ST4 Sheet Metal Drawings

[Enginerd9]

I've seen a couple of threads on this topic, and I'm not sure it's ever been resolved.

I'm attempting to create a drawing (draft, in SE terms) which shows the formed AND flat "configurations" for a *.psm file.

I have an unbend feature in my tree. I have a separate file for the flat pattern. Etc.

What I don't seem to be able to do is, under the View Wizard, tell the software I want to pop in a "Flat Pattern" from the selectable options. Again, the *.psm file itself does have an unbend feature, and the file is definitely a *.psm.

Bottom line, in SolidWorks you can drop a top view twice. In one top view, you can right click, properties, select the flat configuration and it shows the SAME file in the two views... one formed, one flat. I do not seem to have that flexibility here in SE.

No problem. So I created a clean file with the flat activated... popped it into the drawing... and when I re-opened that (sorry, draft) drawing file, the flat view was gone.

What gives? All I want to do is create front, top, right side standard views with formed dimensions, then a flat pattern view off to the side. Of the same file. So no file relations are broken later. If I make my original *.psm file flat by resuming the unbend feature in the tree, it screws up my formed dimensions on the draft / drawing. (Incidentally, coming from the perspective of designing injection molded parts, draft is not the same as drawing. I see draft used to describe a drawing and I cringe. Side rant)

So. Yeah, what now?

Thanks!

If guns kill people, cars drive drunk.

 

[SvenBom]

Unbend feature is not used to create a flat sheet metal model. Unbend is used just to model some other sheet metal features more easily. After this is done, we use rebend feature to bend the sheet metal model back to the original state.
If you want to have modeled and flattened representation of the sheet metal, you must use tools/flat pattern. If your sheet metal file has flat pattern, then you can show both on the drawing.
1. create your sheet metal model as it has to be
2. click on tools menu, then in group Model select Flatten. Select one face of the model and one edge.
3. save the file
4. go to SE draft
5. when in draft wizard, you can now select designed part or flat pattern. Select one first, place the views and then go back to wizard ans select the other one.

So again, unbend feature is just for modeling and tools/flatt is for creating a flat pattern of this model.

REgards.

 

[Enginerd9]

Ah, so the trick seems to be to create the draft from the flat first, then change it to the formed after? Lemme give that a shot...

Wow. Thanks for the clarification! It seems to have worked fine. I'm accustomed to a flat pattern being sort of embedded in the feature tree under the assumption that the software knows if I've created a sheet metal part, I'll need a flat. SolidWorks does it, and surprisingly enough ProE did it too (with some help on the front end).

Anyway, thanks again! Very simple!