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Creating a boss.

mikes

New member
Hello all,

I need a boss to create a thread I a thin sheetmetal part; are there some other ways of creating a boss in a sheetmetal part?

For a while now I tried to create what I needed using Form (Punch and Form features) but all my efforts proved to be futile.

I wonder if I should create my part as a Boolean operation in assembly mode; this would be totally ridiculous
 

anandel

New member
This might be pretty much a rudimentary solution for what you are asking, you pbly are following these rules already, but I am just trying my hand to help.

View attachment 432

Like in the attached pic, make sure you have a radius = or > than the material thickness in the form punch. And I suppose that you are picking the proper surfaces to 'assemble' your form punch to the sheetmetal wall as in the pic.



And after assembling, when Pro/E asks to Select surfaces of punch to be used to create form first accept the default direction that it points. If it fails that way, try flipping it (I almost never used to get it right the first time) it should work.



And don't forget to 'exclude' the top surface from the 'Form' dialog box. If not it will be a closed form rather than an open 'extrusion'.



Hope this helps a bit.
 

mikes

New member
Thanks Anandel,

I did all you showed in your picture.

My situation is a little bit more difficult since the hole and the boss I need are not conforming to the rules that normally we follow in PRO/Sheetmetal- I am stretching a bit the situation.

I am creating this boss in a curved area with a small radius . I tried all possible situations however it does not land to an easy solution.

I keep looking for something more elegant if there is such a thing.

Thanks for the help, indeed.



Cheers,

Michael
 

mikes

New member
Thanks Anandel,

I did all you showed in your picture.

My situation is a little bit more difficult since the hole and the boss I need are not conforming to the rules that normally we follow in PRO/Sheetmetal- I am stretching a bit the situation.

I am creating this boss in a curved area with a small radius . I tried all possible situations however it does not land to an easy solution.

I keep looking for something more elegant if there is such a thing.

Thanks for the help, indeed.



Cheers,

Michael
 

Lazar

New member
Out of curiousity, is the curved area bent in one direction? If so, you could unbend your part, add the form feature, and then bend it back.



The technique I suggested works so that you can add bosses on simple curved sections. If the area is bent in more than one direction, it is highly probable that it won't work.
 

jperkins

New member
Mike,



Not sure what the problem is by your description. On thing that can be a gotcha is that the form must be fully enclosed by a reference surface. Can you be more specific as to what the specific error is?



jperkins
 

mikes

New member
Hello all,



Here is my situation.

I have a bracket with a circular (0.5 inch radius)loop opened, and tangent to the vertical leg (1.5 inch) of the bracket.

The top part of the loop is bent 90 outwards (horizontally), about
 

Dell_Boy

New member
There is another entirely different way to achieve a form similar to the picture posted above by anandel



You can do this by a cheat involving a thin revolved protrusion to give
you something that looks like the following but which is more flexible
than the default sheet metal equivalent



View attachment 522





The rim can be thinner than the parent material

R can be less than the thickness.

You can have a square corner on the inside.

You can show the dimensions rather than having to create them

You do not create a relationship to a punch part that needs to be maintained throughout the life of the product.





The Key Steps

Once you are in Sheetmetal mode Pro/E will not allow you to create a
thin revolved protrusion; however it will allow you to copy one from a
different model.



Using this knowlege, it is possible to copy a thin revolved protrusion
onto the first member of a pattern of holes, Ref Pattern the
protrusion, then add the radius and REF pattern that.



Once you have successfully done it the first time you can block copy
the three features (with no pattern) into the next model that requires
it













Edited by: Dell_Boy
 

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