Join Gabriel Corbett for an in-depth discussion in this video Standard Mates, part of Cert Prep: Certified SOLIDWORKS Professional (2015).
- Once I have all the parts into the assembly, now I'm ready to start adding some mates to control the look and shape of this assembly. So first things first, I'm going to go ahead and add a mate, right here. I'm going to hold down my right mouse button and spin this part around, and I'm going to get it close by to this pin. The first thing I do whenever I'm doing an assembly, is get the components close to the right orientation, and location of where they're going to be mated together. Then I'm going to jump into the mate toolbar, click on mate, and click on the outside of this pin here and the inside of this hole.
Now, If I didn't want to do that I could also choose the outside of this with the outside of this. Go back. There's a lot of different options of how you could mate things together, and choosing the right option. The best thing to do is to say it out loud. I want this hole around this pin. I want the top of this pin flush with the top of this part. And that's my selections as I say them. Now, notice this still spins around here so I have a degree of freedom. And if you click on this part itself, you can see there's that little minus sign directly in front of it showing that it's not fully defined.
So what I might want to do there is maybe choose one of these planes, in this case here it would be the front plane. Choose a mate, and I'll say maybe the side of this part here and make them parallel. Now this part, if you click on it again, you could see there's no little minus sign in front of it showing that it's fully defined. This one's also fully defined and notice the little F in front of there showing that that part is actually fixed right at the origin because the first part we brought in. If for some reason you wanted to unfix that part, I could right click on it, and click on float.
But then I would need to add some other relationships and other mates to define where that is in space. The next part I'm going to add here is I'm going to rotate this piece around here, and get it close to where I want to be so I'm going to drag this up close here, and same with this pin here. Click on mate, I'm going to say the inside of this hole, the inside of that hole, mate those together. Then I'm going to choose the side of this and spin my assembly around, and the side of that. There it is. And then pick the pin, the outside of the pin to the inside of the hole.
And then the end of the pin to the end of the hole. Now, notice it chose that edge, and generally don't try to choose edges, so go back on that one and choose the face to the face. You're always going to get a stronger mate if you're choosing full faces versus edges or points. Keep going with this assembly. This time I'm going to add a mate between these two here, so I'm going to say the inside of this hole here with the inside of this hole here, mate those together, I'm going to say the top surface here to the inside here, and mate those together, and then take this pin here and put it inside that hole.
Once again I'm going to choose the top surface here, going to mate with the top surface there. Alright. Now this pin here, I actually added one additional pin that I didn't really need. So it's okay to just go ahead and delete that pin out of the assembly. In reality I need this pin here, so go ahead and click on control, and drag another copy out, and then I'm going to take this pin here, add a mate to the center hole there, and maybe from the bottom here to this. And there it is.
Those are all of our mates that we need for right now, but now I want to make sure that I could move things around. Now this is very similar to the example you'll see in the sample exam. But I wanted to find now, some angles. So the best way to define angles, I'm going to come up here to mate, I'm going to choose the top surface here, this top surface here, and then define an angle. Notice it's giving me 154 degrees. I want about a 30 degree angle between this top surface and this one, but it's really -- looks like I'm fairly close to that 30 degree angle, but it's choosing me 154 degrees.
Now I could flip that dimension and then put it on the other side, but that's not really what I want to do either. So sometimes the way you define the dimension or the angle is not the same in SOLIDWORKS as it will be on the exam. So in this case here, it's actually 180 degrees minus 30 degrees which is at 150 degrees. So keep in mind you might have to do a little math, and type in 180 degrees and then minus the 30 degrees to get you to the 150 degrees. There it is. And then over here on the side, I'm going to mate these two surfaces together as well, give it an angle, and this time I'm going to say 115 degrees.
Now you could see, everything is pretty much fully defined in this assembly now and now I could go ahead and figure out where the center of mass is. So to do that, go over here to mass properties, looks like we need to update it first. So go ahead and update. And let's go ahead and save it as well. File, save as, and I'm going to call this 2.14_FIN. Okay, now we can go over here and weigh it.
And you could see my mass, volume, and center of mass. Notice this is in inches, and that's wrong. We want to make sure we go up to options, choose custom settings, choose millimeters, and I want to make sure I'm choosing grams, with two place decimal, and click OK. And I could also change that down here, millimeter, gram second. So depending on which template you use to start your assembly, it could be in the wrong unit. So make sure we are putting that in correctly. Once I've made those changes I need to go back, exit out of that window and then do it again.
And now you could see, actually my volume is still in inches, so that's a little bit weird let's make sure we double check and look at that. So here's our cubic volume, and we want to be cubic centimeters squared. Click OK, and there it is. Now, center of mass. It's in millimeters so that's exactly what we want, I'm seeing a two place decimal, these are the values right here that you'd be putting in to the exam to answer it. Once you have those values I would definitely recommend leaving this dialogue box open, and then just typing in or even copying those values directly into the testing window, to make sure they're correct and verified.
And once you've done that, make sure to close out this window, do a rebill on your assembly and then just do it one more time just to double check they didn't change. I've seen a couple times that the assembly didn't quite update, or something was a little bit slow, and the values actually changed. So make sure you double check your work finding the center of mass or the mass of the part because sometimes there's a little bit of a lag or the parts aren't fully rebuilt, and you're not going to get the right values. So again, double check those values just by pulling it up twice. There's a ton of different mate types and methods for building an assembly and it really depends on what the parts are you're going to try to assemble together.
We've covered some of the basic assembly techniques and mates, and you might want to go through and do a couple practice assemblies making sure that you can quickly add parts, mate them together, and adjust angles and orientations.
He also breaks down the three segments of the test (part modeling, configurations, and assemblies), providing strategies that will help you pass each section. At the end of the course, there are two sample exams to practice what you've learned.
- CSWP requirements review
- Working with sketch entities, tools, and relations
- Using the boss and cut features
- Performing sweeps and lofts
- Smoothing corners with Fillet and Chamfer
- Creating linear and circular patterns
- Setting up equations
- Creating multibody parts
- Setting mass properties
- Working with materials and constraints
- Inserting components
- Setting up reference geometry
- Arranging features to change the part
- Working with suppression states
- Using a design table to build configurations
- Establishing standard drawing views
- Annotating your drawings