Holes in Curved Surface - Flat Pattern (Inventor 2014)

[rob_bolter]

I’ve searched the forums and cannot quite find a similar scenario to me, but somebody is bound to have had the same issue. Basically I’m trying to create a circular cut in a flat pattern for a hole made in a rolled piece of sheet metal.

I have created a "case" (this is what we call it) to mount an axial fan, it will require holes for mounting the motor plate. When I create these holes in the rolled case assembly they appear to be fine, but when I flatten it they are turned into two sets of semi-circles or ellipses.

This is only a problem when we run the parts on our Laser; the laser will attempt to start the cutting at the end of each of these "semi-circles" causing a hotspot where the two semi circles meet. This causes the hole to be slightly smaller than intended in this area causing great difficulty inserting bolts, they normally require drilling.

 Our material thicknesses vary from about 3mm to 8mm.

Edit: I’ve included a crude example of what I’m trying to achieve. To really see what I mean, place the file into a Drawing file and zoom into the hole. I couldn't add the file, with only 3 features the file was 5mb in size.

I need it to be fairly simple as my colleagues will need to adopt the technique and their not all trained fully with Autodesk Inventor.

By the way, I have a temporary solution, it's just a little complicated and was wondering if anyone else has another solution. (My solution: use square holes first in the un-flat, use the diagonal lines from each corner of the square in a sketch on the flat pattern to place a circular cut on its mid points.)

[CCarreiras]

Hi!

But, in real world, do you drill the holes in the part already folded or in the sheet flat patterned?

You can unfold the part to apply the holes and then refold again. You will have now perfect circles in the flat.

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[CCarreiras]

Hi!

Also, if you want to send the example, you can pull the EOP at the begining of operations, and the part will be a lot smaller in file size.

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[rob_bolter]

They are drilled in the fully formed part (rolled & flanged).

The machine operators dont currently perform any drilling, the production cell does (the ones who add the other components to the rolled case). These cases range from 250 diameter to 2000 diameter. 

You suggestion would work, however, during assembly its not always possible to place a hole in the flat pattern. We often require fully assembling the product to place holes in the case. If we place them in the flat pattern, they may not line up correctly with the internal components.

[rob_bolter]

This still leaves the file to be over 5mb in size. Im not sure why, there are only 3 features within it.

[JDMather]

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@rob_bolter wrote:

This still leaves the file to be over 5mb in size. Im not sure why, there are only 3 features within it.

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Find the red End of Part marker in the browser.
(End of Folded on sheet metal parts EOF)
Drag the red EOP to the top of the browser hiding all features.

Save the file with the EOP in a rolled up state.

Right click on the file name and select Send to Compressed (zipped) Folder.

Attach the resulting *.zip file here.

or you can send it to me jmather_at_pct_dot_edu

[CCarreiras · Accepted solution]

Hi!

Check this... i use this method to solve issues like you describe.

After finish the part:

1. Unfold
2. create a sketch in the face, and use the tool "Project cut edges"
3. Cut the holes.
4. (If needed, repeat for the other face)
5. Re-fold.

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[wanruly_ws]

Hi,

I want to ask about Hole in Rolled Plate (Shell) using contour roll.

My case is, in AutoCAD drawing, i create a layout of hole for this hole in rolled plate base reference from arc length of outside surface (outside diameter) for distance between one hole to another. This method is make easier for operator in fabrication process for indicate between hole position orientation.

But when i am using Inventor, i create using contour role and add hole, then make a flat pattern, the result is different because a flat pattern reference is netral axis of a rolled plate.

Maybe anybody have experience to solve this case?

Hopely, in a future version of inventor can make a alternative result of drawing for flat pattern result and Layout Hole on outside diameter of surcafe.

i send a file for explain my case.

Thanks,

Wanto Rulyanto

[rob_bolter]

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@CCarreiras wrote:

Hi!

Check this... i use this method to solve issues like you describe.

After finish the part:

1. Unfold
2. create a sketch in the face, and use the tool "Project cut edges"
3. Cut the holes.
4. (If needed, repeat for the other face)
5. Re-fold.

Did you find this reply helpful ? If so, use the    Accept as Solution or Kudos - Thank you!

---

This is eventually what i discovered myself. This should also answer"Wanto Rulyanto"question. It seems the only way to do it without the hole becoming obscured during the rolling process.

[cadman777]

Hi,

Interesting discussion.

I realize this is a late post, but maybe someone can help me:

I want to do the same thing: make holes in a tank shell so that the flat pattern shows proper sized circular holes, not elipses.

In the past I would use a sketch perpendicular to the tank c.l. and o.s. the shell o.d.

Then use 3d sketch to contour roll the sketched circle to the i.s. shell surface.

Then use split surface and then thicken subtract to make the hole.

I use the i.s. surface so the nozzle neck will fit properly to the shell hole.

If the hole was made from the shell o.d. it would be too small for the nozzle neck.

However, using this method makes the hole size incorrect every time.

I tried using all the 3d commands, plus the 2d commands and sufraces, but to no avail.

Doing it w/the flat pattern unrolled is not good, b/c I can't figure where to locate the holes properly using my base sketch.

I always use a base sketch to control all features, sizes and locations in a tank.

IOW, every part in the tank is controlled by the base sketch (and sketch Parameters).

Anybody do it the way I do, and have a solution for a true circular hole in the flat pattern?

Thanx ...

[cadman777]

Guys,

I just figured-out that I do have a way to do what I want to do.

My brain was tired ... must be age and too many hours behind the screen.

Anyways, the truth is, if you make the hole correctly in the rolled view, it will be an elipse in the flat.

Also, the way I do it on nozzle repads is Split Surface using a sketch that projects to the i.s. surface of the thin shell.

Or else for a full shell, I extrude a cylindrical surface, based on a circle sketch, onto the i.s. surface of the thin shell.

Then use Split Surface.

Then in both cases, use Thicken Subtract.

It makes a hole perpendicular to the rolled surface, so in the flat, it looks like a clean-cut opening.

Sorry for the confusion I may have caused w/my long post above ...

[James]

Sorry this may be way too late, but if you select "Cut Normal" it will cut so that the flat pattern has all holes 90° from the flat face. this works on even wavy sheet metal parts.