16 Replies Latest reply on Jul 12, 2018 2:43 AM by Heiko Sohnholz

    Sheet metal bend settings

    Jorn Nijenhuis

      Guys, i have a challenge here.


      I am designing a part as a sheet metal. Which has to be manufactured by a supplier of our company. Their criteria to upload the model is to convert it to a .step file.

      The challenge is: if i do that and upload the .step file, their software gives an error and says: that there is a overlap in the flat pattern of the sheet metal. Their suggestion is that there must be a problem/issue with the way Solidworks handles the DIN 63-something standard.

      The supplier opened the .step in 3 different CAD programs ( hiCad, Creo and Catia) and gives the same problem with all of those software packages.


      Is there a way to configurate the edge-flange bends in such a way that when converted to .step and then opened in an other cad program, the unfold is Always exact ( deviation of .5mm is acceptable) like the unfold in Solidworks?

      I do put in K-factors for the custom bend allowance.


      p.s. see attached pictures, i opened the .step in Inventor, and flattened it out using 2 different unfold rules, 1 gives problems, 1 does not.


      So is there a way to overrule these unbend rules in different cad packages? Or should i just mention to our supplier that they maybe dont use a k-factor based unfold rule?

        • Re: Sheet metal bend settings
          Bill Toft

          Can you post your part?

          Are you uploading the bent part or flat pattern as a STEP file?

          What does your supplier use for K-Factor / Bend Allowance / Bend Deduction for this material & sheet thickness? BD & BA are machine  material specific so using their numbers helps ensure your SW flat pattern matches.

          • Re: Sheet metal bend settings
            Steve Calvert

            If they collide when the flat is un-suppressed in Solidworks, it just won't work, period.


            Steve C

            • Re: Sheet metal bend settings
              Rubén Rodolfo Balderrama

              Attach your fille fella.

              • Re: Sheet metal bend settings
                Jorn Nijenhuis

                as an attachment the part i am talking about

                  • Re: Sheet metal bend settings
                    Ned Hutchinson

                    I had a look at your part doesnt overlap for me.

                    Saved part as step in 2018 opened in 2015 unfolded and folded fine

                    bend c.png


                    usually i just send dxf and we bend ourselves

                    send them a drawing of a flat aswell showing were solidworks bends it


                    edit:another thing is the edge flange settings that other cad might not like


                    Bend Outside

                    bend 6342654c.png



                    Material outside

                    bend 634544642654c.png

                  • Re: Sheet metal bend settings
                    Heiko Sohnholz


                    you have used the wrong k-factor in your part. 0.5 means the neutral fiber and does not suit the AISI material. Should be around 0.3 (DIN6935 says 0.325)! So if you write your part to STEP, re-import and unfold it with the correct k-factor, you will see the issue:


                    And that's what your manufacturer will get...

                    By the way: You used a radius 4mm - in real life (and depending on the tools sets) the radius will be around 6mm!


                    Cheers, Heiko

                      • Re: Sheet metal bend settings
                        Bill Toft

                        Strange. I unfolded the downloaded part (K-Factor = 0.5)  and gap was 1.35 mm  and bend lines 29.92mm apart.

                        I changed K-Factor to 0.3 and got the same measurements. (I went to 5 decimals and the numbers still matched exactly.)

                          • Re: Sheet metal bend settings
                            Heiko Sohnholz

                            You have to try this with the re-imported STEP file. Because this is, what the manufacturer will get and see...

                            But you're right … of course the distance should change …


                            I deleted all configurations, all Equations, all additional Edge-Flange-Feature (excluded Edge-Flange1), and deleted all individual settings with no effect. But when i re-create the Edge-Flange1 than it works! With changing the k-factor the length of the unfolded part will change. So my conclusion is, that there must be an issue in this part...


                            As mentioned above, the unfolded length must change, when the k-factor is altered - as in the re-imported part!

                              • Re: Sheet metal bend settings
                                Heiko Sohnholz

                                So i have done another test right now: Make a new part, insert this part into it and use convert to sheetmetal. When changing the k-factor from 0.5 to 0.3 the intersection comes across!

                                  • Re: Sheet metal bend settings
                                    Bill Toft


                                    I did the export to STEP & import to SW & convert to sheet metal and got your results. K=0.4 changes gap from 1.35 to 0.004 and anything smaller overlaps.

                                    I wondered if there is a bug in SW (changing K-Factor in original part does not change gap)? I noticed several configurations in that original part and also wondered if that was a factor.

                                    So I created a new part of just the features in this area. NOW K-Factor changes affect the gap. I got that same 0.004" gap with K=0.40.


                                    Looks like you should recreate this part from scratch.

                                    • Re: Sheet metal bend settings
                                      Bill Toft

                                      I got an email of a reply from Dennis Bacon, but his post isn't here, so I copied it.

                                      - - - - - -

                                      No Bill,, the part is ok but it looks like somewhere along the line the k-factor was set at the bend, not flange or Sheet Metal feature.. If you change the k-factor there to .3 you will get the overlaps. Select the each bend only then edit.


                                      I changed the k-factor to .3 then changed the bend radius to 6mm so it wouldn't suck up so much material then the part comes out with no overlap. First set the tab area you see to the o.d. of the bends then did a material inside for the flanges so nothing other than the radius would change.


                                      If Jorn does that he can play with the k-factor and bend radius all he wants and see the outcome. Personally I would ask what the rule is that the supplier is using and go from there. I doubt that they would want to change the k-factor but may be flexible on the radius. Sort of looks like they want to be wiping this but probably not necessary..

                                      - - - - -

                                      So I learned something today! There are 3 places to set the K-Factor and I never used #3 (EdgeBend)

                                      1. Normally I set the K-Factor in the Sheet Metal feature.

                                      2. Sometimes I need to override that K-Factor on one set of Edge-Flanges, so I do it there.

                                      3. It turns out I could also override the K-Factor of a single EdgeBend.


                                      I now see that Jorn had set his K-factor to 0.5 in the sheet metal feature.

                                      But then he overrode it (but used the same K=0.5) for the Edge-Flange.

                                      Finally he overrode it again for each EdgeBend (but used the same K=0.5)

                                      That explains why, when I set Edge-Flange to use default K-Factor, the changed Sheet Metal K-Factor had no effect.


                                      So, to keep things simple, Jorn should ONLY set the K-Factor in the Sheet Metal feature.

                                      That means NOT checking Custom Bend Allowance in the Edge-Flange or EdgeBend features, unless of course they are actually different K-Factor numbers!

                                      Bend Setting Locations.png

                                      Bend Setting 1 Sheet Metal.png

                                      Bend Setting 2  Edge Flange.png

                                      Bend Setting 3  Edge Bend.png

                                        • Re: Sheet metal bend settings
                                          Dennis Bacon

                                          Very Good Bill Toft. I didn't like the way I had worded it and was afraid there were going to be too many questions as a result so I deleted it. I remember struggling with this sort of thing in 2005 when I first started using the program and things weren't working like I expected. In those days I would always lay it out the old fashioned way to make sure the flat pattern was correct until I felt comfortable with what I was doing and what was going on.  Indeed there are 3 places that you need to look. I did incorrectly say that by increasing the bend radius you could solve the problem without altering the geometry where it crashes. I should have stated by making the radius smaller (with same k-factor) would work without altering the geometry. Of course I never use k-factor, always bend deduction or allowance.

                                          This is a screenshot of the original file and an altered file on top of each other. The altered file (gold) has the smaller (2mm with .3 k-factor) bend radius.


                                          With a 4 mm bend radius.


                                          I think it would behoove Joran to alter the geometry at the the colliding edges. Maybe even move the holes up if he can.  First find out what the supplier is using for a rule so he can accurately adjust the resulting gap.