Cut in curved sheet metal skews part

[JimmyDoe]

Hello all,

I do not have too much experience with sheet metal, but I believe something weird is going on. In my attached .ipt I have a rolled half cylinder made with a contour flange. I do a 'cut normal' to create a half circle cut at the top. This makes my flat pattern look great, but in my folded model my part becomes skewed and I don't understand why.

I would appreciate any help.

[kgilham]

This is the correct behavior in Inventor. What Cut Normal essentially does is unfold the sheet metal, make your cut and then refold the sheet metal. This is to mimic the typical manufacturing process of cutting out features in the plate with a laser or burn table and then bending them. During this process the cut out will skew just like in Inventor. If you are wanting it not to be skewed in the final part then you would need to un-check Cut Normal, but this will cause the flat pattern to have a skewed cut out.

[JimmyDoe]

I do understand the skew of the actual cut when it is cut flat and then rolled. But when it is rolled, the top and bottom of the cylinder should remain flush so that when it is set on its edge, it does not sit at an angle. As seen in the attached files. Please advise.

[Anonymous]

Turn on the XZ plane. The model is slightly off plane after Cut3

[JimmyDoe]

That is the problem I am asking about. When the cut is put in the model, all of a sudden skews off of the XZ plane. But when the cut is removed it goes back to the proper way. I don't believe this is how things should work. Because in the real world this does not happen.

[kgilham]

Thanks for clarifying.  It looks like you may have found an issue with the cut command.  I will take a look at this problem and see if we need to get a developer to fix it. 

[JimmyDoe]

Ok, thanks Kyle. I appreciate your quick response. Please keep me posted on this thread.

[JDMather]

Good catch!

The attached file clearly illustrates the issue.

[CCarreiras]

Hi!

The Cut tool with "normal cut" option fails lots of times, if is failing to your case, just do it "manually":

1. Cut the curved sheet
2. unroll
3. fix the flat result
4. and roll again.

[kgilham]

It looks like this is a known issue in Inventor that has been around for awhile because there is a workaround.

1. Move your end of part to right below your contour flange

2. Edit the contour flange sketch and add a small straight section that is tangent to your arc

3. Delete your current flat pattern

4. Select Define A-Side and select the inside face of your part

5. Drag the End of Part below your Cut

6. Create another cut to remove the small straight section.

I have attached the part that was created using these steps.

While this issue has been around awhile I will create another report to see if we can get our developers to fix this is a future release.

[JimmyDoe]

When I following the steps above I end up with the same result.

When I open your part(it looks good) but when I try to create a flat pattern I get an error message saying to redefine the A-Side. When I do redefine it by selecting the inside face, the part becomes skewed as before and I end up with the same result. Can you please try the same and see if you end up with the same result?

[JimmyDoe]

Could you save that a version earlier? I am not up to date with my service packs.

[kgilham]

Yes, I am seeing the same problem now.  Here is my last workaround.  I have tried this out and it seems to work pretty well. 

1. Delete the cut you have made

2. Add a small straight section to your arc

3. Unfold the part, using the straight section as your Stationary Reference

4. Create a cut in the part without checking Cut Normal

5. Refold the part

6. Cut the straight section off.

This should give you a flat pattern and keep the part straight against the XZ plane.

I am currently installing an older version of 2016 and will upload the part using this workflow once it is installed.

[JimmyDoe]

I was asking JD if he could upload an earlier version of his part. I have been opening your parts successfully.

I followed your steps and things are working. Previously, how I would make my sheet metal parts was to unfold the part, add my sketch and then cut and refold. But this time I thought I would try it with the cut normal function, since it can be hard to know where the cut will end up on a folded part, if you sketch on the unfolded version. Luckily this was on the centreline...

[JDMather]

Here is one easy technique.

Sheet metal is uniform Thickness.