In this video, learn about other types of load and boundary conditions available.
- [Narrator] The functionality we're going to be describing in this video is load case manager. Just please note it's only available in SOLIDWORKS Professional and Premium Simulation options. We often want to apply multiple loading ingredients to build up a sophisticated load case, such as the Comrade tensile load case. This case combines bearing forces and inertial loads. We'd also like to run several load cases in one analysis, such as the tensile and compressive load cases together.
A SOLIDWORKS load case manager enables us to do this. Right mouse click on the study icon in the analysis feature tree. We're going to choose load case manager. A new panel called load case view appears below the model view port. The contents look similar to a spreadsheet. We've got four main columns which represent the constraint and the three load objects that we applied, the compression, the tension, and the axle acceleration. The icons show the form of the loading objects, and the names we have applied have been picked up and displayed in a spreadsheet.
Notice the acceleration is being expanded into three columns for X, Y, and Z directions. The values in the cells represent the total load or acceleration value that we applied in each case. We can control the entities we see in the spreadsheet with the selected icons. I can display everything. I can hide the constraints or the fixtures. I can hide the loads, and we haven't got any connector loads, but again they can be hidden or displayed, so let's show everything again.
We're seeing both our loads and our constraints. There are two options to create primary load cases, and also combinational load cases, or load case combinations. The two terms aren't very helpful, so I'll try and expand on their meaning. In creating a primary load case, we can select or suppress any of the component constraints and loading definitions. We can also refer to these as constraint or loading objects. Click the plus next to the entry which reads click here to add a primary load case.
The begin constraint has a check sign indicating it's selected. Then the other three loading conditions are either selected or suppressed with a total load or acceleration. We'll set up the compressive load case first, so click in the load case one cell name here, and change that to compressive load case.
Now if we click on the compression load case here, next to it is a dropdown and we have the option to either use the total value, which is 26430 or we can suppress it. In this case, we're going to select the total load value of 26430, and that's the compressive loading object which is now included. Now the compressive load case only has this loading object, so we're going to go along the rest of the row and simply suppress, so suppressing the tesile load and the actual accelerations already suppressed.
So that's built the first load case, compressive load case which consists of the constraint we need which is the big end. In particular load object we need which is the compressive load. We click again to add the new primary load case. Let's rename this as tensile load case. Now we move along the row, we want the big end constraint as ever. The compressive load is already suppressed.
I want to make sure I invoke both the tension load, which is already selected here, and again, you can see from the dropdown, I could either have that value of minus 14,300 or I could suppress it, so I want to keep that as an active load. I also want to unsuppress acceleration, so I click on the value that was calculated, so this is in inches per second squared, also the load is impound force. I don't have any accelerations in the Y or Z directions, so those aren't really relevant.
So we've created the tensile load case, which is made up of the constraint at the big end. The tension load which is being applied is a bearing load on the left-hand side of the little end, and the acceleration loading, which is present throughout the Comrade body. Now the spreadsheet can be a little unstable, so just check before you exit that everything is set up as you need. I could change the values here on the fly, so I could come into here for example, and if I just remove one zero, then I've got 90 and 320.
I'll add that back in quickly so we don't make any mistakes, so the idea is any of the values here could be changed on the fly. Now I would strongly recommend you don't do that. If you do it, there's no real paper trail or a reminder of what you've done in modifying the basic load object, which for example is the tension load here, or indeed there was the actual acceleration and converting that to a different value. That's really not a good idea. So what I recommend instead is you treat these as the final operational load cases.
Don't adjust the values here. You leave them intact. That's just standard good FEA practice. Now if we want to scale, and indeed if we want to combine load objects, that's where the load combination option comes in. So load case combinations is where I would go in and change that number there, and you're going to see that it's become an equation form, so I can say that acceleration times point eight, or that acceleration times one point one. Whatever I want to do, but it preserves that object for everybody to see exactly what it is.
We haven't kind of messed around with it. Under the covers as it were. Let's imagine for a moment we want to apply an extra load case which factors up the acceleration by 20% and reduces the tension load by 80%. So let's create a new primary load case, which I'm going to call a unit load case, 'cause I want to break out the tension load and acceleration load as separate cases, so here add a new primarily load case. Let's call this unit tension, and here I'm suppressing everything other than that tensile loading object that we applied, the minus 14,300 off in this direction to the left.
So that's what I call a unit tension. Now unit doesn't necessarily mean one-pound force or one acceleration per inch squared. It really refers to a fundamental case, so this now becomes our fundamental unit tension case. Let's add another load case in here, and let's call this the unit acceleration. So the idea here would be to suppress everything other than that acceleration case.
And again, although I've called it unit, what I'm really meaning is it's my fundamental case, so I've gpt a fundamental unit case in tension which is shown here. I've got a fundamental unit case in acceleration which is shown here, and these are now decoupled. They're separate, so what I want to do now in load case combination is combine these unit cases together, so let's click on the plus next to click here to add a load case combination. What happens is a new dialogue box pops up, and it requires an input equation.
Now I think it's easier just to start with a new equation, so we just delete the whole line out. You can see the functions that we want to apply down here. The functions meaning our individual load cases, so we want to take unit tension and for the moment, let's just add it to unit acceleration, so that would be 100% of unit tension plus 100% of unit acceleration would form this new load case, which I haven't named yet.
So we want to do a little bit more than that. We want to apply a factor on that, so let's apply one point two times unit tension plus not point eight times unit acceleration. So that equation is controlling in my particular case unit tension and unit accelerations. You can see if we have fundamental load cases, it's easy to manipulate them. So check the box there and I've messed up on multiplication there, so it's warning me.
What I forgot to do was put the multiplication in, so we have an operator there, and we also have an operator here. So there's obviously a syntax that we have to stick to. Now it's happy and you can see it's put the equation in here. Now I just need to name this, and I'm just going to call this operational case one.
You can imagine I have many operational cases, which are made up of different combinations of these fundamental load cases. With something like the aircraft industry, they can literally have thousands of different load cases built up of different unit load cases, so now this becomes a very attractive way of working. It's also very attractive in the sense that it has a great paper trail. What if my operational case one is made up of one point two times unit tension, plus point eight times unit acceleration. I've not gone in and manipulated directly the loading object, so this is a much preferred approach to be taking.
Unfortunately, the results created by the primary load cases and load case combinations are not spawned in the usual way in the analysis feature tree. We have to explicitly set up and control these results from this load case window. So if we move down here, we can click on the paths next to track results. Click here to add a sensor to track a result. So I click on that and we click on add sensor. Now we have the usual controls to set up different types of responses.
Now we're going to set up the default which is sitting here which is upon my stress, so the stress quantity, we could select any of the more normal quantities that we have available. We're going to pick stress. Again the component I'm going to be using is upon my stress. Again, check if the properties are in the right units, which it would be PSI. Again, we can choose what particular criteria we want to apply or step criteria. We're going to leave those as defaults.
So this is a special form now to set up result quantities for the load case view. Now if I check okay at the top of the form, now my result appears here, so results stress one upon my stress. I'm going to create a second sensor in exactly the same way to look at the X direction stress. So I add sensor. The form pops at the top here. Again it's stress I'm looking for. This time I'm going to change it to X normal stress.
Once a coordinate system, so again I can come in here and select the it land coordinate system. Just check the units, which I want to be in PSI and we click okay, and we see stress result number two. Finally, I'm going to add a third sensor, so click here, add sensor, and again simulation dates, and what I'm going to choose is the displacement quantity, and I want to choose the results in displacement.
I could choose component X, Y, or Z. The result makes more sense here. Then check the units would be in inches, and click okay. So these are my three result quantities that are going to be spawned when I run the analysis from the load case view here. Now one thing I'm going to do is just get rid of this operational case down in here, so we just delete that.
I'm going to suppress in here the unit tension. I'm also going to suppress unit acceleration, so back to just the fundamental cases we looked at before on two separate analyses before, which is the compressive load case and the tensile load case. Now at any point, I can shut down this load case view, but then I could get it back again by under the load case manager, I can just say view or edit the definition.
So that summarizes the kind of controls we have there. Now in a following video, we're going to be showing how to interpret the results coming from the load case manager, but for the moment we'll stop there. Now there are some limitations using the load case manager, and I'm hoping SOLIDWORKS will develop it out further. That fact that we've got to look at canned results created is perhaps one major issue. The second is that I can't go in and do for example X, Y, and Z. But for the moment though, it's still a very powerful methodology.
So for the moment we're going to save the model as baseline eight. So in conclusion, we've seen how to manipulate the basic constraint in loading objects into a set of load cases using the load case manager.
- 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