Sweeps on 3D sketches

[Legrand]

Before I put my fist through my monitor... I know this can be done, as I have done it in the past, but I'm apparently not remembering the special "trick" required.

I have created a 3D sketch, starting at the origin. I then create another sketch for my profile (a circle), again using a plane through the origin. I then hit the sweep function, pick the circle for the profile but every time I try to pick the 3D sketch as the path, nothing happens...

Any ideas?

Thanks...

 

[Heckdogg]

Legrand,

I just tried your file, but I edited the 3D Sketch, and I ran the Repair Sketch tool (Tools->Sketch Tools->Repair Sketch) on it, then tried the sweep and it worked. So something is definitly wrong with the sketch. If it's not to late, give this a try.

Good Luck

 

[TheTick]

Arrgh! This is the second time I had to type this. The site went down last time!

I tried making a composite curve of the 3D sketch, and I got an error message that the sketch was disjointed. Maybe some endpoints don't quite meet or you have a segment doubled-up.

What's with the micro-sized straight segment in the middle of your hairpin bends?

I could be the world's greatest underachiever, if I could just learn to apply myself.

http://www.EsoxRepublic.com

-SolidWorks API VB programming help

 

[TheTick]

Eureka! I found it! Delete the first segment in the 3D sketch, and there is a second segment under it.

 

[SnowCrash]

I should have remembered this from fighting with sketches before. Doubled lines is a common problem with imported geometry, too. To find and fix the double line (doppleganger?), drag to the left across each element. If there are two lines, then two will show up in the feature window list. Press "delete." Respond "yes" to one confirmation prompt, "no" to the other. Generally the first line in sequence is good, the next is the duplicate.