Breaking up the geometry model - SOLIDWORKS Tutorial

- [Instructor] Planar symmetry is a very powerful technique where we can represent a full structure with just half or even a quarter of the model. We know that the runtime and storage requirements of the model are based on the number of degrees of freedom to a square power law. So having a half model size means a quarter of the runtime and so on. So we'll start of by creating the geometry needed for a half symmetry model. We're going to create a New Study. And we're going to call this, half symmetry. Going to use the default static analysis simulation. So we check to create the study. I should see the half symmetry tab appear at the bottom of the screen here. I may need to split the model in half to show we've got an accurate split plane. Let's first create some reference geometry. Click on the Features tab. Click on Reference Geometry and pick Point from the drop down. Now here choose the Arc Center method. And select any of the arcs at the little end. I'm going to pick this one here. Check OK. Now we should see a point created on the center of the little end. Once we're here, lets create a new view. So space bar, New View. Lets call this, little end. I want to select Reference Geometry again, and select Plane. So we want to select the point as the first reference. It remembered the point we just created, Point1. If not, then just reselect it. The second reference is the plane that we want to relate this to. So with the Geometry Feature Tree open, what we want to choose is, Top Plane. Click Okay. We can see a preview of the plane that's going to be created forming the central line cut of the con rod. So we click OK. I want to show the Geometry Tree View so lets drag it down here so I can see a Plane1. I just want to rename that as symmetry. And I want to Hide it. So again lets go to our Analysis Preparation tab. This is useful subset to geometry manipulation tools. Especially suited for FEA. So lets choose Split. On the Trim Tool is going to be the symmetry plane I just created so click on that. There's only one part, so if I select Cut Part, it's going to be cutting that part into two bodies. Now I want to choose the action to Consume cut bodies, in other words to delete them. Now the option in here is which body I want to delete. You see the scissor icon indicating which one do you want to cut. I want to cut number two. That's been highlighted here. That's the side of the model we want to get rid of. So click OK. And then we're just left with the half model. Lets drag our Model Feature Tree back up again. I want to right mouse click on con_rod_advanced and apply the material to that at this stage. You can see the various libraries that are available. We've set up a course material library. Lets open that up. This is the category we made of steel. And in here is our 4030 Forged Steel. So we Apply that and we can close it out. And now this model has material properties 4030 Forged Steel. Now we're going to apply the tensile load only at the little end. Just to demonstrate the usage of the Symmetry option. So we need to split the surfaces of the little end, to be able to apply the bearing load over just the left hand 90 degrees and at the end of bow. Lets go to that new view, little end. Click on the side face which is facing us. Click on the Sketch tab, and here I want to create a new sketch. Hover over the central region of the little end and pick the point that we just created. And now we want to convert that entity, so it's projected into our sketch plane. Now click on the Line icon, pick out point and just drag any line vertically, so it just goes all the way through the con rod little end there. Just check Line Properties and Insert Line, close the sketch. Now we can go to the Analysis Preparation tab again. And now we want to use the Split Line option. The action here is remembered, the sketch that we just created. If not, open up the Geometry Feature Tree and select the appropriate sketch. Now we want to choose the surfaces we're going to split. So we choose these four surfaces of the little end. Click OK. We can see now the splits of the curve. And it's giving us the chance to apply our bearing load just on that extreme left hand end of the con rod. Now we need a local coordinate system to be able to define the orientation of the bearing load that we're going to be using. So we go to the Features tab, select Reference Geometry icon and choose Coordinate System from the drop down. So in the Selections box, for the center of the coordinate system, you choose our Point1 we just created. X-axis, any edge which is running along the x direction. Y-axis, you can choose a vertical line here. Z-axis, going to choose horizontal line just running down there. Click OK. This created our local coordinate system which we're going to be using to apply the bearing load. Just going to rename this as little end. And now we can save this model off. We'll save it as con_rod_advanced_1. So in this video we've seen how to create the half symmetry model. And we've split the little end ready for the loading actions.