Using the geometry fixup tool - SOLIDWORKS Tutorial

- [Instructor] In the introductory course on SolidWorks simulation, the fillet runout regions caused a lot of problems with meshing. They tended to produce tetrahedral elements with very high aspect ratios. It was very difficult to control this behavior and we had to accept high aspect ratios in the big end region. We'll now be looking at a very powerful way of identifying and defeaturing these problem areas. We first need to create the split lines to allow the big end bearing load to be applied. Let's select the surface, the little end here, the one closest to us. Go to Sketch, click on New Sketch. Let's choose point, and then create a point which is going to be at the center of the little end. Check OK. I want to go to curve, and I want to drag up a curve which runs vertically and which is clear of the con rod. Do the same thing below, drag a line which is vertical, again, clear of the con rod. Check OK. Now we can close out of the sketch. Now we can go to Analysis Preparation, we can say Split Line. The Sketch should be the current sketch we've been working with, again, if it isn't current, go to the geometry feature tree, and choose the sketch from that tree. Now we need to select the services we want to do the splitting on. Once they're selected, we just check OK, and the new splits are created. Let's go look at the little end closer view. In particular, that's the surface we want to apply the bearing load to. Let's go back to a general view. Let's go to Tools > Geometry Analysis. A Geometry Analysis form shows a series of analysis parameters which we can check which include short edges, small faces, sliver faces, and so on. Now, we can leave these as default, click the Calculate button. The results of the analysis show that, in our case, we've got eight knife edge vertices as shown here. Click on the plus to open that up. In every case, this relates to the infinitely sharp corner formed around the runout of the fillets between the con rod body and the big end and the little end. We can click on these and we can highlight them in turn. You can see each one relates to a problem area that we had, what we've called the fillet runout. This is exactly the area we had problems with in the introductory course. If you remember from that course, it was very difficult to avoid elements with high aspect ratios right at the cusp of any of these vertices. Click the check mark to close out. Now having identified where the problem areas are, we can now attempt to simplify the geometry to deal with them. We go to Analysis Preparation here, click on the Simplify icon, make sure we choose the Volume Based option, and click on Find Now. A list appears in the results menu. These represent the geometric features that were created in the con rod build and which are the fundamental cause of the problems. The first two Cut-Extrudes associated with the pocket region was machined out, and these weren't a problem to us. The first fillet refers to the pocket region again, and we didn't find any particular meshing problems there. Click on this Fillet, and this is one of our problem fillet areas, so Fillet number 2 is an issue. Similarly, Fillet number 3 at the little end, same problem. What we can do here is we can right mouse click and say Suppress, and you can see the fillet has gone away. Also, the feature is grayed out, it's suppressed in the geometry feature tree. Let's do the same thing for fillet 3, can Suppress that. Again, it disappears, and it's also grayed out, it's suppressed within the geometry feature tree. Let's hit the cross to close out the Simplify form. Now, the task panel remains, let's get rid of that so we can go to View > User Interface > deselect Task Pane. Let's click on the Configuration Manager at the top of the geometry feature tree, and we have the default configuration, but if we click here, you see we've got a new configuration. This is the one that's active, it's got a green check box next to it. If I double-click on the default, you can see, now we see the fillet. Clicking between them, Simplify, no fillet, Default is fillet. There are two instances or two configurations of the geometry now, which is extremely powerful functionality. Let's just come back to the Simplify and let's rename that as no_fillets. We'll be using these two configurations to create a study for each one, in other words, we'll be developing two parallel studies. At that point, let's save our SolidWorks model, and we'll save it as advanced_5. In conclusion, we've seen how to identify where there are problem areas in the geometry, we've also seen how to defeature, and at the same time, we've seen how to spawn a second configuration which we can work with in parallel.