Holes in curved sheet metal surface

Experimenter
Experimenter

I draw a simple curved piece of metal that we are going to roll up.  I can add holes simply with a tangental plane and the hole command.  I flatten the piece and add it to a drafting file.  I now need to dimension the holes in the flattened drawing so someone can punch plate.  The dimensions always want to snap to one node on the hole.  It also won't give a correct diameter dimension.  Is there a different way do the holes to make it correct?  I am using ST9.

 

Thank You

11 REPLIES

Re: Holes in curved sheet metal surface

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

Try creating the holes in the flat state.

 

Unbend Command

Create holes Command

Rebend Command

LMGi
www.TLMGi.com

Re: Holes in curved sheet metal surface

Experimenter
Experimenter
This does work to put the holes in the piece correctly. The problem I see with this I need to do the math to figure out where the holes go. In this example of a series of holes in a rolled piece, it can be quite a few holes. Is there no way to do this graphically inside the assembly?

Thanks

Re: Holes in curved sheet metal surface

PLM World Member Legend PLM World Member Legend
PLM World Member Legend

Create the holes as you have originally been doing.  In the flat pattern, the holes are not true circles but b-splines as you can see in the draft file.  The give-away there is the L 1.57" dimension that has been placed instead of the expected diameter.  The work-around is as follows:

  1. In the model, unbend the curved geometry.  Do this by creating an unbend feature (NOT a flat pattern!).
  2. Create derived curves based on the holes.
  3. Delete the holes.  You will now have eight outlines left behind that represent the position and size of the holes.
  4. Create eight circular holes using the derived curves as a cue for the position and size.  Do this by sketching circles.
  5. Re-bend the geometry.
  6. The flat pattern will end up with true circles for the holes and will be able to be dimensioned properly in the draft file.

No math needed!

Re: Holes in curved sheet metal surface

Esteemed Contributor
Esteemed Contributor

Hi there @Rfaber,

 

Yes, you can do this in the context of an assembly.....just need to make use of the "Inter Part Copy" command, and then can make apprpriate relates to the sheet metal Holes/Cutouts.

 

I sometimes use a smaller "pilot" hole in the formed piece, then unbend it, to place the correct holes, in instances where there is no opportunity to use pattern[s] to achieve it faster.

Sean Cresswell
Design Manager Streetscape Limited
Solid Edge ST10 [MP2] Classic [x2 seats]
Windows 10

Re: Holes in curved sheet metal surface

Esteemed Contributor
Esteemed Contributor

@chrisstandring  His model is a contour flange. I don't think you can unbend a contour flange.

Bruce Shand
ST9 MP10 - Insight - Win10 - K4200

Re: Holes in curved sheet metal surface

PLM World Member Legend PLM World Member Legend
PLM World Member Legend

@bshand  Sure you can.  I just did now in the posted model.

Re: Holes in curved sheet metal surface

Esteemed Contributor
Esteemed Contributor

bshand wrote:

@chrisstandring  His model is a contour flange. I don't think you can unbend a contour flange.


You sure can......you just need to select the end [thickness] face to be the "Fixed Face" to remain stationary, and the rest of the part is the bend. [see attached  - modified OP model]

 

 

Sean Cresswell
Design Manager Streetscape Limited
Solid Edge ST10 [MP2] Classic [x2 seats]
Windows 10

Re: Holes in curved sheet metal surface

Esteemed Contributor
Esteemed Contributor

Oh, $hit!

Bruce Shand
ST9 MP10 - Insight - Win10 - K4200

Re: Holes in curved sheet metal surface

Honored Contributor
Honored Contributor

Sean, the pilot hole is a great way to work through the problem. I will be using that next time it comes up.