...imagine.....Sorry for the waste of bandwidth

Doug

No prob. Sometimes just talkin' about it helps. I know. `;^)

I think I might know what's going on, between your descriptions and the picture, Doug. It sounds like you revolved an open cross section (i.e., the geometry didn't form a closed figure, something like revolving a U | without putting a top on it). So, while you could have made it a thin protusion right off the bat, it defaults to a surface. To create the solid you want, make sure the original cross section is closed, even if it buts up against another solid. So, if it is against another solid, you can use its edge as one side of your cross section sketch with 'Use Edge'. Alternatively, create you open, revolved surface, then, make surface copies of your solid and merge the copied surfaces with your open surface to form an enclosed quilt.

The only other thing that corresponds to the symptoms you've described is the rovolved U with separate surface geometry for the top, but which is not merged, does not form a single, merged quilt. So, while it is encloses a watertight volume, is can not be solidified because it is not a single quilt but adjacent patches. Merge the U with its top and then solidify.

To make the component show correctly in the drawing make sure that "Hidden line removal for quilts" is set to yet. The component will stay magenta unless you change the unless you change the system color for quilts to match the same color as geometry.

Bye

sorry, typo. set to yes (not yet)...