Expert Modeling Tips and Tricks | SOLIDWORKS Webinar

my name is Jeremy browning I'm an application expert here at mlc CAD systems basically what an axon expert is is just a super nerd I am my last job I design machines that made artificial DNA for drug research those machines are actually getting put they're put through their paces now if you're counting children in that picture that's three yeah sleep is not a thing especially when we're all at home everyone all tensions are high a little bit about MLC we're one of the largest VARs in the US and what I want you to take away from MLC is the fact that we do tech support a little bit differently so if you've ever called in a Comcast or AT&T for tech support that is Tier one tech support we don't do a Tier one you call in you're going to get someone like myself on the line and you're not going to hear me something through the pages and saying did you reboot your machine II respect your time I understand that you might have a very hot question so we will start answering a question right away if you're not too familiar with MLC cam systems this is our territory we do go all the way up into the Pacific Northwest all the way down into Florida so every state that you see we sell either SolidWorks master cam or 3d printers and more specifically the Mark Forge line of 3d printers now what I want to model today is a speaker this is a nice screen shot of a speaker and it's really good to send to maybe prospects or maybe your customer that you're working with it's very good to send that but let's model it from scratch now I want to prove to you that this is a real speaker so here's some pictures of a speaker that we designed here in our Dallas office so we 3d printed these on some awesome machines we print it a couple different versions some carbon-fiber ones some clear ones and these things actually sound really good but we have some design challenges along the way and I want to kind of walk through how to model this speaker and some of the higher-end tools and SolidWorks that you could use so just for your own information we did run some simulation on this speaker and you can see at this point we were looking at the airflow through the port and how fast that air actually flows through that tube another thing we looked at is the speed of the air going around all of the devices inside this speaker so there's a lot going on inside the speaker we got to really put our engineering caps on and figure out are we going to have port noise there's a bunch of parameters that we had to design around in this simulation you'll see that we actually are building a surface anywhere that this that the airspeed is going too fast and it's going to create noise so one thing that we had the design around was actually having this speaker be between 300 and 350 cubic inches internal volume so here is a completed design and you can kind of see this speaker here model this is fully populated the assembly is complete but what I'm going to do is I'm going to model this speaker completely from scratch every one on here is a Salt Works user and at the end of the day you're going to have to hit file new at some point and model something from scratch so no tricks up my sleeve we're going to model it completely from scratch so let's do that I'm gonna go ahead first I want to point out that there is a front piece and a back piece they slide together with these lips you can see that they they slide together and there's 20,000 sub tolerance a gap around the sides so that they actually will fit for sure so I'm gonna close this thing completely I mean you can see the SolidWorks 2020 emblem there's nothing open so let's hit file new and choose a part in inches freedom units now I'm gonna talk about good practices as we design this as well so not only we're going to model it from scratch we're going to talk about best practices and good things that you should be doing while modeling one of the things I like to describe that you won't see in any training manuals bulletproof modeling so everyone on this webinar has probably opened a model that their co-worker made a change to definitely not you definitely their co-worker made a change too and one small change just made the model explode well if you have bulletproof practices bulletproof modeling skills that change should not blow everything up you should be able to go in make small changes and your intent drive the way the model changes so with that in mind let's go and let's define some sizes up front and to do that I'm going to use equations now if you don't know there is a search command up on the top right of SolidWorks so normally it's on help you can switch it with this little arrow to commands looks like the DOS prompt a little bit outdated but we all know what that is and you can type equ and you can just click pound equations or you can hit the eyeball and especially if your co-workers asking you where it is it'll give you a nice big red arrow and say here it is and then you can just walk away and triumph well let's fire off the equations the first thing I want to do is I'm going to design this speaker where we have four different values and then a radius so we're going to have a top and back with for both the top and the bottom our front and back for both the top and bottom so first of all we're going to have a height so H for height and that's going to equal 7.5 now I've already worked all these dimensions out just so that you guys don't have to see us tweak everything but one thing that's really good about making equations is you have a one-stop shop to change every single value now you don't have to go into every single sketch and make all these changes all you have to do is come in here to the equations so H for height and then I don't even have to put all of that I can just put D for depth and then I can say I want ATF for top front and top front is going to be three point two five you guys get to see it typing exercise today so top front and then I'm going to have a TB and that's going to be top back and that's going to be two inches this is a really good practice if you've ever opened anyone else's model and you're like what the heck did they do this is a really good way to document everything that is going on I'm gonna have another one called B F and this one's going to be seven and a quarter and that's going to be bottom front and then another one called BB and that's going to be bottom back at five inches all right and then I'm gonna have one more we're going to call this curves so we all like nice smooth curves on our models and that one's going to be equal to 20 all right now we've got all these dimensions defined already and once you've defined these equations or these global variables you can find them under the equations folder with all of their names now you don't have to use just letters you could use phrases if you wanted to obviously you see that with curves now in SolidWorks most solvers that users we like to make box we extrude box we pull page we pull out a page we make box it's very easy we make very orthogonal or geometry shapes right but some of the hardest things to do are in fact those curved shapes and if I open this model up again you'll see that there's a lot of curvature to this model you can see it's curving in multiple directions and so this is some of the things that people will get a little timid about and we need to be able to have all those tools in our tool belt to be able to make shapes that are not just real real blocky and the extrude box so we're going to do that here in this brand new file now I'm going to create a sketch on my top plane and the first thing I'm going to do is I'm going to use this midpoint line this midpoint line this is a really good one especially if you need symmetric symmetric parts to build around your origin so at that point I just started with the midpoint line now I'm going to use a regular old line now this is going to be the depth now in case anybody didn't know you can click on a line you can say for construction geometry and switch it over to a piece of construction geometry and then when I draw this other line I could use a midpoint line or I can pick up this midpoint reference and make it coincident with the end here which is perfect now I'm going to pick up a three-point arc here so three clicks is what it takes said the Cookie Monster so there we go we have our original shape now I need to define this because best practice is to always work with fully defined sketches this is an under defined sketch as said in our status bar down here in the bottom so I do need to define this so this one is going to be equal so just like in Excel when you hit the equal key that is going to show us every we can link this to or start an equation in this case I'm going to go to global variables and that's going to be equal to the bottom front which is B F I can hit my green check and you'll see that you get a little symbol indicating that it is linked to a variable I'm going to do the same thing for the back side here that's going to be equal to the global variable of bottom back which is B B I can hit my green check notice that I'm not dimensioning I mean I'm dimensioning but I'm just linking it to a value that already exists exists in this model now this one this is going to be equal to the global variable of curves nice smooth curves on this speaker and I'm gonna make that one and this one on the other side equal I like to use my contacts toolbar if you're not using it you probably should one more thing that we're gonna have is going to this one there's going to be equal to a global variable of D for depth and green check now this is completely defined we have a fully defined sketch as defined in our status bar so that's the way we want to have our sketches is completely defined now I can get out of this sketch now to make something that is a little more complex you're not going to well you could use an extrude but we're going to use a little more complex features you could use yeah either a sweep or a loft in this case I'm going to use a loft but to use a loft I need another shape to go up to well before I do that I have to sketch on a plane that's up there well I sketched on my top plane so what I need is I need another plane up here so I'm going to hold ctrl and I'm going to drag up to create an offset plane now ideally what you would do is hit equal and then link it to a variable but you can't do that that's just a SolidWorks thing so I'm just going to hit my green check but what you can do is you can link that offset plane depth to a variable but you have to accept the plane first and then double click on the plane and then we can double click on that dimension and then we can link that to a global variable of H which is height quick rebuild here and you'll see my plane is in the correct place I can now sketch on said plane and I can do exactly what I need to do here so I can draw another line again obvious we could use our midpoint line if you wanted to or you could pick up that midpoint reference and put it on the origin and at that point I need to define the width of this line and that's going to be equal to the global variable of top front or TF all right now the next thing I need to do is do the back so I'm going to use another line back here you see we can draw another line of course you can pick up this midpoint relation and hold control and put it exactly where you want and then we can define that one now I use a lot of mouse gestures and that's where you right-click and you can drag through any one of these commands that you have if you're 10,000 IQ you can not necessarily that I'm that but I've been asking for a second level for a long time and I finally got smart one day and instead of creating a second level on my mouse gestures I just mouse gestured me hitting my S key because hitting your s key you can then right-click and customize the s key so now I'm just mouse gesture hitting your s key and then you can find everything right there and customize at all so just a little tip for you if you like Mouse gestures then mouse gesture your s key to give you that second level all right now I'm going to link this one to the global variable of T B which is top back hit my green check I need another three-point arc so go from here to there and three kliks said the count and then I've been watching too much Sesame Street with all this quarantined stuff so maybe some of you can relate this is going to be equal to the global variable of curves and hit my green check again I'm going to link this curve to that curve making them equal and then I can get out of this sketch now we have our framework here for our speaker but I need some nice curves for this to follow so on my front plain I'm going to create another sketch that just contains three-point arcs so from sketch to sketch creating like a little wireframe of the speaker and of course these are going to link to the global variable of curves hit my green check and again I'm gonna link both of these where they're the same curvature and then get out of this sketch now there are faster ways to do this but I'm gonna go the most robust modeling way to do this so I could have used 3d sketches but I'm going to use 2d sketches in this scenario now I'm going to take this front plane because I need to sketch the same thing on the back I'm just going to create an offset plane by using control drag what I want this model to always have a plane on the backside back here so I can link this as an offset plane that Pierce's that point so I can then hit my green check now no matter what that depth changes to this plane will always follow so then I can open a sketch there and do the exact same things get a three-point arc here and then link this to the equation or the global variable of curves time make these equal and we're good to go personally I like to hide my plane but you'll see now we have a wireframe of our speaker now remember our design challenges between 300 and 350 cubic inches for an internal volume well right now we have 0 for internal volume so we're pretty far away but what I need to do is go to features and do a lofted boss/base if I loft from this sketch to that sketch that is exactly what I need except you'll see that our curves is going very prismatic up to from point to point so I want this to follow our curves to do that I need to use a guide curve now when I choose a sketch that has to open profiles in it it's going to prompt me to use my selection tool bar and that's totally fine we'll select that group hit my green check I'm going to do the same thing over here the same selection toolbar pops up you'll see what these guide curves do is they pull it out and make it follow that guide curve so I'm going to do two more times we're going to get back here use that one and then finally back here and use that one perfect now we're following our guide curves I can hit my green check you'll see that we have some nice nice solid here it's curved in a couple different directions but now what I want to do is check the volume so I'm going to go here to evaluate I'm going to go to my measure or mask properties let's go to mass properties you'll see my volume is 326 cubic inches well if I'll shoot and be between 300 and 350 I would say that's smack-dab in the middle so I'm gonna say that's okay but this is an internal volume and this is a solid so as you can see with our section view I can prove that this is in fact a solid so what I need to do now is I need a half inch wall thickness for my speaker so what I need to do is create an offset okay now I can use the feature called shell now you guys are probably very familiar with shell and it's going to remove an internal volume well there's another feature inside of shell well it is shell but what you can do is you can say that you want a half inch wall thickness and then you can check the option for shell outward now I want everyone to pay attention when I hit my green check it's going to get a little bit bigger you see it kind of jump out just a little bit what it's doing is it's taking the faces that exist and its offsetting it brought it by whatever value and that's a half inch and then removing the internal volume so it's like an opposite shell so now you can see that we have the exact same volume inside that we just have as a solid so that's a really good technique that you can use to create a cavity inside of a part so first thing I want to do is I want to check the internal volume and make sure that it is in fact still between 300 and 350 so a tool that I can use to check an internal volume is I can grab a plane that completely intersects that that space and also that body and then I can launch this tool called intersect now intersect is one of my favorite tools because now I can create an internal region when I create these internal regions you'll see that I don't want to merge as a result and I want to hit my green check now hitting tab on top of this model you'll see that I have two internal pieces I can then combine them together this is like a boolean addition or subtraction in this case I want to add both of these solids and the reason I have two is because it was split down the middle by that right plane but we were then able to get the internal volume of the overall speaker so now I can add those together and I can evaluate and mass properties and don't include the hidden bodies because we have that thing hidden you'll see that I am at the exact same size that I was earlier so now I can come back and I can delete that body that way I just have a feature in the tree or deleting that combine and I can reshow my speaker and again this thing is hollow now what I need here is I need to add some Phillips so we need this thing to be nice and rounded so let's go back up to the Phillip command now I want to point something out everybody uses manual Phillip what most people use manual Phillip there is also a Phillip expert and what you can do is you can add multiple sides of the Philips in one go so I can say that I want a three quarter inch filament and I'm going to add it to all four my external corners like that and then I can hit apply and then I can come back and say you know what I want to now add an eighth of an inch and I want this to go all the way around the front and all the way around the back and then I can hit apply so notice and I with this green check I added to Philips at two different sizes in the same command so that's how you can use the fill it command to add a bunch of different sizes in one go now I have two pieces that this is going to have to be so I'm going to need to cut this but I'm also going to need to screw them together so to screw them together I need some space for my four mounting bolts now if I cut this model and section it and accept that section view I need some material to follow this edge so that we have some meat there so that we can actually put a screw now one thing that we could do is we could just extrude a boss but I want something a little more sexy a little more smooth that can follow our speaker contour well what I can do is I can create a sketch on this back face convert the entities and then draw a line so when I convert those into these it's going to pull that all those edges right over there to it are on to this sketch so that I can use them now on this one I want this to be a specific distance across so for the back I want this to be a half inch wide and then from point to point I want that to be a half inch tall so a half by half now I have too much here now what I can do is I can trim away I can get rid of all the stuff that I don't need now I want to point something out this is something that a lot of people haven't realized there are these red dots and if you go too far and you accidentally cut too much you obviously going to hit ctrl Z but if you just keep holding and then you back up through that red dot you'll see that we can undo the things that we cut so just keep that one in your back pocket I can then get out of that sketch and I'm going to create another sketch up here that converts these entities again and I'm going to create one down on the bottom so I'm creating sketches that we can use to loft to create our mounting bosses so this one bottom back is going to be 3/4 of an inch wide a little bit bigger and then it's going to be one inch tall now again I want to make sure that I only have a single close profile in here so I can use my trim entities you're rid of all that and then once it highlights in this blue shaded color that is SolidWorks telling me that my shaded sketch contours that is a closed contour all right now I can get out of there I have my two sketches in the back but now I need to sketch in the front well if I hit section again I need to actually flip the direction that I'm sectioning and I can then sketch in the front of this thing so now I can create a sketch on this front face and do basically the same thing convert the entity and then draw a line that goes from that edge to this edge and then give this a height so from vertex to vertex that's also going to be an inch tall and then from that vertex to that vertex that's going to be 3/4 of an inch now this is one of those things that you could also link into your global variables like we talked about in the beginning or this is something you can do on the fly best practices say that you would probably link this into your global variables and that's okay it's going to be a just like I talked about earlier it's going to be a better place to go to one stop and make all your changes and one more sketch here convert these entities draw another line and then hook this up and make them coincident and then finally the top front is going to be 3/4 of an inch tall and it's going to be 3/4 inch wide remove all my your stuff using our trim command and get out of my sketch now how for sketches here and I can turn my section view off now with these sketches that's exactly what I need to do a loss so from one profile to another now I can go features and I can do a lofted boss/base now I'm lofting inside this model so I file off from there there you see I get my preview and I can hit my green check and it succeeds but that might not be exactly what we want and so let's flip this and let's look inside this model so if we're 3d printing this this is going to be a huge design challenge so what we need to do is we need this loft to follow the curvature of the speaker so to do that what I can do is I can then go to my original loft and I can show the sketch for the bottom and the top now what we can do is leverage these sketches so that we can use them again so let's go edit our loft here and this time I'm going to use a guide curve but if I choose this notice that it grabs the entire sketch that is not what I want so I'm going to clear that selection instead I'm going to right click and use my selection manager so I can grab just one segment inside that sketch and then hit my green check you'll see now that if I hit my green check this Loft is drastically different it follows along the curvature of our speaker I'm going to do the same thing for this top side but I'm going to leave it section so you see it happening loft from this shape to this shape and it obviously it goes straight forward guide curve I'm now going to use my selection manager and use this to follow and hit my green check and then hit my green check to accept it so you'll see that we have a lot more meat there now so we can put our our mounting bolts now to speed myself up I should probably do that all over again I'm just kidding please don't unless you're getting paid by the hour I guess don't do that completely all over again what we can do is we can take both those lofts and the right plane and we can use the mirror function so that we can mirror them to the other side creating so symmetry so perfect we have sped ourselves up and we have designed this speaker so that it has a good internal volume now I want to do something really quick I want to do another intersect to check that so listen again let's go right plane and this solid and let's do that intersect command and you're going to create an internal region and hit my green check again I can hide this and we can take both of these and we can combine them together and once you combine them together of that solid and that solid we can then do that evaluate mask properties you'll see we're at 300 217 cubic inches we're still within spec so we're good to go I can just delete both those features or you can leave them in your tree it is totally up to you but now that we're back to looking at our model you see it's hollow what I need to do is cut it in half so to do that I'm going to create a sketch on my right plane and I'm just going to draw a straight line now it's going to be a fully defined straight line but it's just a straight vertical line I'm going to start to dimension this thing and when I dimension this thing I want this to be equal to the global variable of height times 1.5 so you can even use those global variables in equations to modify those dimensions now I want the front piece to be an inch and a quarter back so this is how how big our front and back piece we're going to create a housing basically and then a front cover now I also want to define how far from this point to the our origin is and I want that to equal the equal variable of height and then divided by 4 all right and that puts us in the right spot so you can see that this is going all the way through a model now one thing that people usually are not utilizing enough is surfacing and a lot of times you say that word and horse users will kind of cringe like ah surfaces they're not difficult they're not hard what we can do is you can go to services and we say extrude surface surfaces are very similar to solids you can see I can pull it out a blind direction or in this case I want to choose a mid plane and I want this to equal the global variable of the the biggest one which is bottom front so BF x 1.5 and that should get us all the way through the model that means no matter what you change the speaker to this plane this the surface that we're creating will always be larger than the model then we can hit our green check so what we have now is a solid model or a solid body and a surface body we can now use the surface body to cut but surfaces by definition have zero thickness so I can cut this model without removing any thickness at all if I choose cut with surface I have to remove aside instead what I can use I can use the tool intersect again so using intersect I can create an intersection between the surface body and this speaker body this this time I want to create intersecting regions and hit intersect now one thing that'll get you when using intersect for the first couple times is the option of mergers all even sometimes it's collapsed you'll be like what the heck's going on SolidWorks uncheck merge result and then instead of looking exactly the same it'll look completely different it'll be cut in two now there is a feature inside of follower works that will create a lip and a groove for you it is literally called lip groove now before we go down this path I'm gonna hit save save early save often it's a source motto speaker save alright so I'm going to use the lip and groove command now I remember if you don't know where it is you can come up here and search and look like you remember where everything is all the time now a lip and groove is going to require two separate bodies low and behold we now have two separate bodies I want this component are that solid and that solid I need to choose an edge to follow and so I'm going to choose that edge right there now our groove selection is going to be based on this face and I'm going to choose my outside edge which in this case is going to be that edge so you can see selecting that edge will do it for me and now on my lip selection it's going to be on the other solid I'm going to choose that face and then the edge that I want to fall is going to be the outside edge right there and then the specification it's kind of where the rubber meets the road on the lip groove command is all of these specifications now in this scenario we're just going to let it be a zero degrees of draft and we're not going to put any tolerance here because I want you to see what the lip groove command does and then we may or may not use it so let's set our green check and you'll see that it's going to start to modify your model it might even give you warnings like hey we're going to make this but it's not going to be a hundred percent right okay so it works show me what you got so if you zoom in here you're going to see that it kind of pulled it straight forward it didn't follow the curvature of our speaker perfectly you see these don't line up right now it created the lip and groove which is exactly what we wanted so now our front piece can slide into our housing what the problem is our curvature isn't right so if we were to go 3d print this thing these edges are going to be pretty gnarly they're not going to line up perfectly so you can see how they're not gonna line it up now unless you just want to go out there and file away or sand it away by hand I personally don't want to have to put all that elbow grease in why not get it right the first time so you can see here's our lip and our groove on our model and again shift-tab will will show everything and tab will hide everything in case you didn't know that but because this lip and groove did create geometry it obviously did work but it's not working as well as we want so what I'm going to do is I'm going to crush these lip groove features and I'm just going to get them out of here so we're back to these being solids there is no lip or groove so now what I'm going to do is I'm going to do it manually using surfacing I hear some of you going oh no don't do that it's gonna be cool because surfacing is really fun so don't be scared of surfaces but what I'm gonna do is take this surface body the hidden and I'm gonna go to my surfaces command and do an offset surface now I want to offset this by a quarter of an inch that's how much overhang I want but I want to go back into our housing hit my green check so now I have another surface offset from our first one then I can then use the intersect tool again and we can use this to cut something do another intersect between that surface body and the back housing creating an intersecting region and again don't merge the results otherwise you're just going to have the exact same thing whenever you come back this is the geometry in the middle I'm gonna hide the cover and hide the housing this is the geometry that we want to split we want to rip it in half and then we're going to add some to the back piece or the housing we're going to add some to the front piece or the cover so to do that I'm going to also add 20 millimeter 20 can't even think today so 20,000th not 20 millimeters would be a lot 20 20 thousandths of an inch of tolerance in here so by creating a sketch on this face I gave them do an offset entities and because this is a half inch wall I can then offset it by a quarter of an inch in the opposite direction and that should be smack dab in the middle and in fact it is so then we can use our surfaces and do another extruded surface and we can do this midplane and we just have this like an inch thickness so you can see that it's going through our model and that in that case it's intersecting everything and then we can use that tool intersect again this is one of the strongest tools out there hopefully you guys have realized that we've used it a couple times now we're going to create both this time internal and intersecting you'll see that it has two separate selectable bodies we are not going to merge them in my green check and then to create our tolerance this is going to be an interesting one because if I were to hide that surface the surfaces have zero thickness so I remove zero geometry I just cut it but what I can do now is I can offset that surface again so surface is offset surface and instead of that face I want to offset this entire surface body so that one and I can offset this by whatever our tolerance is so 20,000 so now I want to make sure it's going into I want to remove the internal part and that can hit my green check you see now we have two separate surface bodies so I can then hide the outside now whenever you do a cut with surface you might be cutting more than what you're anticipating so let's not do that let's do a cut with surface and let's cut this and I can go down here and I can check that I am cutting the correct direction and in fact I'm not you see that Arrowhead is pointing inward indicating we're going to remove all the internal geometry I want to flip it using my arrow head another thing I want to do is feature scope I don't want it to auto select I only want it to cut this body so this outside body is going to stay put so by using a surface cut or cut with surface and choosing the correct direction and then have the feature scope only cut that specific body I'm not removing anything except that little gap so now you can see we have our 20 thousandths of Tolerance all the way around our model now all I have to do is show the housing and show the cover and then again use shift tab to bring those back you see my curvature lines up perfectly because we literally just cut the model apart and then we cut that chunk into the halves and now all I have to do is add it so say I want to take this solid and that and I'm gonna add them together so again we're going to use the combined feature and we're going to say you know what I want that solid and I want that solid I want to add them together and hit my green check that is no one solid and then hide that one and show my my cover and do the exact same thing combined and I'm going to take that solid and that solid and combine them together so with that said you can now see that we have our nice pretty rounded speaker that has our manual lip groove here and the curvature is perfect because we use that model with some surfacing techniques so if you guys want to get deeper into surfacing then what you could do is you could contact your account manager Allen Kelly and Adam COO filter both on this call so they'd be more than happy to help you guys out send them an email and give them a call and you might be able to get into our surfacing class coming up now talking about modeling challenges I want to move from a single part design all the way into a very large design so I'm going to save this in case anybody has questions about it but I want to step into something a little more challenging and one thing that I see a lot of people using a lot of is weldments and that's great but one thing that might speed you up is you use this thing called structure systems now this is a completed structure system and you can do this with weldments but that can be challenging it can take a lot of time to create all these members and do all the trimming that you have to do to create a structure such as this so let's open this thing up and we're going to open that structure system from scratch so one thing I want to do is go to structure system and activate a structure structure systems are comprised of primary and secondary members it is weldments on steroids so our primary remember we're going to choose our profile just like in wellness and then all we have to do is specify where our members are going to follow in this case I want to use an up I want to use a point up to plane so I'm going to go up to that plane and I want this point and that point to go up to that plane now you can always say that there's a direction of extrusion if you wanted to but we're not going to do that in this case so go up to that point hit our green check to accept those primary members now then I have primary members let's do some secondary members and there's two ways to design structure secondary members there's either by the plane members or by points so I'm going to do planes and then you select your primary members and then what planes you are going to use so very quickly you can add these members in here all you have to do is choose your Pierce point and in this case I want to line it up with the top there now I want a couple more members now really one member trimmed a couple times so I can do a secondary member this time using points going between that top secondary member and the bottom secondary member so I want them to be on the edges and then I can go to my profile and I can rotate that 90 degrees and then I can even split it so I can say you know what I want this member to be split around that member and around that member and then I can hit my green check now where the rubber really meets the road on a structure system is the the trimming so you can spend a ton of time using the trim command when using weld nuts you don't have to when when you're using structure systems so I can hit exit structure system and this is where it's going to do simple to member and complex corners so in this case for both my simple and my two member I'm going to use the same trim mechanisms but for the complex trims I'm going to go ahead and let SolidWorks figure it out it's smarter than me it's a computer so I'm going to hit my green check and it's going to do exactly what we need to do for corner trims you can see here that everything is nice and trimmed up so what I need to do now to add to this structure is to actually leverage some of my other SolidWorks tools like circular pattern things say you know what I want this to spin around my Center axes but instead of clicking all these bodies in 2020 we now have the ability to use the structure system and pattern the entire structure I can get twelve of those so that's a way that you can really drastically speed up your weldment designs another thing you can do is create a brand new structure system based solely on secondary members seeing say you know what I want to be between these four members and I want to place it at these planes and so now we have these members going in between again choosing my Pierce point so I'll line it up with the plane hit my green check and again exit the structure system and this time let's Oliver's just use the body trims and hit my green check so everything is trimmed appropriately and then what we can do is do another circular pattern and it goes around the center axis and again pattern the structure but this time just that secondary member structure so you see very quickly we're able to create something much more complex than just using weldments and all the trims are perfect everything is exactly where it needs to be and we didn't have to do much we started this thing from basically two points so this a way to really speed up your weldment designs now another thing that I want to talk about while we're on this webinar that I see a lot of people could really benefit from using is something called detailing mode now detailing mode is actually new for 2020 so if those of you not using 2020 I recommend you get on it but if you're using large drawings I would recommend that you open mo open it in a new mode called detailing mode so I'm going to open this drawing that has over 5,000 unique parts it even tells you hey in detailing mode these are the things that you can do cool thanks SolidWorks thanks for them fo but you can see how fast this drawing opens now for those of you that are using large drawings and you open a drawing go get coffee and come back this could really speed you up so this is not just like quick view this is something that you can modify the actual drawing you can come in you can make notes so if you have standard notes you could drop those notes in to the drawing and this is the real drawing this is not a quick view or a snapshot or anything like that notice how quickly we can go through all the different pages here now another thing that I see people using in large assemblies is not necessarily just large drawings is but also just the assembly itself and assembly such as this this little XY Z table here we want to go look at this we're going to open up the assembly and I open it from the drawing using open assembly and there are some tools that I see people under utilizing and that's performance evaluation when you click on performance evaluation it's going to bring up information about this assembly it tells you how many files are in it how many documents are in the newest version how many might have too high of an image quality things that could negatively affect your performance there's also this tool called assembly visualization which I love this is one of the things that I use on support all the time and this really opens your eyes as to how your assembly is made up so when you choose assembly visualization you'll see that there's a couple columns by default there's a quantity which is super helpful especially if you have a thousand screws inside of a file you want to know how many are in there there's also a total number of graphics triangles which is how dense the file is from a graphical or face perspective so things like screws with threads helixes or spring something like that might have a high total number of graphics triangles or just something that has a very high setting on that part maybe you just have something that is not rebuilding very quickly or something that's opening very slowly we can go in and we can look at those open times and figure out which components those are and you see in this scenario the one that opens the slowest is this I guess chain which is kind of to be expected especially because there's a lot of moving parts in there you can also go look at the total number of graphics triangles this was interesting because if there's only three of these but its second in the list of graphics triangles so if we open that file we can take a look and see what it is and to me that's not something that should have that high of a graphics triangle so this is something that you might want to go down and figure out exactly why it has a high number of graphics triangles one thing that you can do is you can go into the gear you can go to the document properties you can go to the image quality slider you can see it's up here kind of in the middle you might want to slide it down and hit OK and that can lower the number of graphics triangles so put that one in your back pocket so that if you have an assembly that's running a little bit slow on you then maybe you run the performance evaluation and the assembly visualization so that you can exactly figure out what's going on and it's not just a guess so I'm gonna close this drawing as well and the last thing I want to talk about is whenever you have complex designs at the Assembly level not necessarily at the sketch or the part level but at the Assembly level maybe you have some robotics and you have something that has a bunch of angles of articulation and you can't fix this model in space because it actually has to have that articulation it has to be able to move like that well if you haven't been using the make controller for designs like this you've been missing out there's this thing that you can launch called the mate controller and it has specified positions so you can see if there's a home position there's a position over object there's a pick up and then there is a closed jaw and then there is a lift once you lift this now we can add more positions we can say we want this to be position 6 we don't have to take the time to name it right now and in this one we're going to rotate the base and we're going to change the upper arm angle so it's going to lift it up a little bit and I'm going to update that position new position position 7 and in this one I want the forearm or the wrist angle to change so we're going to change our wrist angle to be up and I'm going to update that position and make a new one and on this one I just want the gripper to open so we're going to open that gripper and update that one now a quick trick if you're going to use the make controller is I can go back to home make a new position position 9 so now home and the last position are exactly the same now what it does what SolidWorks does is it can then interpolate between all of those fixed positions to create an animation so if you've ever used exploding for animation it's really that easy except way easier because it's going to collect all of your limit distance limit angle mates and allow you to change them on the fly and if you have to do any kind of kinematics or motion study you can take that mate controller and you can push it into your actual motion study so you can import into your motion study as either key frames or motors and you can see that down here under our mates all of those are captured in your motion study so if you're having to do any type of simulation or motion simulation you may want to heavily look into the make and drawer well at that point what I want to do is I want to thank you all for attending this webinar today hopefully someone got something that they can put in their back pocket and use later in any type of design challenge but I also want to open the floor for any questions if you want to clarify anything or anything like that Marcus and I are here to answer your questions thanks a lot thanks for attending [Music] [Music] you [Music]

Channel: MLC CAD Systems

Views: 16,265

Keywords: solidworks, surfacing, loft, intersect, lip and groove, mate controller, animation, large assembly, detailing mode, solidworks premium, solidworks 2020

Id: Kapw0M-XlMw

Length: 49min 9sec (2949 seconds)

Published: Wed May 20 2020