 Hey guys, Vladimir here with desktop makes. So last week I looked at approaching this spider bull design, specifically creating the spider pattern here and creating it to follow the contour of the body. So this was the body I took into this sculpting environment to make. So it's not a perfect sphere. There were some challenges on getting this shape here to extrude and follow the pattern or the contour of the spider bull. So we looked at some options there and hit a few roadblocks. And finally what worked for me was going into the sculpting environment and using the pipe tool there. So check out that video if you want to see the workflow I took there. Now in today's video I wanted to address some of the comments that I received from you on that video. There's a couple comments I wanted to look at and one of them was by James Drager here who said, I think you can extrude lines then thicken in the surface environment also extrude from object. At least those are the first things I try. I don't know if they would actually work the way you'd want. So I wanted to look at into that and give that a try. And there was also another comment here by HPE Christensen who said, I believe the problem with the solid pipe is when three lines meet at one point. If you do the rings and radii separate, are you sure the solid pipe will not work? So those were two excellent questions that I thought were worth kind of revisiting. So here I'm going to go to another design here that I've kind of pulled back the timeline to where I just have this the body here and then the sketch that I created on that center plane. So remember this sketch is just on this center plane here that front plane and it's a complete flat sketch. And what I want to do is take this and create a body that follows this contour here. So let's try James's suggestion here of going into the surface environment and try extruding the lines and then thicken them. So let me untangle the body here. So one really important thing I want to point out here that's going to be very valuable to know is that when you're in the surface environment and you hit E for extrude and then you select your object here and then you go ahead and extrude it, it'll basically mimic the same extrude function as in your solid environment. So you're basically extruding a profile right and you're getting this entire shape which is kind of the challenge here because that's not what I want. I want to be able to just extrude lines. So that doesn't work. So and it's different. The point I want to make there is that it's different when you hit E versus going up to your menu and then grabbing your extrude option there. And now if you select it and then you take your arrow and extrude it. Now it actually does let you extrude lines. So be careful there. Don't think just because you're in the surface hitting E on your keyboard and then grabbing it from here is the same thing. You get completely different functions. Kind of like when you're in sketch mode and you hit F for fillet. It throws you back out when you're actually using 3D fillet and it's different from Modify fillet. But anyway, so we have this situation now where it does kind of work. We're getting our lines but it's not grabbing all of them and it's random as to like which ones it picks. And so it almost gets in. It doesn't quite get there. And then I tried something else which kind of made all the difference here and it's just a very subtle thing. So if I do the order differently, if I for example select first, if I drag select and then go to create and then extrude. Now when I extrude this out it'll actually, oops, bring that again. It'll actually work and grabs all my sketch lines. So the difference there is if you go to create extrude, if you do extrude first, event select then it kind of behaves randomly. You see it doesn't grab all of them. But if you select and then extrude it works. So if anyone knows why that is let me know in the comments. Probably I might send this to Fusion. Your Autodesk can see if they can provide some feedback on why it behaves that way. But good to know. So make sure if you're kind of going for this workflow and you hit the same wall that I did, just make sure you got the order right. So okay, now we have to actually extrude the lines. I'm going to bring in the body here and I'm going to change the operation to not start at the profile plane but to start from object and then click on the surface here and it works. So James comment there actually works really well here. Well up to this point. So let's say here I just want like negative two millimeters. I'll set that and now I've got a new body as operation and I've got this extrusion of surface surfaces from that sensor plane and it mimics this contour here of that body. So I get this. So very cool. The next thing, the approach I would take here is to go and thicken this entire, all these bodies here. You can see I've got all these surface bodies. That was a problem for me when I tried doing that. I pretty much got the little spinning wheel of death and I had to restart Fusion. And I think the problem there as well is like all these intersections here. Just the calculation is a lot for it to make and it didn't work. What did end up working is if I separated these so that I had just the outer parts here like the outer rings and then I did those separate from sort of the spokes here. So if I did the thickening two passes it worked. I'm not going to do that right now because it's going to take a while for me to unselect and then do them both each at a time. But basically do the outer rings all three together first and then do these spokes in two different thickened operations and that worked. This workflow will work for you if you kind of go by the right order and do certain things the right way. But I don't really recommend it because it's kind of long and when you're doing the thickening on all these parts it takes a while for Fusion to do those computations. It's sort of a heavy for the machine to handle. So the other approach I wanted to look at here was Christensen's comment. Let me find it here. So I believe the problem with the solid pipe is when three lines meet at one point. If you do the rings and radii separate are you sure the solid pipe will not work? So let's try that. I'm just going to delete actually this last step here my timeline. So I'm back to one body and I've got that sketch in the center. We're going to try that pipe method but first let's go back to solid and I do need to project this sketch onto this surface. If you recall from my last video create sketch on this my front plane right here make sure you select the right plane and I'm going to now go ahead and project this sketch onto the surface here to do that you go to create it's different than just like a regular project. If you go to project include you have an option that says project to surface so I'm going to click on that. I'll first click on curves here and then I'll drag select all my sketch curves and projection type. I'm going to go with a long vector and then I'm going to click on project direction and for that I'm going to select the y axis or that green axis there and then I'm going to go back to my faces and then bring in that body and then select this face that I wanted to project click okay and now you can see it took that flat sketch there and then projected it to match this surface. So great tool there to take advantage of now I'm going to click finish sketch and I'm just going to show that projected sketch that I made and now we're going to try that pipe tool again but we're going to do it in different selections so we'll do the outer ring first and then do these lines. So we're going to go ahead and go to create down to pipe and here you kind of do have to select these individually which is a bit of a pain but no no big deal. If you did have these lines in separate sketches then you can like drag select but I won't be able to do that and you have to do them in three different operations so I'll do the outer bam there click okay and then right click repeat the nice thing is that this is quick you don't have to wait you know for it to calculate and so it seems to be pretty straightforward for fusion to create these calculations and of course you know I have this my section size sent to one millimeters and circular as the section so we'll do that and it's going to create a second body notice for which it's created some creates its own bodies there and then I'm going to do this intersection here and select all of these and now I can click okay I'll have my three bodies there and I'm going to do one more and that's going to be these lines here coming in and I'll just select those oh yeah so for this one it only lets you do it two at a time so we're going to have to do that approach as well change this to new body yeah so it doesn't let you go ahead and select more if I try to click on more it doesn't work and if anyone you know if you have different workflow here you think would make this more efficient or a different path you would take let me know kind of like you know well I enjoy getting the comments and then following some of those paths you know sometimes you get some some really good advice there and some paths that I might not be thinking of ways to follow okay so now we've got all our bodies here that we need so what I'm going to do I can take this now and combine it into one body kind of say I have all this going on here um let's do you know what I'll just do it all in one shot I'll go to modify combine select my last body here and then shift and select everything else besides the pumpkin body and do operation as join and a lot of selections here so you might have to wait a few seconds I'll click okay and hopefully it should work and all this claps into one body which it did so beautiful and I've got my one spider spider web body here and I can take this and now and create a pattern a circular pattern um to create them on all the four sides so I think this is the approach I you know I think I like the best it was more straightforward um although the other you know going into that surface environment and pulling lines it's really good to know because there are you know designs where that workflow is really going to come in handy so you know I still keep that in your back pocket but this one here for this particular approach I think is more straightforward um and the issue there was yeah it was just um when you have a complex shape where like a bunch of lines are coming together in one point it can be hard for fusion to tackle and resolve that so just doing them in different selections when you're creating the pipe tool or when you're using the pipe tool works out well all right that's all I wanted to come in today and show you this approach and kind of address some of those comments so any questions or any other paths you want me to take I'm happy to jump in and kind of follow follow that workflow and see where it leads us thanks for watching if you guys enjoy videos like this consider supporting my channel by becoming a patreon supporter so I've got the links to that below and I've also got some links to my online courses if you want a more structured approach to learning fusion 360 all right I'll be back in a few