Master modeling - SOLIDWORKS Tutorial

- [Instructor] When working with SOLIDWORKS file references it's hard to go too far without mentioning master modeling. Now in the earlier video we talked about making derived parts, right now I wanna show you how you can create sort of the opposite of that by using a single part file as an assembly to then push out new parts. So, just to backup a second let me explain what I'm talking about. Master modeling uses a master model, it's a main model which drives all of the geometry. So you can see right here I'm working with a sheet metal enclosure that I've designed and this is actually a SOLIDWORKS part file, you'll notice the part icon. This is not an assembly. And inside of that assembly I've got sheet metal panels, I've got weldments, I've also got small plates on the bottom for attachment and weld, I've many different kinds of bodies in here and many different kinds of features. I did this so that I could change my design on the fly without going through each and every part individually, after the fact, to make updates. So, once I created this assembly I then went to the parts that I wanted to export like this TOP SMALL PANEL for example. I right-clicked on there and said insert into a new part. When you do this it brings up a new dialog in the property manager. You don't usually mess with too many of the options, there's not a lot of them, but what you will wanna make sure is your template settings. So right now it's set not to override the default template. Also you can propagate visual properties. So depending on what you're doing you can do all of those options or none, it just depends on your specific situation. Once I hit the green checkbox it gives me this new part in the directory I started with and its renamed it based on the name of the body and the name of the original part. So, we've got the original part name, dash, and then the body name which I've already named before making this so that I knew what it was. So, I'm just gonna add an a after this because I already have another top small panel in there and it's open right now. I'm gonna go ahead and click Save. And you can see in the feature tree now I've created a new part, but I have this stock feature on the side, and what that stock feature is telling me is that it's referencing this solid body from another part, specifically it's referencing 18-1089 sheet metal cover and it gives it a dash one number because it's the first body that's been inserted. And you can also see by the presence of this dash arrow, that tells you that that's an external reference. So if I got up to File, Find References, you can see here that it's not only referencing the sheet metal cover that I made it from, but also the assembly that that part is located in and has references in as well. So you can see quickly this part has built up its connected references. So I'm gonna close this part right now and I already have open the final panel that I wanted to create. So, once I did that, because it was just a body I converted it back into a sheet metal part so I can my flat pattern, no big deal. But, let's say down the road I decide that I wanna do some updates to my master model. What I'm gonna do is I'm gonna go back to the master model and for this example we're just gonna change the size of this hole, so I'm just clicking on it so I can find it. You can see here that I've instant 3D turned on so it gives me the option to change these dimensions on the fly. I'm gonna change this hole from six inches to eight inches. So I'm gonna go ahead and hit green for go, I'm gonna rebuild my part. You can see here that the hole got bigger in my master model. Again, I'm working in the original master model. Now I'm gonna switch over to the model that I pushed out as its own separate part, but is still reliant on that original geometry. You can see it went through an updating process and very quickly it expanded the size of that hole, so now it's got a radius of approximately eight inches. Now I can go back, hit rebuild, Save this file and if I wanna back and change it back again, I'm switching back over to the original part. I'm gonna grab that circle, change this back to six inches, hit OK, hit Rebuild, let it go through the feature tree and rebuild, and then when I switch back over to the pushed out part, you can see it updated it again and now I'm back to the three inch radius. So you can see this can be a very powerful tool when you're trying to manage multiple bodies at the same time and wanna use one main piece of geometry to drive it all. So, you know, essentially in this sheet metal cover I'm using a few 3D sketches to define the entire structure if you will, and then just adjusting those dimensions as I need to as changes came around further down the line. So again, this is called master modeling. One thing that you do need to be careful of when doing this is if you don't have both of these parts open at the same time, they won't necessarily update. And what you'll get by that is you'll see an arrow here with an x next to it or it'll just be broken and it'll say nothing. What you'll wanna do is right-click on that part and say edit in context and that's gonna bring you back to the original master model that that part is driven from. Sometimes it's confusing what part was driven off of what. So just switching back you can always do right-click, Edit in Context or you can list the external references and find out which reference you have. You can also go up to File and Find References and see what part it's referencing to be created. So again, this is a small intro to master modeling.