UNBENDING SHEET METAL

Are your cuts perpendicular to the material thickness? If not, that may be your problem.

WT

Picture this: you cut off a section of a tube to create a trough, with the large open part of the trough aligned toward the top plane. Now extrude a cut downward from the top plane. That is my situation. Is there a better way to do this?

You need to make your profile, make it a sheet metal part, insert an unfold, make your cut, insert a fold. The problem is that you told SW to make a part and then go in with an endmill and make sides of the cut that are vertical, but in the sheet metal world, the edges of the material would not be that way unless manufactured that way.

WT

I tried this but it wouldn't work. I created the curved base flange, flattened, then cut out my profile. Then when I unflatten, I lose everything after the flatten feature. I cannot insert a sketch bend while in the flattened state either.

Maybe I am going about this the wrong way. What I have is a 55" radius on a 7.5" x 8.4" sheet metal part. I have a print defining the curved shape, and I want to create the flat pattern. What is the best way to go about this?

How about sending it to me and I will take a look.

WT

You probably need to check "Normal cut" . (I may have that backwards and you have to uncheck it.) If it won't make the cut with it checked, then you are probably in trouble and will have to try something like making your part as a surface and thickening it. Then you should be able to add the sheet metal feature and unbend it.

Jerry Steiger Tripod Data Systems "take the garbage out, dear"

I took a look at his part and the problem is that SW wants to have a flat face to be a reference for the bends. In some instances you can work with an edge, but it has to be a linear edge. If you use an edge as a reference, the subsequent fold that is based on that edge will be parallel to that edge - might make your part skewed & screwed if it creates an axis that is not oriented properly. I was able to start with a rectangular part, but the subsequent cuts to form the desired outer shape removed the straight edges, leaving no reference. The part is formed as only a large radius with no flat portions, as in rolling a part on urethane rollers to completely radius the part. I did get something usable (I think) by suppressing the fold feature to obtain the flat configuration. Interesting exercise.

WT

I would add a very small flat in the model (only a few thousandths), located so the flat pattern would unwrap in a logical relationship to the primary planes of the part. I suspect a small flat to facilitate unwrapping the part would have no affect on the final part.

Regards,

Anna Wood

I would add a very small flat in the model (only a few thousandths), located so the flat pattern would unwrap in a logical relationship to the primary planes of the part. I suspect a small flat to facilitate unwrapping the part would have no affect on the final part.

Regards,

Anna Wood