In this video, learn to set up and run an FE analysis.
- [Instructor] Having defined the material, the loads and the boundary conditions, and also meshed the model, we're now ready to run an analysis. We want to check out each of our loading actions independently. So right mouse click on compressional load, and suppress it. Do the same with tension load, suppress that. That leaves the axial acceleration as the only active load in our particular load case now. At the moment the acceleration is set at 500 G, if I reset that to one G, then we can balance that against the weight.
So reactions that come out of this should be equal to the weight of the structure. Let's go in and modify that, edit the definition. And the acceleration due to gravity is 386.4 inches per second squared. Check the box there. And you can see it's nicely reflected in the title here. Now we can run the analysis from different positions. We can use run this study, we can go to simulation, run.
Or we can come over to the study and run from there. Command manager option here is probably the easiest, so let's click run the study. We'll see a monitor window appear showing the status of the analysis. Let it run very quickly, and we see the initial results. The default result is Von Mises stress, this is the stress plot we're looking at here, stress one Von Mises. You can see the maximum value is very small, because it's just basically one G being applied to this.
At 3.7 PSI. We can also see the deflected shape just here as well. So these settings we see here are based on defaults, and they've changed since SolidWorks Simulation 2016. You may want to set back to our original configuration. So let's see how we can do that. Go to right mouse click here on the result plot, stress one Von Mises. And then we have chart options. Chart options is our main control for a particular plot view.
So click on chart options. What we can usefully do is to set the maximum and minimum so we actually see where they are. We did that, if you remember, for the element quality plots. You can see they pop straight away as little window boxes. Now what I want to do is to say in the definition, I don't want to see a deformed shape straight away, so I'm going to click that off. And also in the settings, there's a couple of important settings here. At the moment, we have a continuous view of the stress.
Now I don't particularly like the continuous view of the stress without seeing the mesh, because it gives me no idea of the quality of the model underneath the scenes. So, the continuous view, as indicated here, is a very photorealistic kind of view, and it can kind of distract us. Things aren't that smooth, things aren't that accurate. So if I change that to discrete, then it's going to give me a more banded kind of approach, which is the more reasonable representation.
I always also like to see the mesh underneath a structure. So we can change the boundary options from model, which are the boundaries of the model, to being mesh. And if I click that, now we can see the mesh coming underneath. That gives me a much better feel for what the element distribution is doing, and what the stresses are doing. If we go to the little end for example, I can see the distribution of elements, and I can see the mesh associated with those.
Now again we want to switch off the deformed shape, we click okay, and now the deformed shape is gone. So let's get a standard view. And that's really the starting point I like to have for any visualization of stress results. Not the photorealistic, not the deformed shape straight away, let's just go look at the stresses. Now as I mentioned, the peak stress is round about 3.7 PSI. What we want to do is to check the reactions coming out of the big end here.
So I can right mouse click on the results icon here, and go to list result force. Make sure the reaction force radio button is selected, and for the coordinate system, we can drop down the geometry feature tree and choose little end, close that back up again. And we want to summate the reaction forces which are going to be on the big end, which we find on these two surfaces here.
So I can click update, and I get a little spreadsheet in here which is giving me the reaction force summary. So the total sum in the X direction, which is our axial direction, is 18.7 pound force. It's almost zero, it's computed zero in the Y and Z direction. And that's great because that checks with the actual weight of the structure which is 18.7 pounds. As we mentioned in the intro, this is a very heavy con rod from an industrial engine.
So that's a fundamental check out, load in equals load out. So our acceleration of one G, force equals mass times acceleration, is giving us the correct weight in this particular case, or the correct resultant force. Let's check okay, go back to the graphics window. And we want to put in our full operational loading case. So if we right mouse click on this, edit the definition. Very handy trick in here is we can just put in times 500, and SolidWorks dialog box will take an expression like that.
It's very powerful, very useful indeed. So we check the box there, we're back to 139,200 inches per second squared, which is 500 G. Let's just re-run that, we know it's going to scale up, but just out of interest let's run it and see what the stress results will be. Just for a change, I can right mouse click in here and say run. We see the monitor window coming up. It's complete. Now we go to our new results, and now our new results loaded in stress one, we can see it's round about 18,000 PSI.
And again, with the max label switched on, again I can drag this away nicely so if we want to create a report you can show this nicely, it's around this kind of pocket region in here. So the compressive load case, we talked about, that's squeezing the con rod and giving us the maximum stress in here. Now we can also control these other responses, so the displacement response for example, we can go in and say, chart options, similar kind of way, again I can control the different definitions in here.
At the moment I can control and put on a deformed shape. What I can do is the automatic shape which we saw very briefly, is a huge scaling, and we saw a very deformed, or grossly deformed shape, so let's change that, and let's try 60. There's an option here, that's the deformed shape. Let's check that. So here's our stress result. We want to overlay the deformed shape plot on top of it. So very useful shortcut control here is just go to the deformed result tab, click on that.
And now we see our deformation. Now it's scaled off a little bit, so we can just drag the model over, and we can see, we've got again a highly exaggerated deformation of that little end. The big end isn't deformed at all because remember we superglued it down to ground. Now we can check the tensile load in the same way. This is the loading developed by the piston assembly, pulling against the little end pin being reacted through the crankshaft. So now we suppress the acceleration input, and unsuppress the tension load.
This is the only active load that will be considered when we run now. So let's re-run that analysis. Let's click on run this study. See the monitor window again. And now our results option has plotted out again. And we have a highly exaggerated result here, because we have deformed results switched on, so let's switch it off. And we're back to our loading distribution.
Now the peak value here is round about 37,000 PSI, and the smallest value at the little end is a tiny little value there. Let's zoom in to the little end. And we get a feel for where that stress concentration is, again I can move that out of the way so I can see very clearly what's going on. Now the deformed shape, again, was highly exaggerated, let's come on to right mouse click, chart options.
Under deformation, the automatic scaling is a very large scaling, so again let's go to user defined, set that to something more like, say, 60. Click okay. We won't see any deformation at the moment, but if I click on deformed result, then we see a better visualization of the deformation. Let's go to the standard view.
And you get a sense of that deformation. Now one thing we want to do again is to check the reaction forces equal the load applied. We know the load applied is 14,300, so again let's come to results, right mouse click, and say list result force. We can again check the two reaction faces here. Click update.
And you can see we're getting the 14,300 pound force out as a reaction. So again, load in equals load out. Any reviewer, any checker of any analysis report, that's one of the first things he's going to look at, is did the analyst check load in equals load out. So that looks good, check okay. So we can see the sense again, it's going to be that tensile load applied at the bearing face here, that's giving the big local stress concentration at the little end region.
So we want to complete the picture, and check the compressive load. So right mouse click on compression, unsuppress that. Suppress the tension load. And now we can re-run the analysis. The results pop. We're getting a stress concentration of about 16,000 this time. It's in a different position, it's now in the bearing face of the little end.
Let's zoom in and see that a little bit better. So the stress concentration, again, shown in this region. It was the tensile case where we had the stress concentration in this region. Again, let's check the reaction forces, so in results, right mouse click, and say list result force. Let's go to the big end. Pick these two reaction surfaces. Click update.
And we have 22,018. Now it's interesting because that value is less than the 26,430 pound force we defined as the total force applied normally to the surfaces. To apply the correct distribution and hence the correct force, we would have needed to calculate the projected area on the axial direction and then apply that as a pressure. I took a shortcut and applied a normal force. So I've got to correct that to apply the correct axial net force.
So we can scale that directly in the loading input. So we come back to this compression load here. We've applied 26,430, but that's in a radial direction rather than a component X axial direction. So what we can do is to scale that, so let's go to edit the definition. Now, 26,430, if we scale that by the ratio, 26,430, divided by 22,018, 22,018 is the reaction force we got, we want to scale it up to 26,430.
Now what's handy is if you've done that calculation, say, in an Excel spreadsheet, you can just copy and paste that again directly into this expression window. So it's very powerful. So that's updated the force. Again we can see an updated value in here, which is 31,726. That value of 31,726 which is applied as a radial force distributed over this region, if we knew the area then we could work it out as a pressure, that's going to give us a net total reaction force we anticipate.
And let's check that out and re-run it. Let's look at a general view. Again, now we can see that the peak reaction has obviously increased, it's in the same region as before. Let's go to the little end. Again we can see it's on that inside bearing face. Now what we need to do is obviously check those reaction forces, make sure that they're what we expect to see after we've done our calibration.
So let's go in and list result force. Again let's go to the standard view so we can pick off those two reaction faces. Click update. And we've got 26,429, well we're expecting 26,430 so we're one pound out, out of this large number. So, it's a reasonable level of accuracy, that's okay. So we've actually calibrated the model in that particular case to get the right reaction force out. So again, load in equals reaction force out.
So now let's save the model. And we'll save this as baseline 12. Again, it's asking us, do we want to copy the results, we now have a significant amount of results, do we want to copy those over into the database. And the answer to that is yes we do. So in conclusion, we've checked out each of the individual loading components that we're going to apply in the final production analysis, in particular, inertial load calculation is shown to be correct and balances, and the compressive normal applied force has been calculated to give the correct reaction.
- 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