Transcript for "Leveraging Surfacing Strategies to Elevate SOLID Modeling":
Hello. Hello. Welcome to leveraging surfacing in SolidWorks. I see that we're getting 21 people roughly right now. I'll give it a couple more seconds for people to kinda turn in, and then I'll go ahead and introduce myself. Three. Couple more. We have roughly roughly 50 scheduled, so kinda give it a couple more seconds, maybe a minute until we get a little more, and then we'll go ahead and how's everybody doing today? I'm over in in Iowa here working from the cold. Where's everybody joining from? Boston. Okay. Definitely some more cold up there. Heard that, New York is getting some record record snows. You're breaking breaking records up there. Colorado, San Diego, Carlsbad. Awesome. All over the place. It's only Florida, Santa Cruz. Man, I am jealous of all you people that are in some warm states right now. It's pretty awesome. Alright. We got 25 in here. Cleveland. I see that too. See it. We'll go ahead and get started here. We got roughly 25 people in here. But welcome to leveraging surfacing in your modeling, your everyday workflow. The goal of this presentation or webinar is to kinda get you guys thinking about, hey, how can I start using surfacing tools to either completely replace some of my other, let's say, revolve, just extrude a couple of certain commands that you could kinda skip over by doing some surfacing? Another thing you start using surfacing for is building robust references. So as we all know, if maybe we'd make a change at the very beginning, once we're at the end of the process, we make a change towards something toward the beginning. We've seen a bunch of yellow or red in the tree when something breaks down or loses references. Right? So we're gonna take a look at servicing as a replacement for references. So things are a little bit more robust, dynamic, and they update in a healthy fashion. And then overall, we'll just kinda introduce you some some surfacing concepts that kinda give you a peek behind the the curtain as to what SolidWorks does, especially with its, extrude commands. All of the the basic features that you see in your day to day in the back end of the engine are essentially built through surfacing kind of, like, maybe, like, five commands altogether to then then throw it into a extrude command that you can run. Right? It's a little easier in the UI on the user. Okay. Let me go ahead and share my screen here, and I'll introduce you to the model that we'll go ahead and start working with today. Now off the get go there's a lot here let me go ahead and hide some things I have an extra body in there. We've got a can almost think of it as a a puck, maybe even a space mouse or a three d space mouse, something like that, or a fan cover. Either way, the general shape, provides us with a way to look at a manufacturing problem, as well as once we get past the manufacturing problem, we'll start delving into a little a couple cosmetic items that maybe kinda go outside that scope, with maybe indents and extra surface on the outside here. If I roll back just a little bit, right, that thickened turns into a surface and then we can kinda start taking a look at how we start building ribs, get some more natural contour geometry in there. Alright. Alright. Let's go ahead and start from scratch with the manufacturing problem. Early on in the stage, we've got a manufacturing problem where, I'm throwing just this piece of rubber into a manufacturing process where it vacuum molds this into form. And the process or the requirement for that is that we have uniform thickness. Right? Because you throw in the material, you throw in a sheet, and as the vacuum sucks, the ideal scenario is everything turns into the same thickness throughout. As we start kinda investigating some of this model, right, you can see that we run through a shell operation. Right? So this is kinda something before we get into surfacing. If I go ahead and run before the shell operation, you can start to see how we start modeling this. Right? Basic commands right now, fillets, extrude, revolves. As we get into the wall thickness though over here, like, we're running into issues. If I go ahead and run through a section view here let's go ahead and flip this to side. Now I haven't given this any thickness. So I guess what I should do right now is run through the shell and then we'll run through the section view and we can see as I start running this through Go ahead and start pulling this out. Right? You see how it runs into a t joint? That wouldn't really that would be a problem in our manufacturing process. Right? Well, because our mold is now you're gonna have to run into some issues there. So the goal is to run through and make that all the same uniform thickness from moving the top t joint. And as you kinda keep coming out, you can see a transition down into a flat planar side. So essentially, all of our problem lies lies right in this area. So how do I get rid of that extra volume? This is where this initial problem kinda comes up. Well, you could go ahead and run through maybe, I don't know, a manual extrude kinda go ahead and cut off this extra. You could run through a revolve cut. Right? You could go ahead and kinda create a cross section on the side here, come over and revolve that about an axis, That would do the job. But what happens if you change faces? Right now, as you see right now or as as you're looking at it, right, we can see there are two split faces on this side. Well that's because I run through a split line at the beginning. Let's say you come in come into the design process and you start coming back to the original portion here and you need to make some changes maybe for detailing sake maybe you need to add decals to this. And so you need these faces split up. Okay? We can start to have a discussion about when do you include that split line in the process but the matter of fact is right now I have four different faces whereas I used to only have a singular face. Okay? Now we start running into references there right? Well, face one we can consider this one maybe face one this one face two As I go ahead and run through a split line well now I have five additional faces even more because we consider the top portion. So as SOLIDWORKS is trying to track things in the back end we have now included or added additional IDs. Okay. So this edge has its number in the back end of SOLIDWORKS. We don't see that as users, but SOLIDWORKS is tracking that ID number and when we go ahead and run through maybe a surface offset or a surface extrude or maybe we run through a dimensioning or a relationship where we say coincident to that edge. It's tracking, hey, vertices six in the back end is coincident with edge 53. Right? So you can start to see why some of these decisions in our design process end up affecting things later on, such as, right, that revolve cut that we could choose. Now let me go ahead and start to do this from scratch and show you why we can use servicing instead. Go ahead and say new file, run through part millimeters, and feel free if you guys do have questions as I'm going ahead and speaking about this stuff, go ahead and feel free to throw it in chat. I will be reading that and I will be going ahead and answering those. Okay. Let's start on the top plane here. Hit my q key, click on the plane and go ahead and start sketching. Go ahead and add a dimension here, say 1,050, it scales it for me. Hit my s key, hit the extrude and I can go ahead and pull this up say 600 I'll go ahead and build my fill it I'm not going to use a fill it command to do it because right using a fill it command would actually just instead wrap this around a little too quick there, I apologize, I'll just wrap it around the bottom, right, my envision is I'm gonna fill it here, so instead I could either build a volume underneath or I can use a revolve as well-to-do this. I use convert edges on this silhouette edge and use the solve relationships up here to drag this vertex even though it appears black up here. Since I converted it, I can drag it along the edge because it has the on edge relationship. Now we can see once I've dragged it that blue edge or that blue vertex or that black vertex turned into a blue vertex. Super nice on that. It's my favorite one of my favorite things about the convert entity tool. Go ahead and build my fill it here with tangency. Go ahead and say that both of these lines are equal. Alright. We can see that kind of snap back and I can give that a dimension. I'll dimension that three fifty. Okay, let's go ahead and revolve from there straight from the sketch, oh, I forgot to give it an axis of revolution, say no to this, add a construction line at my center, using mouse gestures to make all this go a little quicker, hit my s key again, revolve boss base. Okay. Great. Now the next thing to do, right, is go ahead and add that base that we're talking about, that little flange for mounting. Go ahead and grab my center rectangle tool here and drag it out. Now we did intersect these fillets and we were cut off here right so now making sure that we're short of it, I'll say 800, gets us into a good position, I'll say that both edges are equal to make this perfectly square. Alright, and I can go ahead and say extrude we're gonna make this a 10 millimeter thickness because that is going to be the thickness of the material that we throw into the machine make sure that it's going the opposite way so that we don't merge with any of the fillet. We wanna be perfectly flat. Okay. And one thing I forgot to do is uncheck merge entity. We are gonna leave this unmerged so we can go ahead and run through some other, other functions with a little bit of multi body here. Okay. We can confirm that we are separated by expanding our solid bodies folder right we can see there's two bodies there Go ahead and continue to sketch and build the outside loop here. I'm going to click on the face and hit convert entities that converts the outside for me, right, and I can go ahead and immediately extrude a boss space there now I'm not looking for the inside area instead I'm looking for a thin feature I want to build those walls so I'll hit the thin feature checkbox in our property manager and then I'll go ahead and flip the side to one direction flip it to the inside we can see that kind of change, right, and I'll bring that to 30 the thickness here is going to be 10 so I won't change it there but I will change my end condition to 30 and we can see that wall increase in height. Okay, I do want to merge but I don't want to merge with this let's say center body so I'll turn off auto select in my feature scope and I will select the flat plane and hit the green check. Okay. We can confirm that that does join because the outside face is now one singular and we can confirm that it didn't join at the center because the fillet on the bottom intersects and goes through. Okay. Now we need to go ahead and cut the inside body to make sure that it intersects and doesn't go past this face. I'm gonna go ahead and use some surfacing to do this. You could go through a rectangular extrude cut but I like to use a surface here an existing surface because it's within our bounds right we're just using these bounds to trim essentially. This way it updates with it and I don't have to go into a sketch sketch a rectangle or hit convert entities instead I can go directly to surfaces say offset surface and choose my outside faces. Right I'll turn this into a zero one thing I want you guys to notice is at the top in our property manager it says offset surface at the moment as soon as I turn this into zero it changes to copy surface. Okay so if you ever want to copy a surface one of the methods that you can do this is to come into offset and hit the zero on the dimension. Okay great How do I know that I have a surface? Well, over in my left hand side my feature or my feature tree I can see that I have a surface bodies folder with a surface body underneath. Okay, visually how do I confirm that? Well, if you zoom in you can see that this is a little bit blue. If I hide the body underneath using tab, I can see that now I just have the outside faces and that blue is confirmed on the top and bottom. Why is it not blue on the corner? Well, because it's stitched together on the corner. Blue means an open surface. Okay. It just tells us that we have a surface there as well. Okay great. Let's go ahead and use that surface to cut so I'll say cut with surface One thing to do healthy maybe is to pre select it in your feature tree and say cut with surface auto fills it for us. Now in this case it's kind of like a flip side to cut so you can go ahead and click on the arrow to see inside or outside. I'll say I want to cut the outside and I'm gonna say that my selected body is the center core. It doesn't have to be the center core in this case but let's be a little bit more intentional with some of these selections. In case we end up changing geometry let's make sure that the only intended target is that revolve. Okay we can see that that does cut it away one thing you can also notice is that our surface is still there so it did not consume our cut tool which is also nice if we need it for future use. Okay now let's go ahead and run the boolean command combine so I just hid my surface there bring back up the other solid hit my s key and in my menu I've already used combine a lot so I throw it in here on a typical basis hit my s key, hit combine, I'm gonna add both of these bodies together and I'll right click to accept. Notice all the artifacting that we saw inside the wall goes away because we Boolean command that together. Okay. I'll go ahead and stop right there for a quick question. We've got Jason Wendling, why does your center point rectangle have construction lines to the midpoints instead of corners? Good question. Inside our sketch, let me go ahead and edit that, When we run our center rectangle command over on the left hand side in the property manager, there is an option for from corners or from midpoints. There you go. Thank you, Jason. I could have read a little bit farther. Jason answered that. Thank you, Jason. Okay. We'll keep going. Alright. So one thing that's going on right now that's different than our prime example is, right, our material isn't above. It's not creating that t possibly. One thing to evaluate. Right? Well we haven't even gotten to our shell command yet so let's go ahead and do that let's run through shell you can always type in your s key let's go ahead and hide it we're gonna say that the thickness is 10 and I'll hit the green check No issues. The software does it pretty good. Let's go ahead and section it and we are still running into that tee. So we are requiring that solve. Okay. Well, you could go ahead say front plane convert the silhouette edge there that we get. It convert entities. Right? Convert entities. Right? Soft relationship, I can go ahead and click and drag off. Notice that as I drag it off, what's it doing? Well, it's just gonna continue that radius that we've built essentially. So I'll go ahead and drag it off. Now problem with that is maybe I need to then say that that is coincident with that bottom face right so that I'm ensuring that I'm cutting to that plane essentially. Okay let's go ahead and complete that arc let's establish a axis and then I can hit revolve cut, if I don't have it in there I can always come back to my feature tab revolve cut. Okay, I'll say green check and we can see that that does in fact satisfy our requirements. Alright, that gets rid of all that extra material let's go ahead and section it all of that T a T doesn't even occur anymore right so we've solved that manufacturing problem now again we haven't used surfacing for anything so no didn't really solve it yet with with surfacing What happens if I go up to above the revolve and then I go ahead and run a split line? To do this I'm going to essentially use split line with a projection so I'll sketch on this top face and all I have to do is create a t. Let's do this with midpoint line to be efficient here. Bring it off, say horizontal. Let's do that one more time and show center line. Let's do midpoint, bring it off and let's turn that back into regular. Okay. Our geometry goes past where we want to create split faces of, right, the my s key on the split line command projection and we'll choose on these faces hit the green check and now we can see those places those faces are split What happens if we go down now? Well now our cut revolve has issues. Now it's yellow so it's able to still cut. Right yellow means that you're able to produce the geometry still, red would mean that it's not able to produce the geometry and essentially we wouldn't see that cut. Yellow means that we've lost that reference. Okay if we edit that sketch right we can see that that that yellow for that arc essentially that we had is now yellow meaning it's lost it. Why is that? Well, because again we changed edge ID numbers in the back end. Okay. What happens if I eventually go ahead and increase this diameter? Let's go ahead and select the face that belongs to it and I'll change this to let's say 1,500. Go ahead and control queue it. Well now we've got some more issues. Bunch more stuff broke surface cut didn't didn't work. Why didn't our surface cut work? Let's go ahead and take a look. If we take a look at our surface here, let's go ahead and hide the main body. Our surface is, let's go ahead and turn it on, is only so thick. So what we end up having to do to adjust for some of this is let's go ahead below the surface cut or above the surface cut and run another surface tool called extend surface. Go ahead and select the top side here, I'll say that we want the same surface and we want to pull it up. Okay. It doesn't need to be this exaggerated right it just has to make sure that it intersects the fillet, right and we can confirm that now it does so maybe this reference surface that we're using maybe just to be a little bit healthier maybe we increase that distance so that anytime we change this diameter right it has the ability to work fine and maybe you build a little bit more logic into this maybe you build this to be proportional this dimension for this height maybe you build that to be proportional to the size of the diameter maybe you start working with equations on that to make that even more robust. Okay let's move below the surface cut it now likes it let's go ahead and move down below the shell moving a little too fast shell works. But then if we look at our cut revolve, right, well, that breaks a bunch of stuff. What I would do instead is I would go ahead and use these surfaces in order to do that, do that cut. So let's go offset surface. Now I would like to do this oh, one other thing to notice. Anybody see anything with this face right here? Why am I not seeing that split line? Right? That's what I'd be asking myself. Now both of those features work. Where do I lose that split line? Start evaluating that right? I lose it at the very beginning. Why do I lose it? Well because right our split line doesn't fully intersect one of those faces So if I go ahead and drag this down extend it past and say exit sketch now we get that split face again. That I would call more of an error on our part with the sketch. Instead of using a sketch in this scenario, what I would do is just use a plane. Right? Why a plane? Well, because planes in SolidWorks go out between infinity. So we're not gonna have this worry issue about, hey. How long do I need to make this line? Okay. So let me go ahead and suppress that and we'll do a split line. I'll hit my q key, pre select both the front and right plane, and run split line. We'll choose intersection, and then what would we like to split, and we can see that preview. Okay, so now anytime I change that diameter right I don't have to worry about that sketch changing with it. Okay, let's get back to our effects. Now this this diameter is a little kind of it's a little bit of a joke with what our rectangle is maybe we need to relate our rectangle to this as well so I'm just gonna go ahead and decrease this this is a little bit more healthy I'll run through offset surface I'll choose these for internal or external fillets I'll say zero and now here's a really cool thing that we can do with our surface I'm gonna say untrim surface right you can kind of see towards the bottom right we've got some some kind of indents from where our edge meets our surface. I'll say untrim I select one of the faces right and then you can start to see woah how does SOLIDWORKS know that is what the surface was before? Well maybe from feature history but more so from the fact that it builds every surface as a four sided surface and then trims it in order to fit our geometry. Okay. So that's why we're able to untrim completely like this. Alright, let's go one step farther. I need to use either a cut cut with surface or maybe I need to get this into a volume now if I'm thinking volume I need to close the surface up I need what maybe four additional maybe I just need two additional faces to close this up so you could build the top side and then the bottom side let's skip that that requires sketching and closing up with a knit surface let's just all do it within one command. I'm gonna say extrude surface and I'm just gonna click on the face. Okay great, not getting the preview it's not doing anything it's because we need to tell it a vector. I'll go ahead and hit Q on my keyboard show me planes and I'll choose the top plane to give it the normal vector to the top plane. Okay great I can start to see a preview well now it's essentially extending from the edges of this existing face that's really nice there's also an additional option called cap end cap end great it just kind of replicates the bottom face and stitches it up with where the top meets great let's go ahead and increase that distance right and you can see what starts to happen there Maybe you want this for an additional you know maybe this is your outside shape maybe this is another part maybe it's a bearing something like that that's kind of cool right I'll say net result why net result all because I want to turn this into a solid volume to run a boolean command. Alright now all the blue goes away and we can kind of take a look at that surface geometry. I'll go ahead and bring up the other the other body again and I'm just gonna run through that combined again and I'm just gonna say subtract this time main body central housing body subtract right that main surface that we just built Alright and we go look at those corners and we do have the same type of situation. Okay let's change that center console again let's go change that to just say 100 control Q and we can see that update as well. Okay. Any questions as it is right there? Mark, you noticed it? Very nice. It doesn't go out far enough. Alright. Very nice. Okay. Cool. Now what we did lose is our split faces here. Why is that? Well, because we ran a singular command to cut volume away, it replaced that face essentially. So if I really want to and I really needed this face dissected even farther maybe we're gonna do a quadrant indent I would just rerun a split split line command or even discuss maybe even including that split line later on in the process rather than the beginning. I'll just go ahead and redo it I'll choose my front plane and my right plane and say that these faces are intersected and we can see that that shows up again. Alright, great. I just wanna indent this corner. You may think that an indent could be done through the wrap command and you are completely right about that but there is a difference with the way that I'm gonna show you in wrap so this way that I'm showing you with wrap is hey I'm taking my corner I'm going from edge to edge I've related it to the outside I kind of want half of this to be indented. Okay, we're not going to worry about thickness here. If I go ahead and wrap this and say features wrap I'll choose my sketch and say that I want it on these two faces, I'll choose indent, Now I did it for both faces I'll probably need to do it, two commands and two commands rather than one but if this was all one face at the moment, I can show you let's try doing that delete face and we get teaser delete face and see if this patches it up let's do delete and patch. Yeah, I had a feeling it might not do it let's do one of these rather than two of these let's do delete patch. Yeah, there we go. So delete and patch. Right? Patch just says or delete says get rid of that segment and patch just says, hey. Take an existing face connecting to it and fill it in. Right? Continue that contour geometry. Now you can kind of see. Right? It's still all the way around now. Okay then I'll go ahead and say wrap hey that face is now non existent right another references reference that's broke go ahead and redo it now we can see that work. Okay issue is again it took the length of that sketch and we're missing references right in the sketch that's alright so I've got 1,100 here If I go ahead and take a look at my arc length now again clicking on it doesn't do anything so we need to go to the measure tool. We can see that the arc length is actually the length of that rectangle so this is the key thing with wrap wrap takes your sketch and the distance of your sketch and essentially puts it into a physical piece of paper and pulls it and wraps it around something right so your algorithmic the algorithm driving that geometry to push it onto the face takes the arc length and wraps it Okay. What's different about the method I'm gonna show you is we have a direct face that we're gonna use and we're gonna use that as an indent rather than worrying about hey what's the distance what's the arc length for this you could go ahead and do that right you can say measure arc length 86 and you can copy that small finite number and then put that in it like that's a ton of work let's just skip that Let's take these surfaces and let's just offset them the distance of the indent. So I'm gonna indent this eight. Let's do yeah. Let's do eight. That way we still have a thickness behind this because we are shelled at 10. Okay. Oops. Wrong direction. I'll go ahead and flip that so that we're on the inside. Either way works. Okay again I'll go ahead and run an untrim surface you don't have to do this but I like to do it for my sake this gives me a little bit more confidence. Then what I'll go ahead and do is extrude surface again we're gonna run into an issue though because we have this upper surface and if we remember beforehand right this top surface extruded up into essentially what there's what is there now. So we need to change our surface offset so I will deselect phase two, say green check, and then I'll go ahead and run through that surface extrude again. Give it a vector, give it the top plane and I'll say green check. Okay let's go ahead and bring our tool back up let's go ahead and use that command that we used before cut with surface again right Well, we're gonna have an issue because our surface doesn't fully intersect. Okay so let's go ahead and work with that surface a little bit more let's do extend surface now and as I extend it I can bring it up I'll just drag it in an exorbitant amount okay let's do extend surface again it's not really what I'm after it does seem a lot like untrimmed surface though. Okay so I'm gonna run through an untrimmed surface command first and then I'm gonna run through a extend surface nice, I like that. I'll say up to point so that we stay right in reference, say that this is the top edge, green check, I'll do that to the other side, now I probably could have run that all within the same command, let's do let's just double check my thinking here, yep, since this all belongs to the same surface we're able to untrim both of these sides. If this side was a separate surface then this side I would have had to run that in two commands two differential commands. Okay. How do I know that this is all part of the same surface? Let's use our breadcrumbs select the surface body now graphically it's not showing me it's not showing me my what I'm saying. There we go. It's because I selected the wrong thing this is all part of the surface extrusion, there we go. Okay. Let's go ahead and extend that top one up again up to a point let's say up there, choose that selection box, green check, okay, bring back our volume and then I'll go ahead and say cut with surface again, surface cut there, cut the inside, green check, still failing. Why is that? Well because I didn't join the original surface. So again one one way to tell that I didn't join this we have a blue edge where this one should be black if this is all going to be one surface right so we got some blue right there in the middle. Let's go ahead and knit that surface together and I'll hit the green check. Great that turned into a black Now let's go through run with cut with surface again. Cut away the inside and we'll hit the green check. It keeps my tool body. I'll hide the tool body. Right? Now we have that indent and I haven't even worried about sketching that. Right? So I'll work with it graphically and with surfaces instead and that'll update with anything as well. I don't have to worry about recalculating what's my arc length what's my cord length here and then changing the sketch with it as I change everything else. Okay. This is all adaptive and changes with it. To prove what I'm saying, let's just go ahead and saying that not the height of it. Let's do the diameter. One two five zero, control q. We're gonna break some stuff. Of course, we break the one thing I'm talking about. It's always how it goes as you're demoing. You know why? Because my top side because my split line on the top side works again. So then my split line, I do lower, and later on, I have that breaks it again. So I guess what we could do to kinda show you, Nope. Online. What is breaking now? Trim, combine, you take away the material. There's no need. So when we do the combine this time, it doesn't get rid of all the extra faces here. It keeps them, which is why I'm guessing this split line doesn't like it. Yep. So that's just something to kinda keep a keep a note of. For some reason, it's all words. It got rid of it the got rid of the faces and made it all one with the combined in one scenario. It didn't with the other. I haven't seen that as through all my trials that I've been working on here. I haven't seen that happen before. Of course, it happened now. But I would believe that that doesn't happen on a consistent basis. Alright increase it again doesn't break of course of course. Alright let's bring it back to that number and just see if it breaks again I believe it was and any more questions as I'm going ahead and finishing this portion. Control q. Does it when we go to that small portion? And suppress, then you can ignore. I don't need you. We're gonna do ah, I don't have that command in here. Customize, and we're gonna do unsuppress unsuppress if you can type and we're gonna add unsuppressed with dependence to that context menu and now if I do unsuppressed with dependence all the other features that go with that come with me, which is super nice. Instead of right click unsuppressed, right click unsuppressed, right click unsuppressed. I see Russell say something in chat. Inconsistency. Yep. I feel you, Russell. Sometimes it happens. But that's something to investigate on on my own and kinda get back to you guys with. Alright. And make sure I am a little bit over time. I am ten minutes over time, and I still have more to talk about. So if you guys have time, feel feel free to sit in. I'll keep going for probably another twenty minutes. If not, thank you for joining us, and I'll keep going. Alright. Last little bit is a couple more surfacing commands that we can use for let's say adding ribs or textures. So I'll take this outside these two outside faces and I'm gonna go ahead and copy those again. Different way that you can copy them is hitting knit surface and just choosing the two faces. Now this is already a solid body so there's there's not even a surface here to knit but it is essentially copying them. So let me go ahead and say green check and if I turn off that solid body right we can see that we now have two surface bodies there. I am gonna go ahead and add two more faces there top and top that way I've got the full body. I'll untrim the bottoms here just for my again personal sake and now I'm going to go ahead and create a plane at an angle now in order to do that I'm probably going to create an axis here say through these two, it's vertical, I don't have axis showing up so let me go ahead and turn that on for everybody and myself, I'll use the axis and a right plane to give it an angle and we'll say that this is maybe one thirty five, opposite, let's do 45, there we go, green check. Why did I do 45? Well, because I just want to create a plane that I can create a split line or intersection curve on. I'll say sketch and then if it rotates in some odd fashion, I'm just gonna hold alt and hit the arrow keys in order to rotate it back. Annoying. One thing I'm gonna do as well is hit spacebar, say new view. I'll save this as, just call this bump split line if I can type hopefully okay and what that does is if I ever accidentally come back and hit ISO or something and I just want to edit that sketch again instead of having to right click on the sketch. I know right click on the sketch. Let's get out of it. I didn't even sketch anything so that doesn't happen. Sketch now I'm in a weird view hit spacebar bump split line I'm back there right super nice. Okay go ahead and grab my spline I'm just gonna go ahead and start doing some fancy detailing natural curve I'll make that construction and I'm just gonna go ahead and offset that I'll say bi directional because I want to give it thickness, okay, green check, and then I can go ahead and take that and say split line again and I'll project that onto those two faces. Alright. I'll go ahead and hide that sketch and this is where I love this extra little tab up here. If you guys don't use this, I highly recommend it. It's super nice for turning it on on and off sketches and bodies. Right. There's a little arrow up in the top of the feature tree. You hit control t, you flatten the tree so everything comes out underneath its feature and you can have sketches and all your features raw. Right, you just single click rather than right click and hide and show. Super nice. Okay, great. We split this. I'm now going to go ahead and take these two faces, I'm going to thicken them let's give this a thickness of 10 and I notice what's happening here right I'm getting everything so we do kind of have to run through an offset surface again and I'll choose these two again this is just going to be a copy surface so I'll change that to zero everything's existing on-site on the existing face that's a pretty complex curve that I don't really think we could do any differently maybe a sweep if you have a path but again how do you get that three d path in that same order? Alright, this is something that's only probably done really easy by surfacing. Go ahead and say thicken. Let's go ahead, take a look. I'm not getting a preview. Go ahead and say one side, give it let's give it thirty, twenty, green check, we get a volume now 20 might be a little much right now we're not really keeping to the manufacturing requirements anymore not that we've kind of done the indent or anything so this is just kind of design fun at this point. Okay. One of the things I'm not gonna do is I'm not gonna merge this. Why? Well because that makes doing let's say six more of these much harder. In my circular pattern command right now I can just pattern the body rather than patterning that the six count feature right the surface offset the surface copy the the thickened right You might even not even successfully be able to copy all those commands because that requires right that split line that we sketched and it's unique to that single position. Let's go ahead and say 60 and our spacing this is where we'll have to get a little intentional with our numbers. Go ahead and flip the direction and you can see that get added. Okay. Great. Now if you got the extra material, right, you can always use your other surface that we've got in the background to run another cut surface there. All bodies, let's just choose. Green check. Now did I like it? I might have cut the wrong way. Let's flip that and green check. There we go. K. And then we can run through that boolean command again since they're all bodies and say add all of these together. Alright. We can see those edges and the face of top extend out now. Okay. Great. Let's go ahead and run through another one fun command here which is replace face. I'll go ahead and run another little sketch out in space. Let's make it somewhat curved and let's give that a revolve line and we'll run through a revolve surface this doesn't need to be a body and I can say 180 use my right click menu and change that to midplane, Super nice. Okay great. Let's go ahead and say replace face as a command now I need to choose the faces to replace so I'll choose all of the bumps that I created now do notice right I it's only half of it so in order to kind of hide that existing surface I do need to turn on the future fly out tree and right click and hide through there. Shift and tab shift don't work when we're in commands which is an unfortunate side effect. We'll go ahead and turn that back on, click on this face as the face to replace it with, I'll green check it did I flip these target faces for replacement yes, ah, it's because I'm intersecting Let's do this. Let's change our sketch. Our sketch should probably cause some issues. Let's go like so. And we gotta reselect all of that. Do this from the get go, hide that, replace face, selections. I'll place it with this surface, and now you're not gonna be able to do it for me. Love it. Alright. There's something small that I'm missing in there. That's too why it's not pulling up. I'll hit r on my keyboard and pull up my recents, and I can go ahead and just kinda show you guys what I did with it before. Okay. So again, I've got that existing revolved surface out in space. I do have my ribbed bodies here and then I choose a replace face. Now I don't believe it's because I did only one face here. I believe when I was testing you can do it with multiple, And one way to test that out is just to let's go ahead and choose those faces in here. Green check. It did not like it. So maybe you do have to do it individually. This is a good reminder for me. Place face. One. Two. Replace it with this one. Answered. And there you go. There's your outside complex double complex shape. Right? And as you just wanted this as its own separate individual body, well, then you could run through more servicing to to cut that off from the regular body, send it out to its own file. Right? So ton of custom things that you can do with that. Alright. Maybe we wanna start incorporating this outside surface in as a cowl or something. Right? Then you can give it another thick and and that thick and emerge. Alright now all that's the same body if we choose our breadcrumbs. Alright so, we got about nine more minutes before I kind of hop off. We've got a couple of these questions from Bjorn. Would it be possible to take these shapes convert to sheet metal and flatten these in sheet metal for automated bending? Yes. Well, no. I think in some sense you can, and convert to sheet metal. There's, you can convert an existing body. So most often what you end up doing is kind of build your internal volume and then you use that volume to kind of push out, flanges around that volume. Now when you start getting into some custom geometry with extra, you know, complex spaces like this, I don't think it would be able to turn those into flanges. It would take a little more custom work on that mainly because some of those commands that we have for sheet metal in SolidWorks, they essentially turn on the bend deformation algorithm that we have running and some of the commands that are in SolidWorks don't map to bend deformation and stuff. So might be a little bit more struggle bus on the the convert to sheet metal on this one. You can definitely try it, though. I I would totally recommend, giving it a shot at least with probably the the rough volume rather than the exact surfaces. Would extend surface do the same as replace face for these ribs? It would not. And the reason that that would not do the same thing is if I can go ahead and pull up the same body is let's go ahead back before essentially what an extend surface does is it takes the existing face and extends the geometry of the geometry and you can do this by just doing offset surface let's copy those existing top faces hide everything else and if we do an extend surface, you can choose an edge or a or a face instead of an edge right the face is gonna grab the whole thing all edges essentially kind of the same for like fillets and things like that. Let's go ahead and wrap this down to five and so essentially what it does is it continues pushing that face out into into space as its existing curvature right as I span that out so we can't necessarily like pull it like a clay model if we can pull that face off but we can kind of expand where it used to exist or where it was trimmed back from. I guess we can run an untrimmed surface on this right if I untrim this surface you can see in the back end this all works right well it built it as a rectangle here and then it ran through some sort of trimming in order to get it into our controlled shape that we have. Right. So it trimmed it back into that form. And if I did an extend surface on that, let's see, does it like a distance? Right. And then you can kind of see out in space what that would look like. Alright. And so this this kinda gets to the to the heart of the the essence of understanding surfaces allows you to understand what maybe even an extrude does or a shell. A great example that I have with an with a shell is or even a thicken. Thicken and shell are pretty pretty similar. Right? You can understand that a a thicken or a shell might be, hey, copy all the outside surfaces and then offset them and close it up in order to make a shell. Right? Kind of the same idea. Let's do Nope. Not live one. Actually, why am I doing this? Let's use our thumbnails. This one. Okay. This model I built just to kinda show us show a split line intersection curve and the difference there, but this is offset. Let's do a a thicken. Let's just prove that it doesn't work. If I thicken this to, let's say, a 100. Oh yeah unhealthy right if I hit the green check or now it wants to do it this time around that's funny it accepts it right it last time I did this it didn't like it at all it didn't even say that it was able to do the thicken Why? Because those those corners there was a corner on that thickened whereas right we've got no corners on this surface it's because those radii and the biggest radius of curvature intersect as we offset a certain amount. So one way you can test that is just to hit your offset surface right, change it to that 100, hit the green check and you can see that the offset surface almost has some smart so it's the algorithms pretty good there because it trims itself even though it was intersecting right sometimes I'd even expect on earlier versions of SOLIDWORKS I'd expect that just to fail entirely rather than be able to produce this trimmed corner piece of geometry. Okay. So if you're having problems with shells, if you're having problems with, radius as a curvature, servicing is at the at the heart of that and diagnosing what what goes on there. Russell Zinner says, why not increase the height of the ribs and then cut off the excess with your outside surface? Then it would be done in one trim feature rather than having to pick each face we're replacing. Yes. You're completely right on that in in in essence of trying to reduce the, the commands that you have to run, especially if replace face doesn't allow you to do multiple in that sense. Big thing there is just references. What are you what are you managing? If you end up coming back and changing again, you maybe you you offset that face 200 to be extra. You're still building that extra bit in the in the command and let's say 200 rather than a 100. And if you change the original surface with replace face, right, all you have to do is just change the original surface and everything will update with it because it's dynamic to that surface rather than playing the measuring game again with your numbers. Just making sure, hey, I'm extended far enough in order for the trim to work or something else like that. So that's just the kind of the game you play with with where do you put the effort into and and how do you foresee this model to change, I guess, is even a bigger question. Any good reference material for troubleshooting thicken? I do a lot of complex surfacing that I need to turn uniform thickness turn into uniform thickness plastic parts. Biggest area, pretty much is just gonna be your offset command. Realistically, thicken should, when it fails, tell you the problematic faces. If it doesn't, what I've done in the past is I've just gone through offset a set number of faces. Okay. Does this surface work? Great. Okay. I don't think these are the problematic ones or the thing causing the thickened to fail. Right? If, you know, you offset something and it can't produce that thickened or you can only produce it you can only offset it as its singular face rather than as a group of faces knit together, that's probably the thing that's causing you to fail. And in that sense, what does that tell you what to do? Well, maybe change the radius of curvature, maybe sticking towards the outside. I don't know, kind of dimensionally, depending on what your your conditions or constraints are. So okay. That is it. We got one minute left. Thank you everybody for tuning in. This has been Will with GoEngineer. I'm sure you saw that before, but, feel free to reach out if you have any questions. Your representative, they can get you in right right hands of somebody that can work with you. Or if you need a directed email, w cashen, at goengineer dot com works as well. W c a s h e n. I can put that in chat as well real quick. I hope this was informative. Definitely tons of more information that I can I can go over, if you'd like to go