9 Replies Latest reply on Jul 20, 2017 7:44 AM by Bernie Daraz

    Spotweld Locating for sheet metal parts

    Bernie Daraz

      This is less a Solidworks use comment than it is advice I would like to share from my 40 years in manufacturing.


      In my years in producing precision sheet metal I had encountered a vast number of tools that I had no idea were available. Wilson Tool is one of the premier tooling manufacturers for turret tooling among others.


      I was working at one very progressive place more than 25 years ago, and they used Wilson tooling to produce these ‘locaters’ for spotwelding brackets and precisely locating them. Previously I have made locating fixtures, some of you may know how tricky they can be and do add handling time to the process. Sometimes they also get warm and you need another fixture or you might have ‘timed’ the process so the fixture could cool.


      This progressive place used this tooling and had two sets, one slightly larger. They had to be defined correctly in the programs and they had names, WELD01, and WELD02. WELD02 being the larger one. WELD02 also had to be set ‘higher’ to clear the half shear from WELD01.


      We would put at least two of these on mating parts for location during spotwelding. It was easy for the guys to just pop one part over the other and spotweld without any further clamping or fixturing. We also never used the locators in a manner where the individual parts could be located 180 degrees out. They were always offset in such a manner to be 'crooked or slanted'. The visual would indicate to the spotwelder that he had the parts orientated incorrectly.


      Well, one day the turret guy made a mistake and swapped the tools. The parts would not locate and I was called over. My simple solution for this lot was to just ‘force’ them together using the PEM machine and two flattening tools. I think the issue added less than two hours to the job. To this company, that was a loss.


      I looked at the tools and decided that we would use the ‘form up punch’ of the larger tool (.125 diameter) and the ‘form upper tool” of the smaller (.121 diameter) tool. The upper tool being the ‘die’ and ‘creating a form’ of .123 diameter.


      Now instead of using two tools in the turret we only used one set with no height set requirement as long as it appeared to be about half of the material thickness.

      If you’re thinking how can you use a die smaller than the punch? You know more than the average person. Much more. Since the tooling never punched a through hole, why not.


      So, I reordered another set from Wilson and then received their rejection. I was directed to call their tooling ‘genius’ and we had the discussion, first he telling me that you cannot have a punch larger than a die and must always have a clearance. I countered with, why? I’m not punching through. It’s a half shear according to your description. OK, so now I have his attention.


      I did discuss that I had expected extra wear on the tooling set and we would monitor for that. It all worked very well, eliminated the need for a second tooling set and the potential for errors. All good I would say. Eventually we had three turrets and had three sets of this tooling.


      The image below is from Wilson's website and while not an actual picture it does represent what to expect from using the tool set. Try to imagine a punch being performed from the bottom of the material roughly half way through. This one tool set was used on many thicknesses and materials without concern for die clearances.


      WT Image Half Shear Round.JPG

        • Re: Spotweld Locating for sheet metal parts
          Frank Krockenberger


          Nice write up,  We use a similar process with a semi price and a hole or slot to mate to.

          A while back you did a write up about tig welding two metal parts together at the ends.

          I was asked to design a sealed welded vacuum chute for our de-burr machine and I showed

          the manf. manager this and he about jumped out of his chair.  Worked like a charm.

          This is 40in x 32 tall

          Thanks for your valuable input.




            • Re: Spotweld Locating for sheet metal parts
              Bernie Daraz

              Frank, nice work! I would confidently 'argue' that I developed that process 30 years ago. But for the sake of discussion I developed that process at the same progressive shop I mentioned earlier, I did receive a bunch of objections from the lead programmer on how much time it took. He was overruled after the welder commented that he does not have to tack items in place and 'bench' them into tolerance for the welding. This project had 10 inches per side of welding totaling 40 inches that had to be ground and finished with a textured paint. The welder had no issues and worked faster making that one job more profitable, the sides had no 'waves' in them as was normal before and they came out perfect through every run after that. All good of course.

              Where I was different from your depiction I used a half material open overlap corner for the full length of the sides. I did not use the convention you did with the method you show. Not that it is in any way wrong or incorrect. Our welders, myself included preferred the half open corner. Our quality departments loved the fact that there was no 'birdshit' visible on the inside corners after welding. No corners ever cracked later.

              Thank you for offering another improvement to our trade. Though I'm semi-retired I am still involved. I refer to this process and the half shears as creating 'self-fixturing' assemblies and the resulting accuracy is as good as the punching tolerances, often plus or minus .005 inches.

              • Re: Spotweld Locating for sheet metal parts
                Bernie Daraz

                Frank, I had a little time this morning and wanted to show you what I described earlier. I called this tongue and groove. I am trying to show the half material overlap where I provide the 'grooves' for the mating side when it is formed. I use a half material high 'tongue'. We used just .005 clearance at each end of the groove. The groove would be .25 wide for a single hit and the tongue would be .24, that way the one punch would be able to do both and we would have some room for misalignment on the initial bends. That of course would be corrected. We did use other lengths when a rectangle or square was already being used in the program. Any part could have had any length tongue and groove. I'll bet the welders loved your part! For this company the programming was just overhead, anything we did to improve manufacturing or accuracy made money for the company.

                TnG Picture.JPG

                  • Re: Spotweld Locating for sheet metal parts
                    Steve Calvert

                    Is this in SW2018?  Seems like I saw this somewhere...


                    Steve C

                      • Re: Spotweld Locating for sheet metal parts
                        Bernie Daraz

                        Steve, I did this in 2014 this morning. I originally did it in 1976 or 1977. Back then we didn't have CAD. When I brought it up to the programming manager he said it was too much work but I twisted his arm and he finally did it. We had a text based Windows programming system for the Strippitt turrets. He started complain less when he found that a command was available to mirror the corners. So all we had to do was define one corner of a square or rectangular part and use the commands:

                        SYM/ XB/2 YH/2

                        punching commnds....

                        SYM/ 0

                        B was defined as the width of the part as a variable

                        H was the height of the part as a variable

                        Variables allowed us to enter a material thickness and bend deduction, we could actually change either and the programs would update at compile.

                          • Re: Spotweld Locating for sheet metal parts
                            Steve Calvert

                            Cool...  You're way ahead of the times my friend


                            From the What's New in Solidworks 2018 Beta 2



                            Steve C

                              • Re: Spotweld Locating for sheet metal parts
                                Bernie Daraz

                                Steve, Thank you very much for that! I'll have to look into it. I'm not doing anything of a productive nature any more and I'm not likely to get 2018 so I posted 'the old way' as my procedure.


                                Judging by the picture above and referencing a very old job, we did a .040 aluminum weldment, it was curved with about a 16" radius. The curved flat part was punched in the turret as was the 'flange' or end. We used a few tongue and grooves then tack welded the assembly. Finally we sent the part out for dip brazing. Aside from the square corners (no bend radius) it looked beautiful. I know the picture shows full tongues and groove as an example only, the welders appreciate the half material as it allows us to get really good penetration and avoid the birdshit inside the corners. Also too many of them!! LOL! I could see myself orientating the tig torch every time the welding axis changed.

                      • Re: Spotweld Locating for sheet metal parts
                        John Stoltzfus

                        I have eliminated a lot of fixtures using the tab design in not only sheet metal but also structural steel projects, tubing weldments.. All you need was a flat table, square, tape measure and knowing where to start tack welding...  Especially if you have a vendor that has a 3D Tube Laser.....