14 Replies Latest reply on May 25, 2018 2:06 AM by Shane Zhang

    Using Sheet Metal to do V-Groove Folds

    Harmon Amakobe

      Hey guys,

       

      I hope you can help. I'm attempting to accurately model some of our foldable parts using the Sheet Metal feature, in such a way that we can anticipate any problems with interferences before manufacturing. I've managed to get a good start on how to work around the feature such that it allows me to have material thickness with V-Groove cuts and still be able to fold the part (thanks to the post by Bernie Daraz in Accommodating V-cut and Press Brake in Solidworks). As such, I have no issue with simple parts that require folds in only one direction, ie. boxes.

      Box - Unfolded.JPGBox - Folded.JPG

       

      However, when I get to more complex folding patterns, I cannot seem to get all the folds to work correctly. It works just fine when it's a single thickness profile:

      Simple - Unfolded.JPGSimple - Folded.JPG

       

      But when I add the thickness with the V-Grooves in, using the exact same method as the boxes, I can only get it to fold around 1 axis at a time.

      Unfolded.JPGFold 1.JPGFold 2.JPG

       

      If I make the folds in one direction, any of the folds in the other axis simply refuse to work. I do not know if is an interference issue, a bending radius issue or anything, the error when I try to do the bending line gives no hints. I'm relatively new to using Sheet Metal and I can't tell if there are any fundamental physics rules in the tool I might be ignorant of that cause the bends not to work. Any suggestions?

       

      *I've attached both the single thickness file ("test") and the part with the grooves if it will help.

        • Re: Using Sheet Metal to do V-Groove Folds
          Dennis Bacon

          Hi Harmon,,, I was getting some errors while doing this. Mostly "Flange Interference after form" issues so I sliced some material off here and there until they were resolved. Also added some tiny reliefs. Check it out. It works as it should now. All of the cuts I made may not be required.

           

          Edit:... I included another (cleaner) file. PT1-2.. Hope you can get some ideas from it.

            • Re: Using Sheet Metal to do V-Groove Folds
              Harmon Amakobe

              Thank you very much Dennis!


              That worked quite well; out of curiosity, how did you determine where the interferences were/where to put the relief cuts? Does the Sheet Metal feature point it out somehow or was this simply something you knew to watch out for from experience?

               

              Thanks again for your help!

                • Re: Using Sheet Metal to do V-Groove Folds
                  Dennis Bacon

                  Since I do a lot of sheet metal I suspected that I would need reliefs in the areas where the bends crossed each other. Without the reliefs the bend will curl the material where you really don't want it bent. Then when you try to make a bend that crosses it, it will fail. - Bend across Bend. One of the areas where there was an "interference after bend operations" (I got that message while hovering over the Sketch Bend feature in the tree) was obvious (I'm sure you noticed that). The other was not so obvious so I had to do some searching (zooming in close). I wish there was an interference detection in the part environment that would highlight those areas. It is quite obvious you know what you are doing. I enjoyed working with this.

                    • Re: Using Sheet Metal to do V-Groove Folds
                      Harmon Amakobe

                      Yes, interference detection highlighting would be a useful feature to have, though thank you for teaching me what to look out or in the future. I did notice the bend across bend issues, but did not think to simply do reliefs to alleviate them. I'm glad you enjoyed solving the problem as much as I appreciated receiving the solution . Thanks again, and take care.

                • Re: Using Sheet Metal to do V-Groove Folds
                  Mark McMullen

                  Re: Sheet Metal - want to make 45 degree cuts...

                   

                  This maybe of some help to you, and to better understand SW with SheetMetal.

                   

                  I added one more configuration to play with on this one.

                  • Re: Using Sheet Metal to do V-Groove Folds
                    Lee Wondra

                    Hi Harmon,

                        I work with sheet-metal parts that other people design up all the time. One of my pet peeves is when they use Sketch-bends. I mean, who knows what the flat is when you start out? I get models where they change the bend radius or bend allowance to get the formed part they want. Usually the blank doesn't make the part they show in the print because the bend radius doesn't matching the tooling it takes to make the part or the bend allowance is way off. To my thinking, Solidworks was created to help determine the correct flat from the formed part - not the other way around.

                        Anyway, I set out to do this part "the right way". I've never had to do cardboard before. Removing some of the beveled edges was kind of a pain.

                        Take a look. see what you think.

                      • Re: Using Sheet Metal to do V-Groove Folds
                        Dennis Bacon

                        Not bad Lee.. I would expect if I would have started from scratch I would have done something similar.

                        • Re: Using Sheet Metal to do V-Groove Folds
                          Bernie Daraz

                          Lee,

                           

                          First of all, no insult intended. Back in the late early 70's when I was learning precision sheet metal we had to calculate the flat blank first, then lay it out using Dykem (blueing) and then scribe the lines for the insides and outsides of bends plus the bend centerlines. Looking at the technology now, we get flats from the laser or turret and start bending with bend allowancs or deductions on the setup sheets. There have been more than a few jobs I have done that we had or were supplied a flat layout. Using sketch bends is a unique way to add bends to a part that proves correct with the proper tooling and setups and the slight bit of cheating tolerances allow for. Virtually all jog/offset bends in SW are sketch bends.

                            • Re: Using Sheet Metal to do V-Groove Folds
                              Lee Wondra

                              Bernie,

                                   Seriously?

                                   In the 70's you had to do it that way. That's not the case any longer. It would be crazy to position a hole (or any feature) in the flat and try to keep it in an exact location in the final part - especially as the design changes (like all designs do).

                                   I'm not sure how you lasers or turrets work, but I have to supply the flats layouts for ours. Maybe if they unfolded them right at the machine using a 3rd party software I wouldn't care if the Solid Works flat was correct or not. I'm pretty sure our management won't put that much responsibility on the operators in the shop. I wish it worked that way here. Life would be easy.

                                   Keep designing the way your comfortable. When I get a model designed like that, I'll have to save it out as a step file and bring it back in as an imported model, delete bend radii, and add Sheet-metal (with my own "K" factor and bend radii). Seems like it defeats the whole reason we switch to SW to begin with - file sharing. I could have stayed in a non-feature based software to do this.

                              Lee

                              P.S.    Try checking the "Fix projected length" box next time you use the Jog command.

                                • Re: Using Sheet Metal to do V-Groove Folds
                                  Bernie Daraz

                                  Lee,

                                   

                                  I didn't mean to say I'm still doing that way but I have learned quite a bit from those days. We also supply flats top our turrets or lasers, they are made within SolidWorks using our bend deductions and allowances, we never scribe out anything anymore.

                                   

                                  One of the biggest anal apertures I have ever met in the precision sheet metal world told me the most intelligent thing I have ever heard, you'll never learn anything in sheet metal until you learn how to bend. Only then will you have a clear understanding of the nuances of precision sheet metal forming and then know how to apply them to your models.

                                   

                                  I have bend deduction and allowance charts from 40 plus years in precision sheet metal, SW does not calculate the jog allowance accurately, they use two bends while jogs in close proximity, say less than a two material thickness offset require a test bend to determine the the actual allowance.

                                   

                                  Now if "Fix projected length" actually functioned with my bend allowance for a joggle I would be thrilled. I have asked SW to allow me to put the figure (allowance) that SW uses to do the fix projected length to make that change I would again be thrilled.

                                   

                                  Some of my comments won't be correct or apply to you depending on the tolerances you work to, we have consistently formed to plus or minus .005 as our customers require it. The interesting thing to me is it's actually easier than 'roughing' or 'eyeballing it' when you are sure of your bend allowances and deductions. I posted a part about a year or so ago where I had twelve 90 bends in one axis and had to hold an overall if + or - .010 in less than 19". Rush delivery, write program, run 100 plus pieces and bend them. No test bends. Ship on time too! Boss really happy!

                                   

                                  Have a great weekend!

                                    • Re: Using Sheet Metal to do V-Groove Folds
                                      Lee Wondra

                                      Bernie,

                                           I'm glad you know how much material it takes for each bend using your tooling. Now imagine someone sending you a "Sketch-bend" file who doesn't have your tables. you'd change the bend radii and allowances, fold it up, and.............the part has changed. You'd have to go and move/change countless thing in the flat to get it to come out to what your customer wants/expect for the formed part. I do it every day! What a pain. Solid Works (before Desault) had it right. Bends radii, reliefs, and bend deduction should be at the end of the feature tree where they have almost no effect on the design intent.

                                           I have no doubt you may know what it takes to make part in your shop, but I also know if you send your files to another shop (who doesn't have your same tools) it isn't going to turn out the same. Back when we "coined" all our bends, it was easy to figure allowances. Now with air bending Is a hole different animal. The bend radius (if you can call it that) depends just as much on the die width and material tensile strength as it does the punch radius. It changes from one heat of material to another. Forming ±.005? The material thickness varies that much. We are a "job shop". The name of the game is small orders and quick turnaround. I need to be able to change the blank easily. I like to have SW figure the flat based off of the formed part so I can do that. Letting SW figure the formed part from the blank (sketch bends) is counter productive -unless you really need to work with a specific blank size (doubtful).

                                           Bernie, I'm sure you are very good at what you do, but like I said, this is a pet peeve of mine.

                                           For anyone else out there - if your making your own parts, I don't care what you do. Anybody else - be kind to the end user and do not use sketch bends (with rare exceptions).

                                      Lee

                                        • Re: Using Sheet Metal to do V-Groove Folds
                                          Bernie Daraz

                                          An often missed option is to use your bend deductions no matter the radius. Though if the part is not flattening whether correct or not this could prove difficult to use. In this case you would enter each bend parameter essentially forcing the bend deduction or allowance you need for your tooling..It isn't necessary to 'correct' the model.

                                           

                                          I have in many cases entered a sharp coin bend deduction even though a material thickness or larger radius is showing on a customer supplied model.