Intersection Curve with Sold Body not Closed???

Instead of selecting the body, you could select individual faces and see if that helps at all. Also, just to be sure, run all the usual checks to make sure things are right, meaning Verification on Rebuild, and Tools, Check. Also, by selecting the "body" I'm assuming you mean selecting it from the solid body folder or with the bodies selection filter.

And the other obvious option is that it's just a bug.

Good luck,

Matt

Interestingly, Check reports a maximum edge gap of 0.02 mm, which sounds fairly large to me for a gap in a solid! Selecting individual faces does not change anything.

Too bad, I guess it's a bug in the Intersection Curve code. It propably does the intersection face by face, and when two faces have a tolerance small enough to be considered closed when building the solid, it doesn't recognize this and create a common point endpoint as it should, but rather creates two separate endpoints.

It's rathera annoying that the edges where the gaps appear are originally created by a Planar Surface, and just picking the existing edges as boundaries. So there is really no reason why there should be a gap in this edge... And Surface Knit accepts them as coincident without problems.

Maybe Surface Knit/Form Solid and Intersection Curves have different numerical tolerances?

/C

snipped-for-privacy@verizon.net skrev:

This is my suspicion. This, and similar inaccuracies, can cause havoc.

You might want to try making your two lofted and/or your two planar surfaces larger than needed, then trimming them to size. No guarantees, but it might help.

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

Thanks Jerry, that was actually very helpful. I made my loft a little higher, and cut off the top with a cut extrude, instead of letting it finish on the sketch plane. Intersection Curves are now closed, horray! /C

Actually, I have to say: Gosh!

Since I made the change mentioned above, my assembly rebuild times have dropped to about 20% of what they were before... (From about half a minute to 5 seconds or so!) Quite amazing, given it's exactly the same geometry!

Cool! This may be another reason why Ed Eaton suggests that you try to make lofts longer than needed and then trim them back to size. Lofts seem to be fussiest at the boundaries. By moving the edges of the real part away from the boundaries of the underlying loft, perhaps SW has an easier time calculating the intersections.

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

There are, unfortunately (grrrr...) different tolerances for different curve types. The most forgiving seems to be composite curve. When necessary (and only when neccessary, because split line has HUGE parent/child issues when editing a model) you can create a split line across your model instead of creating a plane, and use composite curve of the resulting edges to get your curve (and even convert that into a sketch if need be and it will be continous while converting just those edges into the sketch will likely not).

Fortunately, Jerry's workaround worked for you. Any reason not to resort to the uglier work-arounds is most welcome. Just thought I would add another option to your bag o' tricks for later on

Ed