Whenever I use the "Convert to Sheetmetal" feature, I get odd and large corner geometry. Unfolding it and trying to add material is a PITA sometimes.
Is there a setting im missing or is this feature not very good to use? Attach is the part I am working on, it consist of 3 different angles.
FYI, im using SolidWorks 2009.
These things happen when you let the computer do the thinking for you..... :-) It may not solve the problem correctly or in the most efficient manner.
I would model it way you want with your cutouts modeled correctly for your manufacturing process, then Insert Bends. Then you have exact control over the results.
Cheers,
Anna
By cutouts, do you mean the corner treatment? Maybe im overlooking something but how can I model this myself when without the part being flat?
Chris,
No not corner treatment. Do not be stuck on only using the sheet metal toolbar to create sheet metal parts. Add your own cutouts, with extrudes, to the corners before you Insert Bends.
Surfacing and thickening will also work very well here. Again you will need to add your own cutouts in the corners before thickening and then inserting bends. This is the technique I would use here for your part.
Lots of ways to get what you need, with and without using the sheet metal tools.
Post your model and we can create a couple examples for you.
Cheers,
Anna
Thanks Anna. Ive never used Surfacing before when creating a sheet metal part, always looking for new/better ways to model. I attached my model to the original post.
Chris,
Here is one possible way to get what you need.
Thickened surfaces work well as you get a true representation of how the metal will look on the edges. The edges of the metal will be normal when formed.
A few more features, but you can control and get exactly what you want.
Cheers,
Anna
Chris,
Here is another way using extrudes and then delete faces to create your surface to thicken. Takes advantage of creating the geometry quickly, then the power of surfaces to get the sheet metal geometry that will match metal reality and be able to be flattened.
Cheers,
Anna
Thank you Anna for the examples. Ive never seen sheet metal modeled like that before.
I think in surfaces a lot when doing sheet metal. It is because of my training and cutting my teeth in 3D CAD in the automotive industry back in the day before solid modeling. We did 3D wireframe and surfacing for class A automotive exterior sheet metal and interior plastic designs.
Sheet metal modeling is just thickened surfaces in my mind. Back in the day with sheet metal we only modeled one side of the sheet metal part, inside of sheet metal (the side that would hold water). For plastic we modeled both sides, completely, with wireframe and surfacing.
Surfacing techniques can make easy work out of solid modeling problems. See Charles Culp's response in the thread on laying plywood on a cone. This is a great use of surfacing techiques to solve a problem that would be likely impossible with standard solid modeling techniques.
Cheers,
Anna
Hi Chris,
Here's one in SM, its all run by the sketches & equations.
Michael
EDIT Just remembered your in 2009 , will redo it
IN SW 2009 you cannot close the corners like you can in SW2010 but i have extruded up to the surface to get the same effect
I've had exactly the same issue in the past and as Anna has suggested, I have ended up modelling as a surface or solid before using the "Add Bends" tool to convert to sheet metal. An alternative method to shrink down your corner relief gaps is to use the "Move Face" tool. Just offset the faces to a more reasonable gap and if necessary, add a note on your drawing when showing the flat pattern.
I often deal with this by modeling the part using the inside dimensions and reversing direction when coverting to sheet metal. For some reason that gives you better much better control over the corner gaps, breaks, and dimensions. If your exterior dimensions are more important, you could get creative with a reversed shell and then use the interior faces for your bend faces & edges.
