flat pattern dimensions SW2006 1

[mkmachine]

I've got SW2006, and I'm working with a lot of parts that are sheetmetal rolled into cylinders.
I've gotten the hang of making the parts as sheetmetal parts. Where, to layout holes I set up a reference plane at the correct angle, sketch a hole, then extrude cut to surface.
But when I make a drawing with the flat pattern, I can't get any usable dimensions from any of this.
The holes don't register as circles (they aren't). I can't get diameter dims or location dims. When I convert to a .dwg and open in autocad, the holes come out as individual curves (not circles) and I can't get dims there either.
I need to be able to make these parts in the real world! I need some help, otherwise I'm going to have to go back to acad14...
Is there any way to get dims from the parts as I describe them?
Or, do I set it up differently, and sketch on the curved surface?

thanks
mike

 

[hendersdc]

When you use this method of extrude cutting from a plane you end up with what looks like a circle from the outside but is not in a flat part, more of an elipse. To get a circle you have to flatten the bend, cut your holes, and unflatten. This way it will not be a perfect circle on the folded part but will be when it is flat.

This reflects punching or laser cutting the sheet metal, if you are going to machine these holes after the part is formed then you should make them the way you are and dimension on another view, not the flat pattern.

 

[ShaggyPE]

I recommend that you use your method with a smaller hole. Then do the unfold method hendersdc describes. Locate your correct hole centered as best you can on the "spline" hole. When you re-fold your part, you will have non circular holes in the formed shape (just like in real life). The draw back is in your assemblies, you will not be able to mate concentric to your new holes. If this is needed insert an axis in each hole before you do the unfold operation. Mate to the axis instead of the face of the hole.

-Dustin
Professional Engineer
Certified SolidWorks Professional
Certified COSMOSWorks Designer Specialist
Certified SolidWorks Advanced Sheet Metal Specialist

 

[mkmachine]

Thanks for the suggestions.
This is exactly what I'm trying to do- I'm trying to set up drawings for parts to be watercut.
I was just going to say that I can't get this technique to work. When I cut parts on the flat pattern, then suppress the flat pattern, the holes are a child feature and become suppressed and disappear.
BUT, I think I've answered my own question, and learned how to use the fold and unfold tools. The fold/unfold seems to work.
Thanks for the help.

 

[NomLaser]

Correct, Fold and Unfold are what you need to use if you want to have a round hole in the flat pattern. Unfold your bends, create holes and then Fold the bends back.