Transcript for "SOLIDWORKS Mates Tips & Tricks":
Hello, everyone. Hope everyone's doing good today. Thank you very much for joining this webinar with me today. My name is Angel Palomo from GoEngineer. And today we're gonna talk about SolidWorks, makes and tips and tricks. You know, this topic is it could be as as easy as we wanted to make it, or it could be very complicated. Right? There's always a good way and a bad way, and sometimes we have our own ways of doing things. So my goal today is to show you just how to be a little bit more efficient, take advantage of some of the things that SolidWorks has to offer with regards to mates. There's really incredible updates, especially in 2026, that have come about. And so before I get started, our plan for today will be, I'll be showing you some tips and tricks for the first twenty minutes, and then I'll leave about ten minutes, at the end of the session today for some q and a. Just a little bit about me. Let me hit the next slide here. So, yes, I'm Angel Palomo. I'm based out of Dallas, Texas. I got my degree from the University of Texas, Arlington in mechanical engineering. I also hold an MBA from, the University of Oklahoma. My my experience is really along the lines of FEA simulation. I do a lot of FEA, a lot of, thermal analysis, a lot of structural analysis, coming from my background in material handling, designing conveyors, you know, truss systems, and and things like that. I do have some experience a lot of experience in in sheet metal, sheet metal manufacturing. K? Just a little bit about me. I enjoy cooking, gardening. My favorite ice cream is strawberry ice cream. Just keep it simple. And me being from Dallas, I'm a die hard Dallas Cowboys fan. So whether they're twelve and four or four and twelve, those that's my team there. So, with that being said, let's, let's get started here. So I'm going to switch over here and show my screen with SolidWorks. K. And I what I've prepared here is, something that along the lines of the in in the industrial world. Right? We've got, a a pretty a good set of components here. Let me just show you around. I've got a a motor here, a 20 horsepower WEG motor. K. And I've got a pump connected to it, a couple of sheet metal parts. And this is basically what I'll what what I would call a sub assembly that I'm gonna put it into a very a larger assembly. But I wanna be able to handle this with with some some good practices when it comes to mates. And what do I mean by that? Meaning, one of the things that I that I recommend, and this is from I would call this design intent one zero one. K? We need to be able to identify what is our base. Right? What is the heart of of your assembly? Right? We need because we wanna base everything off of that. So what do I mean by that? Well, let's do this. I'm gonna start a new assembly here. K. So we'll hit new here. We'll go in assembly. And I'm gonna throw in here a skid, which this this subassembly is gonna sit on. K. So I'm gonna go look for that real quick. It should be here. K. So let's do this real quick. K. So it'd be this guy over here. Let's do this. K. So I've got my skid. Now this is probably the most important thing. So I've already decided that my skid is the heart of this assembly. K. And I want this to be oriented in the correct way. K. So we've got two options, and this is the most critical, right, when it comes to assemblies, is we want to make sure that the origins align with the with the with this particular assembly. K. So notice that on the left, we don't have those options. We don't have anywhere to click. You know, we want to be able to fix it in in the origin. K. So you could do two things. Number one, we can just simply without pressing anywhere in the screen so right here, I'm kinda moving my mouse and I'm dragging the skid. Don't place it anywhere in in space. Just go ahead and go over here and hit the green check mark. When you hit the green check mark, k, we'll see that the skid has been placed right at the origin. So the origin's right here. K. This is the assembly origin. K. And then I've got the origin of the skid. K. So if I I'm clicking on both of these guys, and you can see that the origins are are on top of each other. K? And there's a caveat to this because when I place this, if we look in our feature manager tree here, I've got a mates folder. K. And I have zero mates. K. So I didn't do anything. I just placed it. K. So the caveat is that you can see the little f next to the to the name of the assemblies. K. So that would that stands for float. K. So if I do a right click and I select float, I am now able to move this. K. And so that could be a good thing or a bad thing. K. Because, I've added zero mates. And if we wanna have more control over this, I would recommend you to go ahead and mate this using the planes, the the base planes. K? So in order to do that, k, right, we would simply just go to your mate toolbar. K. And then we then select the two origins. K. Do that right there real quick. And then I'm gonna select the origin. And then SolidWorks should tell us, hey. Do you wanna align the axis? Or do you do you wanna flip them, or or do or you wanna select them? K. In this case, I don't want to. I'm gonna hit the green check mark to accept. And now I've got a mate folder. I've got my coincident in the origin. K. Now I can track this. I can't move it. It says select the component is fully defined. It can't be moved. K. And just like your sketch relations, right, in the assemblies, you can also fully define your mains. K. So the difference between what I just showed here and the first is that the first one when you press the green check mark, it fixes it in space. K. That's why you had the f in parentheses next to the name, but notice the f is now gone. So now this means that I've made it with along the origin. So if I select the origin here, k, and then I go find the origin of the skid, the origins are now on top of each other just like they were before. K. So my recommendation is to do it this way because now you've got a you actually got a mate relation and you've got it related to the origin. K. I'm gonna go ahead and save this because we're gonna need it later. We'll go ahead and save it here. We're gonna say call it epinar example. Alrighty. So let's flip over to my subassembly that I got over here. So the next thing I wanna show you guys is, copy with mates. So copy with mates, allows you to create multiple mates that are very identical. K. They're the same parts. I just want to do it over and over and over again. K. And that's a handy tool because, say, for example, the top of this tank, I've got this bolt pattern, and I want to add, some hardware. I want to add a lock washer and I want to add a, just a hex bolt. Okay. So what I'm going to show you here is actually, the tool itself, CopyMates, is available in all versions of SolidWorks, but the the the hardware that I'm gonna add here is it's it's available in SolidWorks Professionals. K. We're gonna I'm gonna use the toolbox. So if I click on my little library icon here, and I'm gonna head over to the toolbox, and I'm gonna go to ANSI inch. I'm gonna go to washers, and these are all built in hardware that comes with your SOLIDWORKS package, SOLIDWORKS professional. I'm gonna head over to spring lock washers. And I'm gonna go in here, and just say, you know what? I'm gonna throw in a regular spring lock washer. And what's really cool about the SOLIDWORKS toolbox is that it's gonna auto size the part itself to the the size of the hole. So if the hole is within this the tolerance that's that's been set, it automatically pick the size. So for example, if I grab him and I just kinda drag, it'll go ahead and add the the washer, and it detected the size of the hole. So the hole for this particular is was nine sixteenths to add the clearance for the half inch bolt. Right? And so here it picked the half inch washer. K. This is exactly what I want. So I didn't have to go and dig and find the certain certain size of washer. K. So I'm pretty happy with that. K. And here, it gives me an opportunity to add another one if I wanted to. But in this case, I I don't wanna do that. I'm going to go ahead, and add another hardware. So here, I'm gonna say we'll go hex head. We'll do a hex hex bolt. We'll go and drag this. K. And notice sometimes when I try to do something like this, it'll wanna get it to find the size here. Give it a minute there. And there we go. K. So, again, it automatically picked the size of the bolt. So here's a half inch 20. If you're not happy with the selection that SolidWorks made, you can actually go over here, right, and then go ahead and pick the size you want, the length, the thread length, and so on and so forth. K? In this case, it picked the one that I wanted. K? But I'm and I'm happy with this. I'm gonna hit the green check mark. K? So my goal here is that I even though this was pretty easy, I didn't have to go dig through the library and find the sizes. I wanna be able to repeat this process for all the all the all the circles here, the the drilled holes. And in order to do that, I would like to do what's called copy with mates. K. So what I what you wanna do is you wanna go ahead and highlight both of them. K. And then we're gonna say copy with mates. K. So I did a right click copy with mates. K. And sometimes what happens is if it doesn't capture, the other part that I want, you can do them all all at the same time. K. So I can go ahead and add that washer that I did it that I missed. K. And I'm gonna hit the next. So here, what we see in the in the menu is, hey. We've got some mates that you've already put, concentric, coincident, and concentric. K. So the coincident, k, right, is gonna be the washer along the the face of this, the concentric and the other both concentric ones for the bolt and ones for the washer. So what we can do here is simply scroll scroll out. K. And we can then say, alright. We're gonna select the inside here. And then SolidWorks tries to help you. Say, hey. The next phase that I'm looking for is the flat face of the tank here. So we'll click this guy, and I'm gonna select the inside of that, And then I've got my next bolt head there. K. And I could do the same thing. We'll select this, select the face, and then select the inside. K. And that just like that, I'm adding all these mates. K. It's all adding all the mates that we had, the concentric to coincident and the other concentric. K. So there this will save you a lot of time because it's a repetitive process. K. So we'll do this, and then we'll select this. K. Do this. And another thing I wanted to show you is the following. K. So here, if you take a look at my mouse, k, so my mouse pointer's got that mouse symbol to the right of my pointer there. And so when you're done making your selections, you can actually hit the right mouse button to accept. So earlier, I was going over here to the green check mark to to to to accept it, and that takes me about a couple of seconds that, you know, which is not a big deal, but over a eight hour period, it adds up. K. So if I click this face here, and then I go ahead and select the inside, and I do a right click to accept, now it's ready for the next option. K. So that is a neat feature there that will help you save time. So right click to accept. We'll keep going, and it would do the last one. Click the face here. Click here, and then right click to accept, and then we're done. K? So that is copy with mates. K? And if you look at here's all the parts. K? So they're not virtual parts of any kind. They're still parts. K. But if you go to your mates folder, it added all those mates. So we didn't have to go in there and do them one by one. K. So that is copy with mates there. K. Alright. The next thing we wanna do is I wanna show you a couple of things that, that I've personally struggled, when I was in industry, and it's really along when it comes to doing some routing, so whether it's, you know, copper copper routing or electrical, things like that. In this case, I've have a couple of fittings, okay, that, essentially, I wanna orient them at a special specific angle. So you can see here, I've got this guy here, and what's really typical about this is getting this to be perfect, right, this this routing line, this copper line here. Okay. And so what I recommend, right, is make sure to utilize planes as your primary mating source when it comes to this. And why do I say that? Because planes allows you to have control a little bit more control versus surfaces. K? The planes, you can actually slice it through perfectly through the middle. That way, you have good control over it. So for example, here, I'm able to to actually rotate this. So you can see that this this fitting is rotating. Okay. I'm not quite sure where it needs to go. And what's really nice about this is the way I sketch this, you can see that when I turned it, it kind of messed up a little bit. And so when I rebuild this, I can have my sketch line that I did auto update. K. This is very, very powerful because we don't know if the customer or your customer, you're gonna wanna change it later. Right? And so you have that flexibility there. And so once you got got it oriented the right way, maybe I wanna, you know, oh, maybe I went too far, maybe I wanna kinda put it a little bit normal here. K. We'll have rebuild that and then this route line updates automatically, and that's really, really nice. K. But once you've got it ready to go, k, I can simply, make make this this fitting, k, up against a plane. K? So for example, I wanna be able to take this plane here. So we'll say this plane right here. So we'll we'll go ahead and click that guy there. We'll make that plane. We can mate it with this plane there. And so we can then say, okay. Well, what is the angle do you want? K. Well, we can be very very picky, you know, to a lot of digits. Maybe sometimes maybe that's a little too much. Maybe we can keep it to one sixty four degrees. K. But look what's gonna happen here. It's gonna say, hey. You know, if I add this mate, it's gonna break other things. K. And so why is it doing this? Because you have another mate that's in the way. K. So I'm gonna do this. I'm gonna hit cancel. K. And I'm gonna go back and and look at this real quick and say, okay. Well, I've got this plane right here, k, that I wanna mate. K. And I wanna say, okay. Well, how about if I I can get that mate to be parallel, k, to maybe the the the mate of the of the tank here? K. Because I wanna show you a wrote a a really cool trick here, and this is what we call the quick mate toolbar. K? So if I were to go and select this plane, I can do a left click to select, and I can zoom back out, hold control, and then select this plane. I can let go. K? And then I can then say, I wanna be parallel. K. And I've got that mate there. K. Whereas earlier, I had to go all the way to the mate toolbar, k, and then come back over here and then go ahead and start making my selections. So take advantage of the quit mate toolbar as well. K. So there you go. I've got my mates my mate my planes mated. I'm gonna save this to save my changes. K. Another cool mate trick that I wanna show you is called the profile center, and this is one of my favorites, just because it saves basically, you get three mates in one. K. So what do I mean by that? So here we got some structural components. You've got some c channel and a foot, that's holding up this tank, and now I am in need of another structural member. In this case, I'm gonna use some square tubing with another foot to hold a fan that I'm gonna add. K. And so I I need to create that. K. So let's do that. So I'm gonna go ahead and create a new sub assembly, and then I am going to go find square tubing here. So let's go ahead and go to here. See if I can find this real quick. Do this. There it is. Should have just searched that. K. And, again, I'm gonna reiterate the following here that I don't wanna place this tubing just in space. I'm going to essentially hit the I'm gonna hit the green check mark. And notice the f means it's fixed, so I'm gonna go ahead and float it. And then I'm gonna make its origin with the origin of of the assembly. So really quickly, use a quick make toolbar. So click the origin, hold control, click the origin, let go, and then add a coincident. K. Just like that. And I'm gonna save this real quick. I'm gonna save it as square tubing assembly. K. And now I'm gonna bring in one more component. It's called the foot. Bring that component in here. And in the past, in order to mate this foot, I wanna put this foot right at the very bottom of the square tubing. So I would do a coincident mate, then I would then I would mate this face with this face. K. And then I have to add another one that centers it. K. So let me show you that how that would be. K. So first, what I would do is I would select that face, select this face. We'll do coincident. And then I would like to center this, so I'm gonna show you the with mate. The with mate is also available in the quickmate toolbar. So if I click this face, turn it apart, hold control, click that face, and then I'm gonna hold control again and select these two faces, let go, and then you have the quick made toolbar. Here's width. What that's gonna do is gonna center the foot between this those two faces, so you don't have to do any math of any kind. K. So I've got one more. So I'm gonna do that one more time so we can see that. So select these two faces by holding control. So there you go. Then hold control. Click these. Let go. Width. Perfect. And you can see my assembly is fully defined. So that's great. Right? That took a lot of work though. If you look at your mates, we've got the coincident, the two widths. K. So what if we could do that easier? So let's delete those mates. Gonna delete them. Yes to all. K. Let's bring this over here. What if we do this? What if we click that face? Click this face, let go. We've got this other mate called profile center. So it's gonna take the two shapes, find the center of those, and make them. K. And there we go. Fully defined. Same exact thing, but I I got it done with one mate instead of three. K. We'll hit save, and we can then come back to our assembly. We can enter that component. K. Right. And then pretty quickly, again, just as a summary, use a quick make toolbar. Click the faces. Make them coincident. One thing too that I wanna show you guys is you can actually rotate the component itself. So normally, the middle mouse button turns the whole part. K? But you can actually just rotate the actual the actual part itself, the sub assembly. So for example, this, just hover over it, hold down the right mouse button, and you can reorient it, so without turning everything else. K. So we could do that as well. So that's very helpful. You wanna get things aligned and kinda try to see where it's gonna go and drag this without messing around with everything else. So the right mouse button, hold it down, you'll be able to turn that. K. You also have distance mates available to you with the quick make toolbar. So if I click that face there, hold control, we'll let go. We'll do distance. K. Maybe we wanna be seven away from there, and then I click this face and this, this face here, let go. We'll have a distance meet. Maybe we'll put that as a foot away. K. So just like that, I've got my structural member that I'm gonna use there for later. And you can see right here, I got fully defined. So fully defined also is also an important thing, within SolidWorks. Make sure that everything is fully defined. You don't have you're not missing mates or things are loose out there, and that's gonna be a good way to keep track of just the the integrity of your of your modeling. Right? You wanna make sure that when somebody opens your model that nothing breaks or things were flying out in space. It happens, but if you follow these these practices, you will not have a problem with that. K? So alrighty. Well, that that went by pretty quick. So it's, two twenty three central time on my end. So are there any questions, for me? I'm gonna look I can look in the chat here, and that can answers. Alright. So I've got a question here for Mark. Is there a benefit or downside to the other way? And I'm assuming that's, when it comes to fixed versus aligning the the aligning the the axes and and meeting the origin. In reality, I would say there's one upside to mating the origin because you have more control. I'm more about control, and if you have a good process within the the engineering and drafting department, make sure that everyone's meeting the origin. We at least understand why something's not moving, and we understand that the f means fixed. Right? If you float it and everything's based off of that, if you unfloat that, you start moving the part around, and then it's just gonna cause all kinds of of of errors because of all the relations that were added. K. Looks like Gary had a question as well. Are the x y z planes aligned? Yes. When you do the when you made with the origin, it'll align the the planes. So if you do the design intake correctly, so the front plane will be aligned with the front, top with top, and then right with right. K? Gary, you got another question. So why not pattern the the fasteners? That's a great question. The fasteners state, a lot of times what happens is maybe in this case, it would have been a great great idea to do the pattern because it follows a bolt circle. But maybe something like this down here, where the there is no pattern. There's just holes everywhere and it's and actually has different sizes of holes. Right? We can we wanna be able to maybe utilize copy with mates because it's more of a guaranteed that you'll have everything at your disposal, especially when you're using SolidWorks Professional in the toolbox. Just drag and drop some of the fasteners, then you've got for example, these two holes are the same and these are the same. So I'll do one and then copy with mates and do the rest. But, yes, absolutely, you can do you can pattern the fasteners. K. Looks like, we've got another one. Gary, when you delete a part from the assembly, is there an efficient way to delete the old mates? You know, that's a good question. I wouldn't say there's a an efficient way. We just have to make sure that we go back and delete. Yeah. It's just it gets tricky when you have a lot of different parts that are related to the the one that you're deleting, so there could be some that are kinda still lingering. So, the one that comes to mind is a lot of them when it comes to distance mates is what what kinda kinda gives a little bit of trouble with that. I think if we if we just one of the things that I would recommend, at least for that is make sure that when you have when you're looking at your feature manager tree here, take advantage of the main folder. So every every part, every assembly has a main folder. So for example, this bay baseplate sheet. K. It's got all these mates. So these mates are all related to in some way, shape, or form to base plate. K. And that's gonna be that's important. So if you wanna go and troubleshoot some things, go to the part that that was removed, right, and see what parts were related to that. And that's that'll help you try to figure out what was related, and they'll help you troubleshoot that. K? So hopefully that answers that question there. Alrighty. We got time for maybe a few more questions here. Let's see. Okay. Question from Glenn. For the support post you added, how to transfer the holes into the base? Okay. That's a great question. So for that, you would we would need to do something called in context modeling. So one of the one of the ways to do that, and there's a couple of ways. The first one is we would need to maybe draw we need to draw the the cutout within the assembly. So we we would start a sketch within the assembly and then cut through the foot and then cut through the cut through the the base plate here. That way those two will get that hole and it'll project both of them. And then when you get to the part file, it'll have both holes. A lot of times that it's not desirable to do that because it's hard to keep track. It's all about keeping track. So what I would recommend, which is something if you guys have are interested in is what we call smart features or smart fasteners. K? So what that does is you can configure, a a piece of hardware, a bolt, k, that has specific cutouts. Like, for example, we wanna do a cut extrude. So whenever you drop the the fastener in, it'll actually go ahead and cut through the parts where you made them to. K? And I can send there are some really good blogs out there that have that have been written about this so that we can set up one, and I encourage you to try that and see if it does what you needed to do. Because if you wanna do it that way, you can then also customize your SolarEdge toolbox to do that as well. So that way the the holes will propagate to not only just the foot, but any other component where that bolt touches. K. So check out smart fasteners. K. Perfect. Alright, everybody. Looks like we ran out of time. So one of the things, obviously, reach out to us. We've got, you know, over 250 experts in SolidWorks to help to help with things things like this. If you guys have any questions, you can always reach out to us for any help. Check out our website. Make sure to take take advantage of our blogs that we have out there for anything that I've covered today and anything along smart fasteners and more tips and tricks on other topics. Okay? Thank you very much for your time. Enjoy the rest of your day, and have a great weekend.