Name: Pattern Like a Pro: Tips & Tricks to Patterning Fast
Uploaded: 2026-02-26T20:24:10.291Z
Duration: 51 min 25 s
Description: Pattern Like a Pro: Tips & Tricks to Patterning Fast

Transcript for "Pattern Like a Pro: Tips & Tricks to Patterning Fast": Alright, everybody. Thanks for being here today. We're gonna cover a lot of material. We're gonna go really fast. if you have questions, put it in the chat. At the top of your screen, you'll see a little green slot looking shape. It says SOLIDWORKS expert tools webinar. That'll be the one that we're coming up on the twelfth. That will be a transformers themed event. Thank you, George. Thank you, Jeff. It's a cool one. It's it'll be a cool one. We're focused on that. But, Darcey, we gotta hurry because time is money, and you know I love that money. I love that money. Alright. Let's go. The main presentation is about to begin. I just got three things to say. God bless our troops. God bless America. And, gentlemen, start your I'm Steve Darcey, elite applications engineer, expert in three d design engineering, robotics automation technology, and robot man, most interesting man in the world for three d experience world. And I also have done a fireman helmet simulation webinar, which is pretty cool if you haven't seen that. Got a little QR code in case you need to reach me. My name is David Cersley, senior application engineer here Austin, Texas with Darcey, SOLIDWORKS Elite certified. I like to think of myself as an astronaut, professional shark surfer, part time sith lord, and a race car driver. If you need to reach me, there's a QR code on the bottom right. Alright. So here's the race rules. David and I, we're gonna find out who's the fastest. The results are based on the live event from three d experience world. So we had some little kazoos. Whoever liked the videos best, Dave David versus Darcey, made some noise. When they made the noise, we recorded the noise, decibel reader, and then we that was pretty much the votes for the winner. So here's the little setup. We have, of course, SOLIDWORKS. We're using, motion, and you do have to have SOLIDWORKS premium for the, motion analysis part of this. And what we did is we just ran two cars, and depending on what the results were set to will depend on whether the path motor is actually gonna make the car go faster or slower. Alright. So in the agenda, we have different heats, six different heats. In each heat, I'll do a demo. Dave will do a demo or vice versa. And then, of course, whoever voted for the most will decide who wins. So on to heat one. So I'm gonna start off with speed matters, and then David's gonna go with speed matters with the fill pattern. So, of course, you gotta start off with SOLIDWORKS demo with a simple block, and I'm gonna go into the sketch. And in the sketch, we're just gonna do a pattern here. So we'll select on the entities. We'll do a 19 by five. Give it some dimensions and hit okay. So simple linear pattern in a sketch. We're just gonna do a cut extrude through all. Hit okay. And we've got our pattern. So how do we find out how fast that actually is? We're gonna go to the evaluate tab, do performance evaluation, and we'll look at the total rebuild time. So right now, we're here at point five eight. Alright. Then we're gonna do the exact same thing, just a little bit different way. So we're gonna do I've got the cut as a feature, and then we're gonna do this as a linear pattern. And then, again, we'll go to performance evaluation and notice the preview time. The rebuild time is point zero six. Alright. So our results sketch linear pattern is point five eight seconds. Feature linear pattern is point o six. So if you're gonna do it, do feature linear pattern. It's much faster. So then I went down a little rabbit hole on whether blind up surface up to next or through all is faster, and I wanted to just find out what's best. So we took a look at the evaluation results, and they all came out point o six. So for the most part, it doesn't matter which way you do that. Pretty cool. But it's good enough. Alright. So then we decided to do something a little bit even, like, harder. So we're doing a circular pattern in this, and I'm gonna do it in two different methods. So, initially, I'm just gonna do a cut extrude, and the cut is gonna go up to surface. There's a little surface back underneath there. And I do two different cuts. And then after the cut, I'm doing a circular pattern. So you can see it actually takes a little bit more time to do it. And if we go to performance evaluation, I did speed that up. It did take about eighteen seconds for it to complete. So then we're gonna do this a little bit different. Instead of doing a cut extrude, I'm extruding these solid bodies up to surface. So I've got my two solid bodies. And then, again, doing a circular pattern, but in this case, doing circular pattern with the bodies, and I hit okay. And that circular pattern goes fast. No resulting no resulting geometry to do, so it fills in just fine. Alright. Then we gotta do a combine to cut and remove that material. And there we go. And then evaluate performance evaluation, and you see this took thirteen point eight seconds. So when we put them side by side, if I do a circular pattern, it's eighteen seconds. If I do it with the solids, then it's thirteen point eight. So it is faster typically. And in older releases, it's way more faster to do a solid pattern and then do a subtract. Alright. So fast parts equals fast assemblies. Feature patterns are typically faster than sketch patterns, and pattern bodies can be faster than patterning features. That's fast. Nice, Darcey. There you go. Alright. So what I'm gonna show here is what we call a no c pattern, and this turned into a light. So I wanted to start with the same size plate that Darcey had, and that's gonna be sketch number one. So keep that in the back pocket. So I'm gonna do a fill pattern. And when I do a fill pattern, notice over here on the left side, I've got all the properties. And all I've done so far is just select the boundary that I want to put the pattern. And what I'm going to do is I'm going to select my horizontal, my vertical spacing. I'm going to select an edge to start the pattern down, I'm and gonna hit this button that's over on the left. It's called create seed cut. Now when I do this if you haven't used this before, it's pretty cool. I can pick three or four different shapes, and I can control it, especially if I have, a pentagon or octagon. I just set it. But let's match up to Darcey here. So point six two five. Right? Looks exactly like Darcey. So I say, okay. Execute it, the command, d to confirm, and I go to performance evaluation. I can see that right now, Darcey was what? You were what? Point o six. Point o six, and I'm point one seven. So Darcey a little faster, but let's take a look and think about what happens not only when we make parts, but we have to edit parts. And that's where this may become a huge advantage for you. So let's take a look. So speed matters just like a NASCAR pit stop, right? So what if I come in here and I have to change that from a diamond to the hole? Look how quick I changed that. All I did was change the seat cut there in the fill pattern. Now if I wanna change it back, I can. Okay? Now what about instances to skip? So when SOLIDWORKS looked at this plate, it looked at the boundary and it created this pattern. I can turn all those instances on, whether I manually select them or I do a shift select. And if I had to do a hard chamfer here on this plate with a seed cut there, I'd be in Agony City. So here I'm just going to do a right click, clear performance evaluation. And with a circle, notice my time is down to point zero eight. So that made it a little bit faster. And again, I'm a little bit faster here just for the ability to change things. So sometimes maybe you want to be a little slower, but go faster on change because unfortunately we do have change. So I got the plate, and this is where I kind of made a mistake, but I'm going to show you the deform tool, and we'll talk about why that was a mistake later. So I've got my second sketch here. So, keep that in mind. So that was our second sketch. I'm going do the deform tool. But to do that, I'm going to create a copied surface. I'm going to offset zero. Okay? I'm going to come back. I'm going hide the original body. And now I want to deform this surface. Okay? So I'll hit the deform tool, and I'm going to say, okay, use this aligned segment here and this one here to apply the curvature. I'm going to say uniform. I'm going to go pick my surface, and you can see the yellow preview. So I was quickly able to keep the pattern. The holes look good. Pretty happy here. I'm going to deform it one more time, and this will be the third sketch that we use to create this part. So I deformed it one more time with a sec with third sketch. Pretty good. I'll turn off my sketches, and this part looks pretty good. Now to turn it into a solid body, all I had to do was use the surface thicken tool. So now I quickly went from just a surface into a thickened, part. So I got it this thing up. Looks good. Okay. So here's where we run into a change. I wanted to change the shape back to the diamond. Right? So watch what happens here. I just simply changed it and, oh, man, like, Cal Naughton Jr. Said or Ricky Bobby, help me, Oprah Winfrey. So I had to make a quick change. So I'm gonna pick on the face. When I go back to the original body and pick that face, guess what? It's now updated not only the original body, but the curved body we deformed earlier. So I'm moving pretty fast here. So now what I want to do is one more type of pattern to complete this light. So there's my part, and I'm going to do a move copy body, to create the pattern. I'm gonna say seven instances. And when I picked on rotate, something interesting happened. I said 45 degrees, seven instances. I had to go back and recheck the copy box. When I do, there's my cup. Looks like something out of Game of Thrones. Right? But here, all I'm gonna do now is do a cut with surface. I'm gonna cut half of it away, and there's my light. So when we talk about going fast, we used our fill pattern. The other thing is we didn't spend a lot of time on sketches. There was three sketches to create this part. So some of the benefits to you on this are I didn't have to use, sketches when I did this fill pattern. And I put a little asterisk there because we're going to show you a way, if you have a custom profile, how to use that later, okay? And I can quickly change the pattern. Now, the mistake I made on mine was I did the offset surface and then deformed it and then thickened it. I could have just deformed the body. That would have been the better way to do it. And I have full, instance of visibility for adjustments. So those are the benefits for you there. Alright. So then at the at three d Experience World, we did a heat one vote, and here was the results from that first one vote. Alright. So what we have to do is just edit that, PathMate motor. So put the dimensions in, and then we're gonna just gonna hit the little calculate button. It's pan in just a little bit. Let me reset that replace key. There we go. Now we hit calculate, and it looks like blue wins. Woo hoo. Alright. Moving on. Alright. Let's move on to heat number two. Darcey and David. Curve driven, sketch driven, and then David gonna do composite curve. So on curve driven, there's a cool offset option on the surface. So I'm just gonna use that tool, and you see it makes that whole curve there on the surface. But I need to position my hole, so I'm just gonna go ahead and draw in a line in that three d sketch and make that construction. Then we'll go right into hole wizard. The sneaky part about this is I'm just using a three d sketch and position that on the surface first and then move it to where the location is. And that way, it'll always stay normal to that surface. So then we're gonna go into curve driven. We'll just select on the three d sketch. We can make more or less in there. Looks cool. And then make sure you do the face normal and select on the face. That way, all the whole locations are gonna be normal to that face. Turn off our three d sketch, then we'll go into kind of a section view mode so we can actually see all that the holes are normal, and that looks pretty cool. Alright. Another one of my favorites is a sketch driven pattern. And the reason why I like this is because it's very simple. We just put some points out there in just a two d sketch, and then we just go right into the pattern. So we'll do sketch driven pattern. We're gonna use that same sketch with those three holes. We'll pick on the boss and that hole and hit okay. And there we've got them done. So this part goes out to you woodworking peeps out there. That's a little wood clamp. It's kinda cool. Alright. Something else I found out that the SketchRim pattern doesn't have to be a two d sketch. So I'm gonna start a three d sketch. And in here, I'm just gonna select on three points. They can be in different x, y, and z locations. And then after I have that sketch with the points, we can just do, again, sketch driven pattern, and we'll use that three d sketch. In this case, I'm gonna pattern bodies. So the only thing sneaky about that is you usually have to select the point, the reference point that you wanna go about. So now you can see all those little plates are in there. Looks good. And then we just got a simple pattern to finish off one side and then, of course, mirror it to the backside, and we're done. So pretty quick, fast ways to create your patterns. That is neat. Cool. Alright. So what are the benefits? Pattern normal to curved surfaces. You can easily copy from point locations, and you can also utilize a three d sketch, for your point locations on the sketch driven pattern. Go for it, David. Cool. So I'm gonna show you guys this one's called curved driven pattern. We're gonna focus on creating the green piece, and I've got a multibody part here. And this was a jewelry box that I made for my daughter that she said, dad, I need a jewelry box. So I thought, oh, this will be easy. But then I ran into problems and thought, crap, let's see how this worked. So I'm going to show you both the errors and how I fixed it. K. So I started out. This is that middle body, and I just did a cut. Now key point here, make sure you do through through all. And because it's a multi body, I just selected the body I had open here. K? So you do not want to do up to surface. Up to surface, again, will not work when we try and go around the corner. So I thought, well, I'll just do curve driven pattern. I'll go pick that feature I just did, the cut, hit the green flag, and guess what? It didn't work. It only went around part of the way because it only used that one line segment. Alright. So option, option one failed. Let's try option two. Right? So I thought, well, I'll do what Darcey just did. I'll make a three d sketch. And I came in here to sketch, pick those three line edges right there, converted them. And I was like, I'm off to the races. This will be great. This will be easy. A neat little trick. If I hold both of those, the cut and the three d sketch down, when I pick on a curve driven pattern, everything is populated correctly. But look what happened again. We got a serious problem. It didn't follow that path. I tried clicking on every button over there to try and make it work. You know, like most of us, we just click on the left buttons and sometimes it works, sometimes it doesn't. In this case, it didn't. So what would work? So what I did here was I tried a composite curve. Okay. So I used the composite curve, and I grabbed those same three line segments I did with the three d sketch. But guess what? The composite curve is gonna look at it now as one single line segment. So when I do my curve driven pattern, I'll go up. I'll grab my composite curve. Notice it went all the around the corner this time. And I can set the direction arrow right there. Cool. Looks good. I'll go grab my cut polygon, and I'll hit the green check. And guess what? It patterned all the way around the corner. So now all I had to do was add another cut. I went over to the feature tree. I reorganized my feature tree. I added an additional cut. I have to add that back to my original pattern. And guess what? There's that body. Now to make this, this is a square part. So all I did was a mirror and I checked the merge entity. So once I did that, all I had to do was come back in here, add a few fillets. So, started out trying one thing, that didn't work, tried a three d sketch, that didn't work, and it was the composite curve that allowed me to make that around the corner. So, again, some of the features and benefits to you, the end user here, is I I can can get a pattern to go around a corner, which is really cool, and it's symmetrical. It's great if I'm doing something like a multi body part modeling like this little jewelry box, and it made it easy for when I went ahead and three d printed the part. So pretty good. Hopefully, you guys saw something there. So here's where we did the second round voting. It was Darcey versus David, and, everybody blew on the kazoos, and Darcey went ahead and updated the the race information. Alright. So we'll make our little changes in here. Add this for heat number two. I'll go ahead and reassign where the orientation is and calculate. So there we go. David started winning at the beginning and, oh, he pretty much tied. So I caught back up on heat number two. Well, it's gonna be a tight race today. I feel I feel the need for speed. Alright. In this one, I'm gonna show you guys how to vary your pattern using the sketch. Okay? And then Darcey gonna go into variable pattern as well. So let's take a look. So, this is a part here, Darcey gave me. I think a coworker had done it, but let me kind of back you into what did here. I made a solid body with some lofts. I cut it in half. I did an offset surface. I'm going use that surface to extrude up to. I then did a sketch on the mid plane and I projected it. I did a split line. So now I've got two regions. I want to create a cavity from that first region, so I did a surface cut. Okay? So then when I cut it, I went ahead and filleted the corners. So that's all I did to create that cavity. Now here, all I'm doing is I'm doing an offset sketch, and I'm gonna offset it one millimeter. Alright? So real quick, real easy. Here's the key for us. I'm gonna go ahead and put this little slot in here. The tangent relationships are what's gonna be key to us here. I'm also going to set this, dimension here to eight, and I'm going to use this to set the direction. Now I need to fully define this guy, so I'm going go ahead and put a radius on it. And notice that I've got a fully defined sketch. Okay? And what I want is this slot to go, in this case, left to right and follow the orientation of that offset sketch. And in order to do that, I needed that tangent relationship in there. So let's see how that's gonna work for you. The first thing I had to do was create a solid feature in order to pattern. So I just did a feature, and I said extrude up to surface in that original surface. So again, my grip is maintaining the shape of the original body. So I'm gonna do it a linear pattern. I'm gonna pick on that eight, and that's gonna set the direction. On the left side, under options, check very sketch, and that's the key here. I'm gonna come up. I'm gonna set, the number of instances, and I'm gonna do an up to vertex. I'm gonna pick the vertex on the far end of my cavity, and I'm gonna say, hey, I wanna stay off of that by three millimeters. And where am I gonna pick this other little vertex? I'm gonna pick this other vertex. It's gonna say from here to there. Right? And I'm setting everything up. Now by doing instances like this, I can go up or down, and I can just quickly control the number of grips. Now this is great because what I can do is I can set these, and overnight, I can print three or four versions. Right? So to finish this off, all I did was a cut through the middle. I filleted the ends of it, and it's all set to go. The nice part about this is if I wanted to make five or six or seven configurations go home, a lot of the printers are running, the next day I can come in and have folks test out this grip to see if it which one's the right fit. So, hope that helps you. The the advantages and the benefits to you guys here is this. I can update the patterns without editing multiple features, and that's where we're going fast. Again, the more features that you have to edit, the more likely you are to make mistakes, and you're also likely to end up with a bunch of ketchup and mustard in your feature tree, and we don't want that. So this keeps your patterns up to date, reducing those rebuild errors. Cool. Alright. So I'm gonna show you something that's kinda cool that I didn't know. But notice that when you do just a linear pattern, you can actually use lines, axis, dimensions, and circular faces to set the orientation. So this is just quick little tip. So I'm doing just a linear pattern, but I can select this the cylindrical face, and it's using kind of the axis of the cylindrical face for the direction. So I just put five of those in there real quick just for the heck of it. Alright. Now let's get into the very pattern. So I've got two features that are sitting in there right now. The variable pattern kinda what the way it works is it just uses a table. So I've got my table. I'm gonna just add a new row, and we can just put in what the x and the y locations are. So I'm gonna make one go up 15 millimeters or I'm sorry, negative 15 and then up 17 millimeters. So I've got three of them in there now. But the cool thing is for all you Excel spreadsheet lovers out there, we can actually import an Excel spreadsheet. So if you can do all your equations and stuff in Excel and then import the table. So we I actually did that, three d printed it. It didn't feel very comfortable. So I went back to Excel. We'd made one that had a straight pattern grip. So give that a second to load in. We'll update that preview. And notice I'm not only varying the location and the height and the width, but also the sketch dimensions. So a lot more versatile and fast. Alright. So that looks pretty cool. And that's a variable pattern. So the benefits are, of course, it utilizes Excel spreadsheets. It dynamically controls all pattern instances all in just one tool. Alright. So now for heat three vote. So we got our results. We need to make our changes. So I'm going down to heat three and put in 73 inches for that one and sixty six, and then we'll hit the calculate button. We'll go through each of the different heats. So David went in. We tied on heat two, and David pulls off. He actually won a little bit. Woo hoo. And v three. Looking good. And now a public service announcement. We would like to talk to you about a subject that affects two out of every one engineers. Have you ever had to make a pattern and said, nope, not today, Satan, or just unplugged the laptop? It's called trypophobia, the fear of patterns. What do I do? Never fear. There is a cure, and it's called Patternol. David, that's amazing. Are there any side effects? There are. Joy, happiness. Your feature tree will be free of ketchup and mustard. Puppies will like you. I guess in some adverse cases, stomach pain and explosive diarrhea. But don't worry, you'll be okay. Sweet. I'm gonna eat many right now. Cool. This'll have you seeing patterns in no time. Trappophobia and paternal. Alright. Heat number four. We're gonna talk about smart components and pattern driven component patterns. Alright. How many of you are using smart fasteners? If you can just chime in on the chat. But the the advantage to using smart components is the ability for us to be consistent as not only individuals, but as a team. So how do we do it? I'm in an assembly. I'm gonna say smart fasteners. And what I'm gonna quickly do is I'm gonna just hit add once I pick this face. And you'll notice that when I do that, I can add top stack or I can add bottom stack components and the bottom stack being on the backside. So if I pick bottom stack, I can come over here and pick a a washer. And notice as I pick these items, they appear right on the back. And the good news is when I go to do a bill of material, all these will be accurate. Right? So now I've got my washer and I put that on the front. We say, okay. So that's kinda first step. I've added my hardware. Alright. So what's the next step? The next step is I'm gonna make a smart component at the assembly level. My smart component is this connector. The components are gonna be all the screws, nuts, bolts, washers, whatever that I want to go with it. So notice that they turn like a magenta color. Cool. And they're automatically populated. Now the features, I want this advanced hole that I've got here and this hole pattern. Now in this case, it did make me select the other hole patterns, which was weird, but I would have thought it would have grabbed all of them. But over at your component level now when I go to the connector, look what I've got over here on the left side. All those components are with it, the advanced hole, the the screws, nuts, bolts, everything. So back here at the assembly level, let's implement this change. K? So here's my smart components, and I'm gonna insert it. Now you can do this a myriad of way. I just did a control left mouse drag and hit the green check. Now you'll notice that I've got a little lightning bolt here. If I pick on the lightning bolt, SOLIDWORKS says, hey, David, what's the initial face? What's the ending face for my cuts? Right? Because I've got those advanced hole cuts that I wanna bring over in the hole pattern. So when I hit the green check and I rotate this around, guess what? There's all the hardware. I can see that the hole came. But what about my hole pattern? So if I come in here and I hit shift tab or tab, I can hide a body. So I can see that the whole pattern came through. And if I hold shift tab and hover it over where I think a body would be, guess what? It reappears. So the advantage here is I was able to add a connector and, you know, 16 pieces of hardware in just a few seconds, and what I could be super consistent, and so can the rest of our engineering team. So I hope you find that useful. The benefits here again, faster assembly creation. You saw how quick it was. My BOM is gonna be up to date. I've got reduced errors and reworks, and I've got can make this with configurable designs. Alright. So I'm gonna do pattern driven component patterns. I like the smart components, so I'm gonna kind of go the same way that David did. I'm gonna do a coincident mate real quick. Just plop that guy inside there and then hit the little lightning bolt to insert the smart feature. And in this case, it's creating the hole for that bolt. So all I have to do is select on that top face, hit okay, and now I've got my my pattern. Cool thing is if you drag this guy around and just hit the update button, then it's got to create that hole in that new location. So just to put it in the right location, let's put a concentric made on there. There we go. And it's up to date. But now I want the hole in all the different years. So let's open up the part in its own window. You can see the smart feature is in the feature tree. So I'm gonna drag it up above the circular pattern. We'll edit the pattern and just add that hole to the the pattern for the ears. So now it's in all four of them. That's great. Save that. But now I don't have the bolt only in this the first one. So we're gonna do a pattern driven component pattern, which means that the assembly is going to link to the part. So I just need to select on that ear. And if there's four ears, then there's four parts. And so the cool thing is I can change it. So just double click on that dimension. We'll see what five looks like and rebuild. So I got five ears. Do six. That's cool. I wanna bring it back down to four. We just wanna make sure that everything updates right. And there we go. Save it and close it. So the benefits here, the assembly is driven by the part pattern. It's faster updates and rebuilds, utilizes smart features, and the BOM bill of material is always up to date. Alright. So heat four vote. Let's go. So we have to add in the the fourth heat there. Let's go change some of these dimensions, and we'll just recalculate. And here we go. Round heat one, two, we tied, three, David started taking the lead. Oh, yeah. And four oh, I'm coming around. Oh, man. Coming around the end. Who's doing the voting in this thing? Who in the I disagree. I disagree. Alright. Moving on to heat number five. Go for it. Alright. So we're gonna go back to that fill pattern. We're gonna use a custom feature, and then Darcey gonna show you some awesome stuff with three d textures. So we're gonna make this grip right here. Okay? We wanna make a prototype of it, but what we're gonna do is we're gonna focus on that green area. So I've already got that pocket, and I've got this surface here. Now we've I've offset that pocket surface by zero, copied the surface, basically. So what I need to do is a couple things. I've made my part symmetrical, and I'm gonna have to flatten it. So the first thing I'm gonna do is I'm gonna use an intersection split line. I'm So gonna grab the plane that's going through the middle of the surface, and notice that yellow line? That's gonna be my my line here that I'm gonna flatten from. I needed a point of reference to flatten from, so I created that with that line. So when I go to surface flatten, which is in SOLIDWORKS premium only, notice anywhere that I picked on that original yellow line, it's now pink line in this image here, wherever I pick, SOLIDWORKS flattens the surface from. So I can come back in here and hide that original surface now. Okay? So let's do that. Let's come in here. We'll do shift tab and hide that surface. I'm gonna come in and I'm gonna thicken the body, and I'm gonna thicken it the same as my cavity depth, the point five, and I'll hit the green check and make sure merge result is unchecked. Now I'm gonna advance this just a little bit. All I did was make a sketch with a cut in it. Now I've got a custom feature. I'm gonna use fill pattern, and I'm gonna set the options over here on the left side. Okay? And just like we did before, we set all our options. And over here on this time, what's gonna be different is what I wanna pattern is this original cut, but I need this directional arrow here or the direction for the pattern. Okay? So I'm gonna zoom in. I'm gonna pick on that cut that I just made. Okay? Great. And now I can see that it's gonna pattern. I'll pick the surface. And the cool part is notice over here on the left side, it gives me an instance or a validate count. It tells me there's a 103 instances of this in here. So now I can go back and adjust the spacing and then get a different count for different grip prototype testing. So when I hit the green check, now all I have to do is the hard part, and this is something I screw up every single time. I'll go to convert entities with a new sketch, and I'll say inner loops one by one, and I'll pick the face. Where I fail to do is I always fail to hit that inner loop. If you don't, it just gives you the outer profile. But if you select it, guess what? It grabbed all those inner profiles. So I'm gonna turn that sketch off for a second or that surface off, that body off rather. Turn it off, and now I gotta get that sketch onto the grip. So how are we gonna do that? And we're gonna use a tool called the wrap feature. So what I wanna do is I'm gonna come down here. I'm gonna hit wrap. I'm gonna come up here. I'm gonna grab my sketch, and then I'm gonna grab the body or the surface that I wanna go up to. Bonk. There it is, and I got a preview. And I'll set whether I want it embossed or debossed. And down on the left side, I can set the accuracy of this. Just for speed of today, I'll go ahead and hit, low accuracy. And all I have to do is hit the green check and see how quickly I was able to get that on there. The nice part is if I needed to create a bunch of prototypes of this, I could play around with the settings, print them overnight, come back the next day, and decide which one of those grips is best. So the benefits of using this is I can use custom feature profiles, on that fill pattern, and it's great for prototyping and three d printing. Again, I can just create a whole bunch of different versions, print them overnight, and test out the next day. And I did all that, by utilizing the wrap feature. What you got, Darcey? I got something cool. Alright. We're do some three d texture. So I'm gonna use my little handle grip here. And right now it's flat. So we're gonna kinda go through this step by step. And the first thing we need to do, I wanna put a neural pattern on here. And in SOLIDWORKS, if you go underneath here, we have some three d textures that are automatically included. And when I drag that on, make sure you apply it just to the face. And then it's always gonna be a little bit weird, so you have to go in there and edit the appearance. And on the mapping, I'm gonna kinda straighten that up. First, I'm gonna tell it to map on the surface and not projection, and then we can scale it up and down. And the main thing here is the difference between the white and the dark. So when you're chick choosing up a texture, make sure that you have something that has very highlights and very low darks. Alright. Then we just right click on the solid, go to three d texture, check the box for that, and then you could see the distance. We can make this really tall if we want. We can also change white up and black down or vice versa, and then we can also change the element size. So in this case, depending on what type of three d printer you're printing on will depend on what your texture needs to be. So that looks pretty cool and pretty easy to create. We'll go ahead and make it a I like it that that cyan color. So we'll save that. Change it to where we just see the the faces on that, and that looks great. So pretty easy to create a pattern. You can make pretty much make a pattern on anything with a JPEG, black and white JPEG. So here's some other things that I did instead of just the the diamond pattern. You can also do dimples. You can also remove the dimples just by hitting that reverse option and hitting the okay checkbox. So what are the benefits? It's great for three d printing, reduces amount of features, and quickly utilizes complex patterns. Alright. Heat number five. Let's vote. So let's see what the results came out for heat number five. Cool. Around the corner. The corner. Down the backstretch. And then I was catching you on four Oh. And five. Looks like you're get a victory, Darcey. That's right. And you know what, Dave? Can I win all the time? It'd be great if I could win and be number one. Number one? You can't be number one, Darcey. Because if you're number one and I'm number one, that makes 11. Oh, yeah. Okay. Well, you can win then. Alright. So heat number six, we're gonna do a lattice and visual scripting. That's some pretty cool stuff. So let's get to it. So here we go. Why lattice matters? It enables fast, lightweight, strong structures. It has a really good workflow with SOLIDWORKS to CATIA to three d experience, and it's ideal for additive manufacturing. So how do we do it? We, of course, get into SOLIDWORKS. There's a couple of different ways we could do it. I'm just gonna do this with the surface and extrude that. And then want it on the other side as well. I'm gonna do two different patterns. So I'm just gonna mirror it. And that's it. Then we take our SOLIDWORKS part, and we're gonna save it up to the three d experience platform. I like to put it into my Lattice bookmarks so that way you can find it easy. And then once it's on the cloud, then we just select on the Lattice design role, and that's gonna automatically start up Katia in the Lattice design role. And then I can just drag and drop and open that thing up in Lattice Designer. Alright. We'll maximize CATIA. And then this is actually a SOLIDWORKS part, so I can't make changes unless I do what's called an abstraction shape. So in the abstraction shape, I can make extra little additions to the feature tree here. So we're gonna copy that in there. We're gonna close-up these surfaces. So it's just a real simple way to kind of make these things booleans. That's where the lattice is actually gonna happen in here. And then five quick easy steps for lattice designer. What heart body are we gonna do it to? What are the different cavities? So here, I'm just gonna select on these volume cavities. So one there on the right, and then we'll make another one on the left. So it's looking good. And then now that I have those two in there, I need to tell it what am I gonna do with each of those. So am I gonna do it with bars or TPMS? TPMS is surfaces. And then we have different options for the different cells. This one, I'm just gonna use cubes. And we'll go ahead and do the one on the left, and we'll do that one as diamonds. We have a lot of different options for the length and the radius, and you can also orient it in different directions as well. We'll say okay to that. Concept information is just some, options on how much filling is happening to it. And then step number five is just the decimation sag. Hit that and hit okay. So pretty quick and pretty easy. This would be very difficult to actually model up, especially when it hits those side faces. You have to put all those fillets and stuff on there. So this is a really quick easy way to make lattice designs. Now I went ahead and did an update to it just to make a a really cool shape, and it it's pretty fast. This took, I think, about a minute and a half to actually create that lattice structure. How long would that take you in regular SOLIDWORKS? It'd take you a really long time to make these models. I would have to hire somebody else to do it. I would not wanna do it. So some other lattice applications, if we did surfaces, we could do some stuff for heat exchangers. You may actually be buying some sports applications that already have some lattice structures in them. And any medical applications, you're gonna start seeing these in more and more stuff as well. Alright. So the benefits are, of course, create complex lightweight bodies, reduce modeling times, three d print manufacturing, and optimize design for strength to weight ratios. Alright. Cool. Next, we're gonna talk about visual scripting. And if you had to make this part in SOLIDWORKS, well, in the words of Ricky Bobby, are you kidding me right now? And for those seeing visual scripting for the first time, here's a little sneak peek. Mike Britton is going to have a webinar coming up. Stay tuned. Check out the GoEngineer calendar. Mike's gonna be doing one on visual scripting and Lattice, and I think it'll pretty much just, like the rest of us, make our heads go, wow. I can't believe that we can do that now. Keep your eyes open for that, but this is what visual scripting looked like. I've got the model over on the left side, and over on the right, you can see what we have on this gray screen. These are what we call the operators. So let's take a look at it. So last year at three d Experience World, we created this rocket, okay? Our space exploration rocket. So what we want to do is get this individual scripting from SOLIDWORKS. So we're going to pick and we're going to do some surface, right? That offset surface or copy the surface. And now I'm going to bring this up to the three d experience platform. So once I've got it, I'm going to save it into my bookmarks. Know we're a nice, easy way to find my part, right? So it's in three d experience. I'm gonna go over here to the left side. I'm gonna click on the compass, and I'm gonna open up the app, visual scripting. When I open up visual scripting, this is a Katia based role. There's my rocket. Right? And so now what we wanna do is start to get this guy in here. And what we want to do is we want to play around with generating like a really organic, heat shield. So let's let's isolate this surface. And then let's start playing around with visual scripting. So here's my surface. I'm gonna go down here at the bottom, and I'm gonna pick on visual scripting, say, okay. Now over on the left, what we're used to when we do stuff in SolidWorks is a feature tree. Over on the right, what we're doing is visual scripting, and these are called operators. Think of the operators as just a feature in your SOLIDWORKS feature tree. That's how I explain it to myself. Hopefully, that helps you out. So now what I want to do is I want to start to divide this thing out. I want to create these subdivisional surface, and I'm going to use these points. Now I have all of these operators and notice that I'm drawing a line between them. So I'm saying, hey, do this and do the next thing and do the next thing, just like in SOLIDWORKS where we have features that are referencing each other. So what we're doing is we're doing Voronoi, we're creating boundary surfaces, and I'm starting to, if you watch over here on the left, as I create this script over on the right using the operators, I can start to see that this surface is now being broken into smaller pieces. So what do I want to do now? I want to put some fillets on these corners. So I'll set the corners. Pretty good. And I set the radius. Okay, great. Now the next thing I wanna do is add another operator, and I wanna go ahead and fill, and I wanna add these to get some volume to them. Right? So let's go ahead and say, let's do this. Now, if you've ever done this in surfacing, this would be a great addition to SOLIDWORKS to be able to add draft to a surface when we extrude it. But look how quickly with just a couple operators, we were able to take that flat surface from SOLIDWORKS and with just a little bit of scripting, we were able to create this heat shield. But we're not gonna just leave this alone. We're gonna try and take it to the next level. So now what I really wanna do is to get something that's less mechanical looking and something very organic looking. So let's start to tinker and let's see what happens here. Here, what I'm going do is I'm going take one operator and reconnect it back to that pattern, right? So now when I go in and look with just a couple simple operations, think about how crazy that surface would be to create in SOLIDWORKS. And each one of those, you know, has some crazy patterns, some crazy shapes, and they have drafts. And I've got nice spacing, and I can quickly control how that looks. Look at that surface. That's pretty awesome. So that's a visual scripting if you haven't seen that before. Again, be on the lookout for Mike's webinar here in a few weeks. Some use cases. Folks in the automotive industry are using it. People who use it to design buildings, things like that, they're using it as well. When we talk about visual scripting, the benefits here is I can automate complex geometry. You guys saw how quickly it was to create that. We use SolidWorks, GATEA and the three d experience workflows, and it works seamless. What you saw there was was no punches, no clever editing, just as it was. And I can capture and reuse engineering knowledge over and over again. So, pretty pretty nice way to do it. Alright. So the final heat This So, coming down to the last we had everybody vote with their kazoos, and let's see how this race turns out. So here we go. I think they kinda like the visual scripting a little bit better. Yeah. It's it's close. It's so close, and we're gonna have to find out here. I'm gonna need a lot to catch up. Yep. I was winning at the end. Heat number five. There we go. Uh-oh. Slingshot. Engage. Shake and bake, Darcey. Shake and bake. Woo hoo. All right. I wanna thank everybody for coming today. We know we showed you a lot of stuff. We're gonna go ahead and start, if you wanna unmute or put something in chat, we'll go ahead and start answering all the questions. If you need to reach us, there's our QR codes at the bottom. And again, thanks as always for being here. Thanks guys. Shake and bake. Shake and bake. one of the questions that they asked was, you know, how, like, performance wise or stability issues with patterns. And it looks like a couple people were actually have your trichophobia with afraid of patterning. They don't wanna do it. But Yeah. I mean, get some the most all, and everything will be good. just get some pattern off. Yep. But, Yep. yeah, you know, patterns, you know, they're just they are finicky. They're almost like a cat. You know? Sometimes you feel like you're clicking the right buttons and anything it fails. You got ketchup and mustard, but just a few best practices usually cleans that up. You know? Yeah. I kind of agree. That's if if you do them the right way, then they're just as stable as extrude. and revolve and that stuff. But if you do them on some weird kinda ways, then, you know, they can get a little bit finicky for. sure. Thanks for all the great comments and questions over in the chat during this event. There's been. some great questions over there. Yeah. Looks like we got them all answered. It let's see. I like that, Don. Don's gonna take some Patanol. Alright. That's hilarious. Apparently, that was a hit. Yeah. I see Jeff Jacobs over there talking about the deform tool. Very interesting. I'm looking forward to watching it back and trying it out. Yeah. The deform tool is is very, very powerful. Again, Yep. I wish I had done the mistake I made there, Jeff, was I made that by making a surface in another body. What I should have done is just deformed the original body, and that would have taken out that whole error that's in there. But I left it in there because I screwed it up, and maybe my screwing up or learning, as I would like to say, is hopefully helps you and you don't do the same thing. So Yep. it's a cool one, and it it did a really good job. You notice it didn't really make goofy shapes out of those that pattern when we wrapped it around there. Again, allowed us to change the pattern fast. So great. Yeah. When of the questions is when was the form tool available? I think it's been there for, I'm gonna say, eight, maybe nine years. It. used to be very finicky, but over the last couple where you actually have, you know, where it's going from and where it's going to, it's been quite stable. Yeah. I was thinking my first my gut reaction, Darcey, was 2015 to 2018. Somewhere in that window, so. we're probably close to that. think you're right about that. Mhmm. It is not a premium feature. It should be in every version of SOLIDWORKS. I just came from SolidWorks '20 one premium. I've I've been trying to get to speed this last week, and half of these new features alright, Jim. Well well done on the upgrade. If you need any help, just reach out to Darcey or myself. We're happy to schedule some time with you and show you some tips and tricks along the way. That goes for everybody on here. We teach you how to. make a wire mesh basket. Yeah, John. Reach out to us. We were happy to, schedule some time. And it it usually, these things are are trial and error, and you learn. I guess it's like the the the Matthew McConaughey green light books. If you learn what you're not, then you'll know what you are. And in SOLIDWORKS, if you know what you can't do, then you'll know what you can do, and then you'll fig we'll figure it out. So we're happy to help you with that. No problem there at all. Smart fixtures, can you add a parameter so the screw length can change depending on the thickness of the material? So kinda what I did is I put a smart fastener in for, like, say, for instance, a bolt. So it's actually just creating the cutout for that side bolt. So I would actually I can do configurations on the bolt. And depending on what the bolt size is, I can have configuration of all sizes. You can add I believe you can add multiple smart features. So you if you add different tolerances, you may be able to do that. I'd I'd have to do some testing on that, though. Say, for instance, you want something that's a little bit tighter versus looser, may have some changes on that. Alright. Yeah. Thanks everybody for being here. We appreciate you. Again, pay attention to that GoEngineer. I believe it's forward slash calendar. Look for upcoming events. And then the next one Darcey and I will do will be, I believe, in just, like, two or three weeks. You can click on that link at the top of the screen there. It says SOLIDWORKS expert tool webinar and register for that one. We'll see you there. Yeah. Thanks, If you. like if you like transformers, that's gonna be a fun one..