 I occasionally receive requests to do videos on how I would approach a particular model that's been uploaded to Thingiverse or similar sites. So I've been thinking of doing a series called How It's Made, or more accurately, How It's Designed, where I take an existing model and show how I would tackle the design in Fusion 360. I would take requests and then pick a design to tackle. If this is something you'd be interested in me doing, then let me know in the comments. I'm putting together a list now, so if you have a model that you've been wanting to tackle but just didn't know how to begin, then leave the link in the comments and I'll take a look. Depending on the project and of course giving priority to my Patreon supporters, I'll make a decision on which ones to do a video on. So today's video is kind of on the same realm. In my weekly live class, which I've linked below if you're interested in checking it out, we decided to tackle this Spider Bowl by DSK001 posted to Printables. Now, no way am I going to cover this entire design in one YouTube video, but one of the features I thought would be fun to tackle is the spider web that's patterned around the bowl. Here's my finished design of the model. The spider body was created in the sculpting workspace and therefore is this complex shape, which means I won't be able to simply use the emboss tool. There are some other challenges we'll face to get this pattern, but I'm going to address each one and hopefully introduce you to some new tools that you can throw in your design toolbox. Now, I will emphasize that this will be my approach to this design. I don't know what approach the original designer took or even what software they use. All right, let's jump right in. We'll begin by creating a sketch on the front plane. That's our ZX plane there or that blue-red plane. P4 project and I'm going to project that front surface there. Click OK. Untaggle bodies and that'll give me sort of my boundary there to see where I'm designing. And it makes it a lot easier to see your sketch lines when you untaggle body here. All right, I'm going to begin with a circle. So C for circle, I'm going to create a circle here and give it a diameter of 60 millimeters. And then I'm going to take this circle and vertically constrain it to that origin point there. So I'll grab my vertical constraint there, click on the center of the circle and the origin. Now it's locked to the center and I'm just going to eyeball it into place here. You'll notice throughout this design, I'm not going to be so strict with constraints. This is more of this sort of organic shape. So I'm going to do things that I wouldn't normally do with ignoring constraints here. Okay, now I'll create two more circles and I'll give one a diameter of 40 millimeters and the other one a diameter of 20. I'm going to come in with a line right from the center of the circle there. I'm just going to make a diagonal line here and then I'm going to take that line and I'm going to do a circular pattern. So create circular pattern, select my line and then my center point, I'm just going to select the outer circle here and create 12 of those. Okay, and since I have 12, you'll notice that the dimension here or the angle between each line here is going to be 30 degrees. Alright, next I'm going to come in with my arc tool. So I'm going to grab a three point arc. Now choose one of these segments here and I'm going to create an arc between the two points in here. I'm just going to give it a little bit of a bulge here. I'm not going to again worry so much about the diameter there. If it's snapping into a certain position, just hold the commander control button and that'll give you free, you know, it won't lock it into place, just allow you to kind of set it. Okay, so three arcs and I'm going to come in again with a circular pattern and choose these three arcs and my center point, I'll just select the circle here. Again, create 12 of those and there we have it, something that's resembling a spider web. Now I'm only going to keep what I need here. So it's going to make it a lot easier when I go to select things later. If I just delete stuff I don't need. So I'm going to select this outer projected line. I had made click delete and I'm going to delete these three circles as well. Alright, and then I just have sort of my web features that I need. Finish sketch. Alright, now I have this sketch and I have this body. Here's what I want to end up with, right, is getting this web feature on the outer surface here. So to do that, there's probably like a few approaches you're thinking and I kind of went through each one of these. Really quick, I'll show you some of them that I thought about doing. For example, you may think of, okay, emboss this onto this surface. So create, emboss. The problem with the emboss is it wants to select profiles. So you can see here I can't select each of these lines. What I want is those lines projected. So I can do, for example, a profile. But then I run into another problem where the emboss does not work on complex curves. So if I select faces, it's not going to let me select the face here. So that's out of the question. The other thing I thought was thin extrude. So thin extrude can kind of, well it starts to work, but another issue I hit was, so if I do, instead of profile plane, I do object and I select this object and say a negative one millimeter thin extrude here, it just, it wasn't working for me. It kind of thinks about it and it gives me an error that that's not going to work. So I tried a few other things that didn't work. Let's go straight to what did work here. And this is a tool, I don't know if you use often or you may not even know exist, but it does come handy. And that's going to be our project to surface tool. So the way that works is first we need to create a new sketch. It cannot be the same sketch as that our current sketch is on that we're trying to project. So I'll create another sketch and I'll choose the front plane again. And that's on tiger bodies here for now. And so we're just seeing, I only need to see this. Yeah, the second sketch there. Alright, so what we're going to do now when you go into a sketch, you go down to click create, go down to project include, you'll see an option here project to surface. So we're going to choose that. And let's go to curves first. Now, I'll click on curves and I'm going to go to select here selection filters, uncheck select all and I'm just going to do sketch curves. That's going to make it easier for me to just drag and select. And it'll just select the curves and no other points or anything else there. And you'll see you should have 48. Alright, next I'm going to choose project direction. And this is the direction I wanted to project. I'm going to want it to project along the front face. I'm just going to choose this y axis here. Be careful. It's not letting me select it. That's because I have to go back and turn selection filters back to select all. Alright, now I can click to select it. Now I'm going to choose my face that I want that to project to. And that's where I'll bring in the body. And then I'll click this face here. And then there you go. You see what it did there. I'll click okay. And it took this flat surface here, this flat sketch, and it projected it. Let me click finish sketch here. It projected it right onto the surface here. So if I untoggle that body, you'll see that this now matches the curve of my body, which is great. So no matter what shape or how complex that curve is, it's going to take that flat sketch that's in one plane and project it here. So you can see that with this sketch, I can select different profiles because these are all on one plane with this. It's all on separate planes. So great tool to take advantage there when you need it. Okay, now what we are going to do is we have this sketch on this surface. And here's the other challenge is how do we get the web to happen here. So a couple of options you may be thinking here. One thing that came to mind was using my thin extrude tool and selecting profiles. One issue with that is it's kind of teased. It doesn't let you sometimes select more than one line. So if I do like a negative one millimeter extrude, I can get it to actually come in and create an extrusion there. But then I have to do these individually, which is just, you know, that's going to be quite a bit tedious. So let's not do that. The other option you may be thinking is pipe. So let's go down to the pipe tool. Kind of the same issue. It doesn't let you select everything. It'll let you select maybe, you know, two or three depending on what you select. But you can see here, there's a lot. It's not letting me select. So you'd have to do these in sort of different sections in here. It's not even letting me create it. So at the end of the day, it's just not going to work. Let me see distance negative one, actually. Let's go the other way. So at the end of the day, this didn't really work for me. However, I do know that the pipe tool works a bit differently in the sculpting workspace, as it does in the solid workspace here. So that's what I ended up going with. We're going to jump in the sculpting environment here by clicking on the create form button. And here, what we can do is grab our pipe primitive here. And so I'll choose pipe. Let's go to a front view here, and then I'll drag select everything. And at first you may get, I think usually to the fall is like 20 as your diameter, and you may get something that looks like this. So all you have to do is change that diameter. I'm going to change it to one millimeter. And you see here that it was able to select everything in just one click and drag. So it makes it a lot easier. However, let's say, let me see. Let me go with display mode as smooth here and type square and then click okay. So here now we have, you know, this is perfect exactly what we need. And if we click on finish form, we're going to hit one of our walls here because there's an issue there. It's saying, hey, we can't convert this. So it wants to convert this to our solid body can't do it. So we're going to have to click on return. And the problem ends up being, I believe, is at this point here where you have sort of these intersection of these three bodies, it just can't solve that. That doesn't mean we have to quit here because I think there's another way around this. So I'm going to undo. I think if we just make these in two different operations, it can work by avoiding having to calculate these three intersections here. If you know of any other way, let me know. But this is the way I'm going to go about it. I'm going to go back again to create pipe. And I'm going to select just the outer portions here of the web first. So unfortunately, I have to kind of click these one by one. If I did have, let's say I have these in separate sketches because I'm trying to avoid these lines here. If I had them in separate sketches, I can just go ahead and drag and select. But because they're all in the same sketch, I'm just going to have to come in and select them one at a time. No big deal. We'll just go ahead and do that. And if you accidentally select the wrong line, just click it again and it'll deselect it. So okay, now that I have that, I'm going to again, display mode. I'm just going to go with circular error or what's it called smooth. And then end type, I'm going to go with square, click okay. And there we have it. And I'm going to right click repeat pipe. And then I'm going to go back and select all the lines here. And so basically, I'm just going to do these as separate operations. And once I have them all selected, I'm going to come here, display smooth end types. So here look that you can see that these are open. If I untargle bodies here with my first one, see a little bit better. So if I bring that over and convert finish and click finish form to convert it, these will actually come in as surfaces and not solid bodies. So I have to change the end types here from open to square. That'll close that up, click okay. Now I have, you know, these two bodies here. And let's try that finish form again. And drum roll, yes, success. So it works, comes through. And you can see here that we've got all these different bodies. So let me untargle sketches here. So our main body and then these separate bodies here for our web. And what I'm going to do here is now I can combine them. So modify, combine. I'm going to select the lines here first, going out and then make that my target body. And then my tool bodies, I'll select all the other intersecting pipe there. And then click okay. And make sure, actually, let me just go back and make sure that your operation is joined and you have keep tools not checked. Click okay. And you should see here that these three bodies all collapse into one. And there we have it. So now we have these two bodies. And what we can do now is take this and do a circular pattern. So create pattern, circular pattern. And our axis there, I'm just going to choose our Z. And let's see. Oh, bodies I haven't selected yet. Let's choose our object. And I'm going to create four of these and click okay. You see I have four of them and they will match my spider bull body perfectly. So you can see there that they perfectly wrap around this bull, even though this is a sort of a complex curve there, right? It's not a perfect sphere that I have here. All right. And now that's basically it. And then I can further combine these into one body, modify, combine, choose my main body here. And then for my, or choose that as my target body, my tool body, I can left click the first and then shift and then left click the last body that I want them to combine. And operation is joined, click okay. And you'll see here that all these will combine into one body. And there it is. So that's how I approached the spider web here. So hopefully you added a few more tools to your fusion toolbox. The projective surface tool there came in handy there to take that flat plane and get it to project into a complex curved surface. And the other thing is that pipe tool. So if you're trying to do a pipe in the solid workspace, and it's not working, jump into that create form here, your sculpting environment and try it there. You may get better results. All right. If you have any questions on my approach here, leave it in the comments below. And if there's an approach you would take that I didn't cover, leave down in the comments as well. I'm curious to see what path you would take. Also, make sure to check out the resources I have linked below. I've got a great fusion 360 constraints cheat sheet, which is free to download. If you want to get started with Fusion 360, take a look at my online courses and of course my live class that I do every week. I will see you all in a week or two.