Is it possible to project the hole pattern of one part to another part?

[Anonymous]

This client sent us a step file that I need to unfold but their designer did a $hit job so I have to redraw it. It's not a difficult part in that sense but one thing that would really help me in the future is to somehow project the hole pattern of one part to another. 

Mine is the one called UTB at the end. It would really help and minimize the risk of error if I could do that somehow and not measure every hole and all that.

Thank you!

[salariua]

I think you don't need to remake the part. Just add 2 cuts and it flattens.

If you do need to remodel it then place them both in an assembly and project the original holes.

Here's my result of the original piece after the cuts. I have attached the modified ipt in 2015 and the resulting dxf:

One cut here and one the other side, Use delete face to remove the punch in the middle but it will flatten with it and the outside contour won't change.

[Anonymous]

I noticed that as well just as you sent it to me. Thank you!

But what about this projection thing? Is it possible?

Cause I have a file that is kind of twisted at the flanges that I have to remodel. It would be nice to somehow be able to sketch while using the original file as a model.

[salariua]

This flattens without a problem. You can also derive your original model into a new part and work around it.

[Anonymous]

085708 flatten without problem? How? I get several error messages and my colleauge told me it's because it is twisted.

[salariua]

All I've done was adjusted the thickness and it flatten.

[Anonymous]

That makes no sense at all. Could it be a difference between 2015 and 2014? What thickness did you put in?
Do you mind sending me the dxf?

[salariua]

3mm

Check attached.

[Anonymous]

I really don't understand why it won't flatten when I do it. But I appreciate the help.
You must have been working with Inventor a long time?

[JDMather]

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@Anonymous wrote:
1. That makes no sense at all. 2. Could it be a difference between 2015 and 2014? 3. What thickness did you put in?

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1. Makes perfect logical sense.

2. No.    Yes, this one unfolds in 2015 but not 2014.

3. You should be telling us what the thickness of the part is.

Use the Measure command reveals that the part is 3mm thick.  So that is a known value.

Since you converted that part to sheet metal - you need to tell Inventor what the thickness is that you just measured.

Click on the Sheet Metal Styles editor.

If, after setting the Thickness to 3mm and it still isn't unfolding - attach the new file here.

[Anonymous]

I did that already. I was wondering if he maybe put in another thickness than I did. I still can't fold it out. No idea why. I added some print screens at the attachments. 

[JDMather]

Oops, I edited response above.  This one does unfold in 2015, but not 2014.

But if I Delete Face and Thicken - it does unfold in 2014.

[Anonymous]

Any idea why?

[Anonymous]

I see what you did there with the Thicken thing. Very clever. Thank you!

[JDMather]

If you Derive as a surface body - there is no need to do all of the Delete Face work.

[Anonymous]

You mean I derive it as a surface body and then thicken it? But then I'll get 2 equal parts, totaling 6 mm. And I can't unfold a surface.

[JDMather]

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@Anonymous wrote:
You mean I derive it as a surface body and then thicken it? But then I'll get 2 equal parts, totaling 6 mm. And I can't unfold a surface.

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I don't know what that means?  Did you try it?   See attached example.  (expand the derived component in the browser)

Turn on the visibility of the surface body.  Delete the Thicken and see if you can reproduce it.

[Anonymous]

Ah ok. Now I get it. I made the mistake of thicken it the wrong direction.