Holes in flatten sheet metal parts

[krywarick6]

I have a curved sheet metal part, a simple arc, that holes on the curve. When I flatten the part, I can't add ordinate dimensions to the holes. They translate into slpines when flattened.

Any suggestions on how to add dimensions for the drawing?

Christopher Zona - Product Designer
Loretto, Ontario

 

[ctopher]

Worked here.
Show the part in the "flat pattern" state of the drawing view.

Chris
SolidWorks 10 SP4.0
ctopher's home
SolidWorks Legion

 

[SnowCrash]

If you project a circular sketch onto a curved surface it will be a spline, not a circle, when you flatten it out, an d difficult to dimension. Create a sketch with points at the center of your holes (which is not a simple task) and dimension to them.
In real life you would punch the holes in the flat, right? I would suggest that you create a location for the holes in the curved, but put the actual holes in the flat pattern configuration.

--
Hardie "Crashj" Johnson
SW 2010 SP 4.0
HP Pavillion Elite HPE
W7 Pro, Nvidia Quaddro FX580

 

[ctopher]

Change dimensions in the view to be "True".

Chris
SolidWorks 10 SP4.0
ctopher's home
SolidWorks Legion

 

[ctopher]

Four of the holes don't like ordinate dims.
Files attached.

Chris
SolidWorks 10 SP4.0
ctopher's home
SolidWorks Legion

 

[krywarick6]

So the PITA solution was to calculate where the holes land in the flat state and add a feature. I had to trick the holes though.

Since a round hole going through a curved surface will create a spline in the flat state, I had to make the curved holes just a smidge under size so that they would be cut away with the flat holes.

Referencing the design table will so how I calculated the positions. The hole wizard features before and after the bend show what I had to do to get a valid hole in the flat.

Works for now, but still a PITA!

Christopher Zona - Product Designer
Loretto, Ontario