How do I convert a curved chamfer to sheet metal?

Ragwing

In this example:
https://cad.onshape.com/documents/957561517fb0dc9252f6f1f2/w/a7dbf37b75d2e1888db006ff/e/5a8176a063a390144cd3cdd5

I'm wanting to convert the chamfered shape to sheet metal. One of the surfaces is curved. I can chamfer this curved surface with the adjoining surface and achieve the solid I want. Now, when I try to convert the solid to sheetmetal, the chamfer along the top of the curved surface won't convert.

What is the best way to achieve the desired result?

Thanks,

Bill

eric_pesty

The problem is the shape you are trying to create cannot be flattened without stretching the material. Onshape sheet metal tools are meant for parts that you can manufacture from a flat sheet using straight bends.

For something like this your best bet is probably to use a "shell" feature to get the shape you want without using the sheet metal tool as it's just not meant for this kind of part.

Ragwing

Thanks Eric!

I'll play with the shell tool. For some reason it seemed to me that all the sheet metal parts would be flat. Have read some about the difficulty of accurately flattening. Not an easy challenge..

My initial thought questions how I'll flatten and segment the shell. Maybe will figure it out.

Thanks again.

Ragwing

Yeah. Shelling is the easy part. Can't figure out how to make a pattern for the sheet metal....

eric_pesty

That's the thing: if you can't make it out of cardboard, you can't model it in sheet metal because it can't be flattened!
So the short answer is you can't flatten that shape.
There are more specialized software that can generate a flat shape by stretching material but that's not really sheet metal anymore... More typically used for fabric design I think...
That said it would be neat if Onshape could do "stretching", you could try this app: https://appstore.onshape.com/apps/Design & Documentation/3RPIJMNQJ2SXMC7IZEUELB23XF3VEXVAAKM4UUA=/description

EvanReese

If i'm reading the shape right, it's a conical surface which can be flattened (i.e. made from cardboard), but Onshape sheet metal doesn't support it right now. You could facet it somehow and get an approximation. Here's my hack at it. Not finished, but hopefully enough to get you going. 

https://cad.onshape.com/documents/dec36813f165f0453c918023/w/ab58d8f970f53ca5c8505ce1/e/4098e526bc3f08dccb164210

eric_pesty

I guess I wasn't thinking about splitting it up in chunks like this, I was thinking about flattening the entire thing to a single piece of metal/cardboard, which isn't possible. But if you are welding (taping/glueing) the pieces together rather than bending then yes that one piece is a conic and it can be flattened even though Onshape can't do it directly!

EvanReese

@eric_pesty
yeah, I see your point for sure. I don't really know the end goal, but hopefully this is a helpful start.

matthew_stacy

In CAD parlance, the scope and meaning of "sheet metal" is limited to parts with straight line bends, as @eric_pesty stated, to simplify the  flattening computation.  These are sometimes described as "developable" surfaces.  Bend radius and location of the neutral axis (as expressed by the k-factor) suffice to relate the formed part to its flat pattern.

In the broader manufacturing sense "sheet metal" often includes more complex parts with "double curvature".  Consider dimples and louvers (which we routinely struggle to include in our CAD sheet metal models) and automotive body panels.  Stampings.  These parts can be formed and there is a corresponding flat pattern (quite possibly multiple viable flat patterns depending on where material is stretched to/from).  But the math relating flat pattern to formed part is incredibly complex ... and the solution perhaps indeterminate.  And the pattern is likely to include a perimeter flange that will be trimmed away after forming.  A skilled tin knocker can readily form beautiful complex shapes with a hammer and anvil, that we as engineers with expensive CAD software will struggle with.  Consider a part as "simple" as a salad bowl or deep-drawn sink.

EvanReese

matthew_stacy said:

In CAD parlance, the scope and meaning of "sheet metal" is limited to parts with straight line bends, as @eric_pesty stated, to simplify the  flattening computation.  These are sometimes described as "developable" surfaces.

Agreed, but a cone is a developable surface. I've found need to flatten them before and I wish this were part of onshape's sheet metal tool. Likewise with certain kinds of lofted sheet metal parts which are handled in other CAD systems. It can be done, and I'm sure it's on the dev's radar, but just may not be at the top of the list. I'm looking forward to it anyway.

Ragwing

Thanks guys for the dialogue. It’s helpful to a rookie like myself!

The conic section is understandable to me and that idea will help me layout the one difficult part by hand/manually. 

The intent is a collection of 2D parts that can be laser cut.

 Thanks again!

Bill