I am new to sheet metal and am having a problem embossing a rib onto my part. I keep getting the error that my parts thickness is not compatible with the form tool. I have tried multiple combinations and variations of part thickness and radius on the form tool. I have attached my part, form tool and error screen shot. I am also still using 2009. I would appreciate it if anyone would give me some guidance on this.
Paul,
I didn't open your files but from my experience the most common reason is that you didn't allow a sufficient radius. The thought train here is that any outside radius that your tool will form must be greater than the material thickness plus .001" at least. I use .005 as a calculated minimum inside radius.
Paul, you can do it. I was able to get the results you were after using your model.
Unfortunately, I'm running SW14 so my model file isn't going to be of any use to you.
To make your forming tool work correctly, you have to meet the following criteria:
Radii at the stop face have to be greater than the thickness of the material (you got that)
If your forming tool crosses bends, you want to set your forming feature to remove all faces on the underside of the tool (not including the stop face)
When the tool crosses bends, the stop-face contour has to be a perfect match to the contour of the bent part-In your case, the forming tool radii and geoemtry weren't quite the same as the base flange sketch in the sheet metal part. When you do your radii calcs, you have to remember to increase the convex bends by the thickness of the material.
You have to locate the form tool so that the bend starts line up correctly. Add relations to the locating sketch to position the forming tool
Placing a form across a bend screws up the flat pattern of the part, so make sure the form is suppressed in the flattened configuration. (you really can't add this form to the flattened state anyway)
Closing thoughts: SolidWorks sheet metal is very particular about applying thickness uniformly in its operations. For that reason sheet metal tools arent suitable for stamping, progressive die or tube bending and as such, a forming tool probably isn't the long-term answer for this part. Think about it, you can't change the part without modifying the forming tool. You can only use this forming tool with this part, and you can't edit the forming tool in the sheet metal part file. If this is a part that's going to be made by stamping, then i'd look at BlankWorks or one of the other tools for generating forming flats. If this is going to be a plastic part, then I'd use an indent feature with a toolbody defined in the part file to get the final result.
Good luck.
John,
Could you please post what you did to my models? I have a friend who has 2014 and he will open them up so I can see what you did.
Thank you
Paul Ronning
Paul, there's the finished part. The forming tool is on my other computer. I'll post that tomorrow.
Finally got it to work. I was picking the middle surface as my stopping face but it would not work as expected. I finally selected one of the ends as the stopping face and it worked. Thank you John for your insight, especially your hint on selecting the faces to remove.
Thank you
Paul
See, now I didn't think of changing the stop-face to one of the other faces. You've taught me something.
Paul, you can do it. I was able to get the results you were after using your model.
Unfortunately, I'm running SW14 so my model file isn't going to be of any use to you.
To make your forming tool work correctly, you have to meet the following criteria:
Radii at the stop face have to be greater than the thickness of the material (you got that)
If your forming tool crosses bends, you want to set your forming feature to remove all faces on the underside of the tool (not including the stop face)
When the tool crosses bends, the stop-face contour has to be a perfect match to the contour of the bent part-In your case, the forming tool radii and geoemtry weren't quite the same as the base flange sketch in the sheet metal part. When you do your radii calcs, you have to remember to increase the convex bends by the thickness of the material.
You have to locate the form tool so that the bend starts line up correctly. Add relations to the locating sketch to position the forming tool
Placing a form across a bend screws up the flat pattern of the part, so make sure the form is suppressed in the flattened configuration. (you really can't add this form to the flattened state anyway)
Closing thoughts: SolidWorks sheet metal is very particular about applying thickness uniformly in its operations. For that reason sheet metal tools arent suitable for stamping, progressive die or tube bending and as such, a forming tool probably isn't the long-term answer for this part. Think about it, you can't change the part without modifying the forming tool. You can only use this forming tool with this part, and you can't edit the forming tool in the sheet metal part file. If this is a part that's going to be made by stamping, then i'd look at BlankWorks or one of the other tools for generating forming flats. If this is going to be a plastic part, then I'd use an indent feature with a toolbody defined in the part file to get the final result.
Good luck.