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Trouble creating flat pattern..

12 REPLIES 12
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Message 1 of 13
prajwal
784 Views, 12 Replies

Trouble creating flat pattern..

I have a part here whichj I made by thickening the surface body. I am trying to create a flat pattern and Inventor keeps giving me a wrong pattern. Any suggessions would be highly appreciated.

12 REPLIES 12
Message 2 of 13
blair
in reply to: prajwal

I get to this point in the flatten and it stops without any error. I think if a person creates the cone portion first, does the thicken and convert to Sheet-Metal and then does a Counture Flange for each of the lip treatments it should work.

 

Capture1.JPG


Inventor 2020, In-Cad, Simulation Mechanical

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Message 3 of 13
prajwal
in reply to: blair

Just tried doing that. After I create the sketch and try to do the contour flange, I cannot select the edge where I want the flange to start from. Since it is a pseudo edge instead of an actual edge, I am assuming it cannot be selected for a flange.

Message 4 of 13
blair
in reply to: prajwal

Did you convert the cone to Sheet-Metal first, then do the Flange?

Inventor 2020, In-Cad, Simulation Mechanical

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Message 5 of 13
prajwal
in reply to: blair

Yes Sir. I removed the flange part from the sketch and made the sheet metal and then tried to add the flange.

Message 6 of 13
Mario428
in reply to: blair

Why not do it as a contour flange from the start.

 

Message 7 of 13
prajwal
in reply to: Mario428

Well, It would give an incorrect flat pattern if you did it from the beginning as shown in the image above.

Message 8 of 13
blair
in reply to: Mario428

The central section is cone shaped

Inventor 2020, In-Cad, Simulation Mechanical

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Message 9 of 13
blair
in reply to: prajwal

Try using the lower options and use the offset from each end. Possibly the angle of the cone portion is causing and issue at each end. I would try but I'm up to my neck in alligators this morning. This would also give you the offset at each end that your currently had. Did the cone shape only flatten out?

Inventor 2020, In-Cad, Simulation Mechanical

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Message 10 of 13
Mario428
in reply to: blair

Then do it as a lofted flange with straight sections .1 long on each side. If anyone thinks that .1 will make a difference in the part as made, ask the guy on the shop floor and listen to him laugh.

 

Like has been said many times before if you want a sheet metal part, do it in sheet metal. Yes I know it is easy to do it as a solid but converting it does not work.

Message 11 of 13
alewer
in reply to: prajwal

Does anyone else get a crash by selecting a certain face (see attached), before creating the flat pattern?

Message 12 of 13
prajwal
in reply to: prajwal

Finally the flat pattern works great after adding a contor flange to the rolled conical section and offsetting it from the face to get the notch. I was just making it more complicated by making in surface model and then converting it to sheet metal.Flat Pattern.png

Message 13 of 13
alewer
in reply to: prajwal

You beat me to it (see my attached model). You may want to stick with the surface loft + thicken because a bend line does not appear when a lofted flange produces a conic section. But I agree that the contour flange with offset is correct.

 

Edit: It's also worth mentioning that you don't have to start with a standard part to loft surface and thicken, then convert to sheet metal part. This can be done even if you create a new part from your sheet metal template. I prefer to avoid workflows that include converting between standard and sheet metal parts.

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