A stupid question...

OK. to preface this absurd question, I feel that I should say that the company I work for will not send any of us in engineering to a course on solidworks. This creates an interesting situation, wherin I have to ask stupid questions.

That being said, It IS possible to extrude a hole through all parts of an assembly(this I have done), and yet the cut does not translate to the individual part when open on its own. It seems to me, that the answer is very simple, and I just cant seem to find it on my own.

Likewise, it seems to me, that a cut should be able to be made in an unfolded or flat state in sheet metal, and then fold back into its finished form, with the cuts relative to the material instead of the plane.

Like I said, im sure this is painfully simple, but i really could use some help.

Thanks, Cris

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When created a cut extrude in an assy, the whole will not show up in the individual parts UNLESS you are editing the parts "In Context" of that assy. When editing In Context, you are basically editing the part while the assy is open. When you do a assy cut extrude, the hole(s) will show up when doing an assy drawing, which is what the assy cut extrude is for.

Heres something that may help.

  1. Do the assy cut extrude. After this is done, you will have the hole(s) in all of the parts you want.
  2. Next, edit each part that has the hole(s) "In context". When doing so, use the command "Convert Entities" on the hole(s) desired. After doing this, do a cut extrude on the part(s).
  3. After you have the hole(s) you want, open each part and edit the feature for that hole. You will see that feature is referencing the assy, so you have 2 choices. a) Delete the reference. After this, dimension the hole. b) Keep the part referenced. In the early design phase, I usually keep my parts referenced, but when the design is done, its best to delete reference, and dimension the features in the part itself.

Hope this helps, and isnt very confusing :)

Post back if you need more help...

Reply to
SW Monkey

When you use a feature cut in an assy, it stays there as is - it doesn't propogate back to the parts because it's not supposed to. Think of it this way. You make some parts, you weld them together, and then you drill a hole through several parts because you want to make sure the holes line up after the welding. If the holes went back into the parts as you suggest, then the piece part drawings would show a hole, and that would not be correct. Maybe that's what you really want this time, but it's the wrong approach.

Instead, you have a few options.

  1. Put the holes in each of the piece parts manually.
  2. Put the hole in one of the piece parts, and then in the others with an in-context relation to the first one.
  3. Same as 3, only use a sketch in the assy to drive the holes in all the parts.

When you put holes in a sheet metal part, there are many different ways to accomplish it. Per your direct question, you need to do an unfold, put in the holes, and then put in a refold. This will put the holes in the flat & formed configs. Do some reading on sheet metal in the help - you'll find some very good info.


Reply to
Wayne Tiffany

Depending on the type of hole you want, maybe a hole wizard, "hole series" may fit your needs. These show up in the assembly and the individual parts. You can modify them to fit. See the "elp"area


Reply to
Michael Eckstein

"Help" It must be "Beer30"


"Michael Eckstein" wrote in message news:cgoqe.1090$ snipped-for-privacy@fe06.lga...

Reply to
Michael Eckstein

Use the Hole Wizard Hole Series, as someone else said. It will put the hole to each individual part

It depends what technique you're using for this. If you use the "base flange" technique, you can put in an "unfold" feature, make the cut, then put in a "fold" feature. If you're doing the "insert bends" technique, you can put the cut between the "flatten bends" and "process bends".

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Couldnt get the hole wizard to cut through all parts either. not sure what the problem is...it worked the same as extruding a cut through the assembly. It showed up in the assembly, but not in individual parts.

Im just not a big fan of having the circles of different parts relate to each other, it makes it a pain for another engineer to play with the assembly later on, and not follow what ive done...but thanks for your help so far. Im using SW 2004...BTW

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