Clean way to show after bend dimension for sheet metal parts?

Tristan_Neumann

I have a sheet metal part where I want to give a dimension from the face of the first flange to be bent to the next bend line. Is there an easy wat to show a part with only certain bends having been made?

Please see bellow

https://cad.onshape.com/documents/9870de6526a6a3a16602ba19/w/0938d873b9adda3f339d43b6/e/4626c0c9290a4138dba744d3

eric_pesty

Tristan_Neumann said:

I have a sheet metal part where I want to give a dimension from the face of the first flange to be bent to the next bend line. Is there an easy wat to show a part with only certain bends having been made?

Please see bellow

https://cad.onshape.com/documents/9870de6526a6a3a16602ba19/w/0938d873b9adda3f339d43b6/e/4626c0c9290a4138dba744d3

Not 100% clear on what you are trying to do. What I might do on a part like this is show a side view and add dimensions to the virtual sharps.

Are you making the parts "in house" or are you sending them out to a 3rd party? If using a 3rd party then we normally just dimension the finished part as they will adjust the flat shape to suit their specific machines.

If doing it "in house" ask the operator exactly what they need.

Otherwise you would want to crate configurations of the part showing it with every bend added incrementally but that seems like it shouldn't be necessary and would require some manual work as you can't just "unfold" bends one by one (maybe you can with a move face with the rotate option but that might mess with the flat pattern dimension which wouldn't be good...

You could re-create it step by step using a series "Sheet metal fold" features: https://cad.onshape.com/documents/9f116620b0f6d04445f57293/v/2df4f2beeec4dae0b92bdf58/e/de11451baedbaa3f6c9bae51

Unfortunately it doesn't look like you can derive in a flat pattern so you'd have to create a sketch of the flat pattern first, then derive that into a new part studio and create the bends one by one, here's an example where I've started, it seems like the flat pattern length is preserved after the first fold so it should work in theory.

https://cad.onshape.com/documents/a8f932a8375c8d68c7cacbff/w/e0108f735b056605cfdc4644/e/6442f36e0a3e59d1714d1bd0?renderMode=0&rightPanel=sheetMetalPanel&uiState=62eac5a5d15f25022f7bf3fc

bryan_lagrange

@Tristan_Neumann all you press brake operator needs to do is use bend allowance and add it to the bend line to accomplish what you want since the first flange is bent at 90 degrees.

If you need to show a step by step you can use the Unfold 2 and Refold 2 feature scripts along with configurations (this way you just have one part) to get a step by step on the drawing.

For the first bend you can use the default flat pattern and dimension to the bend line. For the second bend and gauging off the bent flange use the configuration of the top view, show tangents, put a center line between the tangents of the unbent section (since this is where you bend line would be) and dimension. You will also have to manually put the bend note.

Here is a link to the test document.

https://cad.onshape.com/documents/7b82bd7a676f7074238e0a1b/w/f4936701d42b1001d7fc756b/e/9640da5c4d419d2e0850acd6

dirk_van_der_vaart

I think I know what you mean, but then you will have to create the sheetmetal part in step's, make a drawing of the part with the first bend, make the second bent and make the next drawing etc.
I think it is normal procedure to have a drawing of the final product and a drawing of the sheetmetal flat with the bendlines.
If your bend parameters like radius etc are correct for your machine's then there will be no problems.

Tristan_Neumann

I could make separate parts representing each step of the bend process, but the issue I run into with that approach is that onshape will not give me the location of the bend lines for the bends that have not been made up until that point. Unless there is some approach I am not familiar with.

eric_pesty

Tristan_Neumann said:

I have a sheet metal part where I want to give a dimension from the face of the first flange to be bent to the next bend line. Is there an easy wat to show a part with only certain bends having been made?

Please see bellow

https://cad.onshape.com/documents/9870de6526a6a3a16602ba19/w/0938d873b9adda3f339d43b6/e/4626c0c9290a4138dba744d3

Not 100% clear on what you are trying to do. What I might do on a part like this is show a side view and add dimensions to the virtual sharps.

Are you making the parts "in house" or are you sending them out to a 3rd party? If using a 3rd party then we normally just dimension the finished part as they will adjust the flat shape to suit their specific machines.

If doing it "in house" ask the operator exactly what they need.

Otherwise you would want to crate configurations of the part showing it with every bend added incrementally but that seems like it shouldn't be necessary and would require some manual work as you can't just "unfold" bends one by one (maybe you can with a move face with the rotate option but that might mess with the flat pattern dimension which wouldn't be good...

You could re-create it step by step using a series "Sheet metal fold" features: https://cad.onshape.com/documents/9f116620b0f6d04445f57293/v/2df4f2beeec4dae0b92bdf58/e/de11451baedbaa3f6c9bae51

Unfortunately it doesn't look like you can derive in a flat pattern so you'd have to create a sketch of the flat pattern first, then derive that into a new part studio and create the bends one by one, here's an example where I've started, it seems like the flat pattern length is preserved after the first fold so it should work in theory.

https://cad.onshape.com/documents/a8f932a8375c8d68c7cacbff/w/e0108f735b056605cfdc4644/e/6442f36e0a3e59d1714d1bd0?renderMode=0&rightPanel=sheetMetalPanel&uiState=62eac5a5d15f25022f7bf3fc

Tristan_Neumann

Yeah, my explanation wasn't very good, let me try to clarify.

We are making this in house. My operator needs a dimension from the face of the small one inch flange. He needs to make this bend first because he will run into interference issues on the press brake  if he tries to make that bend later. Because he plans to make that bend first he will not be able to push the edge of the part against the backstop of his press break to line up the next bend. Instead he will push the face of that first flange (highlighted in green bellow) against the backstop.  Because of this he needs the dimensions for the subsequent bends to come from said face (NORMAL DISTANCE 14.886 shown bellow). In Solidworks I was able to selectively unfold the part such that this is the only bend that has been made. I don't believe this is an option in Onshape innately, but your approach with the "Sheet Metal Fold" feature script does give the desired result.

Thank you

bryan_lagrange

@Tristan_Neumann all you press brake operator needs to do is use bend allowance and add it to the bend line to accomplish what you want since the first flange is bent at 90 degrees.

If you need to show a step by step you can use the Unfold 2 and Refold 2 feature scripts along with configurations (this way you just have one part) to get a step by step on the drawing.

For the first bend you can use the default flat pattern and dimension to the bend line. For the second bend and gauging off the bent flange use the configuration of the top view, show tangents, put a center line between the tangents of the unbent section (since this is where you bend line would be) and dimension. You will also have to manually put the bend note.

Here is a link to the test document.

https://cad.onshape.com/documents/7b82bd7a676f7074238e0a1b/w/f4936701d42b1001d7fc756b/e/9640da5c4d419d2e0850acd6

bryan_lagrange

It is just Unfold and Refold feature script.

eric_pesty

bryan_lagrange said:

It is just Unfold and Refold feature script.

Ha! I didn't know these existed! That's a much easier way to do this than what I was proposing!

The only thing I noticed is that the unfold feature flips my part orientation in some odd way for some reason

bryan_lagrange

Just stumbled upon these going through public feature scripts. I found that odd as well with the orientation flipping. 

I would only use these if you wanted to represent folded and unfolded states in a sequence. It will not allow any cut geometry.

S1mon

Unfold and refold (with appropriate tune-ups) should really be part of standard Onshape sheetmetal functionality.

bryan_lagrange

It has been a while since we have seen sheet metal enhancements. Hopefully we will see a new batch soon.