Ok the video went a bit long at 10 minutes, but I decided to just show my entire work flow for a part like this. If I were to make this part, I would make some adjustments to the tabs, making them look more like what Certiflat does to allow space for the welds. And there is no audio, as I do not have a good mic setup, and I feel strange talking to my self.
I downloaded a certiflat welding square from grabcad as a IGS file. It imported as a bunch of unstitched surfaces. So the first thing I had to do was enter the surface workspace and stitch it back together into a solid. Then I enabled the design history. Next I wanted to split this model into 4 bodies. I was able to create the first split with a sketch line. But the second one would not split with a sketch line for some reason. So I just extruded the sketch line into a surface, and used the surface to create the split. I did the same for the final split.
Once I had all 4 bodies, I wanted to add locating tabs. I started by creating a sketch on one of the narrow pieces, and projected the face of all 3 bodies on that plane. I turned off the visibility of the bodies, to prevent anything from snapping to them. Then I turned the projected geometry to construction, as I only wanted to use them as references. Next I sketched 4 rectangles, and made them all equal length. Dimensionned everything, and added a few more constraints.
I turned on the visibility only for the body I wanted to add these tabs to. Then I used the extrude tool and selected all 4 tabs in the sketch. For the distance I used the āto objectā option and selected the second face. Make sure that the extrude tool is joining, and not creating a new body or cutting. Then repeat the same steps on the second inside part.
With the male tabs on both bodies, I used the combine tool to create the matching notches in the side plates. Just make sure you check the box to keep tools, and you set the operation to cutting. After that I used the press/pull command to offset the female cuts slightly, to ensure the tabs will have some breathing room for assembly.
Last step before creating the DXF is to make a flat pattern. I converted all 4 bodies into components, so I could use the joint tool to arrange them. This also helps place them all on the xy plane.
To create the DXF, I simply created a sketch on the face of one of the parts. I then used the project tool and set it to bodies. Clicked on all 4 bodies and then pressed ok. Then right click on the sketch, in select save DXF.
