PROBLEM AFTER CUTTING SHEET METAL

[an18211821]

After cutting sheet metal via split body, the edges of the cutted sheet metal follow the splitting path, so i can not handle the as sheet metal edges to bend them etc

they are not flat any more . I tryed to select the face, sketch along path a rectangle and then cut via exture, after that i can select the flange tool, but when i try to use it i get error or strange results. 

Any advise

[TheCADWhisperer]

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@an18211821 wrote:

Any advise

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Can you File>Export your *.f3d file to your local drive and then Attach it here to a Reply?

[an18211821]

this is not the original design, just a test model to see the problem

Please see attached file, 

thank you

[TheCADWhisperer · Accepted solution]

See Attached (adapt as needed).

[an18211821]

Thank you very much Sir

[an18211821]

what defines the fillet distance? How can i know for different thickness of steel , what fillet should i use on bend points?

[TheCADWhisperer]

I should have made the Fillets (bends) a function of the Thickness so that if the Thickness changes the bends automatically update.

As far as what size to make them - that depends on the material and manufacturing process.  A general rule of thumb is minimum inside radius = thickness, but you should talk to your fabricator, especially if you have a need to go below thickness.  Going with a bigger radius is no problem.

[carl.j.barker]

Can also be done using split face rather then split body. Split the outside 11 (or inside which ever is the correct position) faces using the sketch, unfold the component and extrude cut the unwanted faces.

[an18211821]

the first design was made using Sheet metal, not a solid body. When i tryed to use split face i didnt manage to cut to metal. could you post an exampe with screncast?

Thanks

[carl.j.barker · Accepted solution]

This is your original file altered to use split face.

[an18211821]

i checked the method. what if i want to keep both splitted bodies?

[carl.j.barker]

Then I am afraid you made an error right at the start. Sheet metal parts should always be their own component since there can only be 1 flat pattern per component and  it allows you to use joints etc. But the big reason is Fusion will not let you copy/move, nor create a component from, sheet metal bodies. In this case it can be rescued by saving your design, starting a new one then inserting the part twice, this has the effect of converting to component. You can now break the links and edit the second component to remove the lower part instead. You'll now have two components one upper part and one lower part.

Caveat...   Before anyone jumps on me, Yes there are times when creating a single body sheet metal part you can ignore this rule, bottom up modeling single part files and the like. Or you could save two copies of your design, insert and not break link, use edit in place and pretend you were going bottom up all along.

[an18211821]

i managed to get the result by "project" the surface cut when it was unfolded , and then i used the split body with the new sketch line that created by project tool. The result is correct and and metal parts can now be handled without errors