Swept Cut in an assembly 1

[mechycontrols]

Hello all,

First time posting here. I've got an assembly that I need to make a profiled cut on a flat surface (think of using a mill to cut a pattern no a surface). I need to include a radius at the bottom of this cut. Problem is, 'Swept Cut' is not available when you're in an assembly. Mind you, I'm not trying to add any material to the assembly, just trying to add a radius to the profile of the cut.

I did a search for 'Swept Cut' in assemblies, and found this closed thread: thread559-107328 (from a while back), but no real solution.

Any suggestions?

Thanks in advance!!!

 

[handleman]

I believe you're out of luck on this one. Why can you not do it in the part?

 

[mechycontrols]

The assembly is one that is brazed together, and this feature is going in after the brazing process. I can put them into the part and use a configuration, but I'd rather do it as it will happen in the real world.

 

[rfus]

You could create this profile and path as a sketch in the assembly, and then you will have to use edit part on each part you want to cut, convert the sketch entities from your assembly sketch, and perform the swept cut with the converted path/profile on each part. All parts will have in context relations to the assembly sketch, so if you update that assem sketch and rebuild, the swept cuts in each part will update.

Be careful though, if you create the assembly sketch with relations to parts, but then edit the parts and cut places you used for the relations, you have essentially created circular refs.

RFUS

 

[bvanhiel]

Another potential solution: instead of assembling the parts into an assembly, insert them into a part. Then you have all the part operations available to you.

-b

 

[Luca83]

Create a new part in context to the assembly, create your sweep, exit out back to assembly mode, and edit in context the part you want to remove material from in the assembly, go to Insert>Features>Cavity (one of those "forgotten" commands), pick the sweep in the design features dialouge box, it should have removed material from the solid body.

This is essecially like performing a boolean subtract in assembly mode but without consuming the body it referenced, so just hide the sweep when your through.

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[CorBlimeyLimey]

If the sweep path consists of straights and radii, you could do a series of Extrude-Cuts and Revolve-Cuts.

 

[mechycontrols]

Thanks all for your responses,

We came to the same conclusion as CorBlimeyLimey: used a series of Extrude-Cuts & Revolve-Cuts. Ended up creating five features (1 Plane & 4 Cuts) to get the job done.