Learn about the reason for producing well-shaped mesh of adequate mesh density
- [Instructor] The finite element analysis method discretizes the continuous CAD geometry into large numbers of small elements. The shape of these elements is very important. Badly shaped elements will result in numerical inaccuracy and possible failure of the analysis run. The total number of elements has also to be kept within reasonable bounds. The solution time and memory requirements of the analysis are roughly proportional to the number of nodes squared. If the element numbers and hence node numbers are uncontrolled, we can rapidly run into very long run times.
The first thing we will consider is element quality. SOLIDWORKS uses tetrahedral elements for solid meshing. The ideal shape for a tetrahedral element has 60 degrees including angles at all vertices, or we can describe this as having equal length edges. As the distortions increase away from this perfect shape, the result is increasingly poor numerical representation of the displacements and the stress field within the elements. This means that the stress distributions can be badly affected. If the element distortion gets too bad, then we can contaminate the whole numerical solution throughout the model.
Let's run a trial mesh on the conrod and see what kind of elements the default meshing gives us. So we click on the Analysis Study tab, conrod static analysis. If I right mouse click on the Mesh icon in the Analysis Feature tree, then we want to Create Mesh. We'll leave the Mesh Density slider bar in its default central position. This controls the size of elements globally throughout the model. Click OK and the mesh will run.
We right mouse click on the Mesh icon, we go to Details, and then we have a summary of important details of the mesh. So we have, for example, the total number of nodes is just over 13,000. The total number of elements is just underneath 8,000. And then the maximum aspect ratio is about 9.8. Now one of the fundamental measures of element quality is this aspect ratio. A high aspect ratio is a fundamental measure of element distortion.
We've got a ratio of about 9.8 to one. We can see where this is positioned. So if I close down this dialogue box here, right mouse click again on the mesh icon, and say Create Mesh Quality Plot, we can check on the Aspect Ratio button here and then hit OK. Now there's a new element in the Model Feature tree under Mesh, called Mesh Quality Plot. We've got one mesh within that which is labeled Aspect Ratio.
We can right mouse click and we can hide that, and we can right mouse click, and we can show that at any time. If I now Hide the mesh quality plot, you notice the mesh has disappeared. We need to come back up into Mesh and say Show Mesh. So it's just a little quirk. If we'd plotted and shown the aspect ratio, and I say Hide, we lose the mesh. You find it back up here again if you just say Show Mesh.
So let's just see that mesh quality again, and it works again. It was around about 9.8. We could see it's located up here. Let's go and look at the big end. And it's associated with an element that's trying to run through the fillet. Now if we look in really closely, we can see that element has really flattened out. This type of feature in the geometry is really awkward for us to deal with.
It's not ever really there physically. You can't machine a feature like that, and when we discretizes it, do the FEA mesh, then we start to pick up features like that. We'll come back to this point as we go on through the course. Let's zoom out of the model. The blue here is indicating the lowest aspect ratio is just close to one. Let's zoom in and look at an area with that kind of aspect ratio, and they're well shaped tetrahedral elements close to equal angles within there.
We come back out to the full model. Now there's a second mesh quality review option within SOLIDWORKS called the Jacobian. So right mouse click and say Create Mesh Quality Plot. This time let's check Jacobian. Now the Jacobian isn't a geometry measure, but it's part of the numerical evaluation of each element. Strictly speaking, it can only be calculated accurately when the full FE analysis is run. However, SOLIDWORKS can produce an estimate of the Jacobian.
To be useful, this needs to be a high quality estimate. The high quality estimate can take longer to run within SOLIDWORKS and could be very time consuming for a large model. So with the Jacobian selected, let's check OK. Now we can see under the Mesh Quality Plot icon, there's a new Mesh Quality Plot called Jacobian and that's what we're looking at here. The maximum value is 2.416. If we zoom in that area again, again you can see it's associated with these problem areas that run out of the fillet.
Now the Jacobian check isn't particularly accurate here because we've used the default settings. Later on we're going to improve the accuracy of the Jacobian check by increasing the order of accuracy which again could take longer to run within SOLIDWORKS. Now the other aspect of meshing we need to consider is the number of elements. So let's right mouse click on Mesh and look at Details again. So we've got a default mesh size of around about 0.4 of an inch, and we've got just over 13,000 nodes, and about 7,700 elements.
Let's experiment on half the elements sized down to 0.2 of an inch, and this will be globally throughout the model. So I right mouse click on Mesh, choose Create Mesh, open the Mesh Parameters option, and rather than accepting the default which as I said was around about 0.4, let's halve that and go for 0.2. Click OK, and it'll remesh.
Let's go to the standard view. We can see in general we've got a much finer mesh. So literally globally, we've halved the element size. Right mouse click on the mesh icon, choose Details again, and now we can see the total number of nodes has jumped to around about 92,000. The total number elements has jumped to over 60,000. The key metric is the number of nodes. This is directly related to the number of degrees of freedom in the model.
So here we've got about 6.6 times more nodes than we did when we had 0.4 inch as the default size. Now analysis runtime is roughly proportional as a square law, so the analysis on this basis will take up to 43 times longer. It is not always that extreme, but certainly it is some kind of power law there. So 40 times longer to run, that could be quite significant. So we'll close that down. Let's check the aspect ratio by going here Mesh Quality Plot, opening that up, and we've got our Aspect Ratio Plot here ready to go.
So we now just say Show, and now we can see our aspect ratio has gone up to 12 and, lo and behold, it's in the same place as before. So putting in a finer mesh is actually making this aspect ratio worse. If I zoom in really tightly, you can see this element here is really flattening out. You can imagine in the limit as we try to put more and more fine elements in, we're getting tighter and tighter in here and we're really chasing our tail.
We're trying to mesh something which isn't physically realizable, and that's a kind of a trap that we can get into with FE analysis. So we're going to think about techniques to avoid that. It's a limitation we just have to accept. Let's come back to our full view. Let's repeat this exercise and halve the mesh size again. So Mesh, Create Mesh. Again we had 0.2, so now we're going to halve that to 0.1.
Just click OK, it's remeshing. You can sense it's taking longer to do the meshing now. It's not instantaneous, even on the machine I'm using here. Now it's complete. You can see the model is really saturated now with very tiny elements, 0.1 of an inch size throughout. Let's right mouse click on Mesh, go to Details. We can see the metrics, see what we've done. The total number of elements is over 400,000.
The total number of nodes is over 600,000. That's a big factor on the number of initial degrees of freedom on the initial mesh. And if we scale that up, I've worked out it means a runtime of about 1,000 times longer in an extreme case. So we're getting to the stage where we're chasing this power law. Successively halving the element size means much, much longer runtime. So it's obviously not a very effective or productive strategy to try and improve the quality of the mesh.
Let's check out the aspect ratio. Again we open up the Mesh icon, Mesh Quality Plot. Let's right mouse click on Aspect Ratio and say Show. So if we zoom into the same place, we see now we've got extremely high aspect ratio elements again. Let's zoom out. Let's also check the Jacobian. So come over to the Jacobian Quality Plot, right mouse click and say Show.
The Jacobian is around about 2.11. Again, it's slightly worse than before but again the Jacobian here is a very inaccurate measure. So let's set the element size back to 0.4 to avoid saving a large database. So we come into Mesh, Create Mesh, reset it to 0.4, check to run the mesh, you see that was very fast, back to our course mesh.
So we'll save off the model now, and again we've kept it as a small size model. We'll go to File, Save As, and we'll save it off as baseline_9. Now it's asking do we want to copy the result files? The result files here are actually the mesh fill plots showing us the Jacobian and the aspect ratios. So they are classified as results even though we haven't run the analysis as yet.
So the answer is Yes to that. So in conclusion we've see that the element quality can be very badly affected in difficult geometric areas such as that fillet run out. There's also a relationship between the local element size and element quality. In this case, refining the mesh actually makes the element quality worse in that problem area. We also saw a factor of 1/2 and 1/4 on element size has an increasingly dramatic effect on the size and the number of degrees of freedom in the model. That meant that the mesh had took a lot longer for the last model and the analysis was slowed down even more dramatically.
We'll be looking for more efficient methods of meshing and controlling element quality when we come to do the production meshing.
- Setting up Simulation properties and defined views
- Preparing the geometry
- Setting up a local coordinate system
- Splitting surfaces
- Defining the constraint and the loads
- Running analysis
- Contour control
- XY plots