Fusion 360 - Unfolding Sheet Metal Tubing

[Music] hi guys Kevin from mechanical advantage comm in a previous video I took a piece of tubing and I put some tube notches in there that were meant to be cut on a like 4th axis laser or water jet or plasma table I get a lot of questions about what if you don't have one of those and you want to do sort of the same thing but you want to use a paper template to do that and why don't you know if that's possible or not I'll put a link to that video a card to that video so you guys can go back and review that if you've never seen it so there is a way to do this the bad news is there's not a way to easily do this and I haven't found a way that you can do it using the pipe command but I wanted to kind of show you how we could do this with sheet metal tools and then create the flat pattern and I also want to at the end show you tools that Autodesk already owns it has implemented an inventor the things that would make using the tube command to do this a cinch to do and we'll put a link so that you guys can go out to the idea station for fusion 360 and vote for ordered us to add some more sheet metal functionality into the product so with that said let's get going and how we could draw a piece of sheet metal tubing that could be unfolded so that we could create a paper template to cut with either a plasma cutter by hand or even you know even just using a grinder or something to do it so I'm gonna start out by sketching I so I should switch to the sheet metal environment it doesn't really matter for the sketch part but we're gonna go to the sketch menu and I'm a sketch in arc and I'm gonna choose to do a center point arc and I'm gonna choose my front plain this is my Center now when you start have to try to figure out is where you want this seam to be when your design is done you'll see what I mean when we get done with this but I'm gonna kind of pick a point something to click here I'm gonna rotate around and I want to come back almost so that it's sort of touching but I don't want it to touch so that's close enough for what I what it is that I want to do I'm gonna add some dimensions to this and then we're gonna add some construction geometry to finish it out so I'm gonna start the dimension command I'm gonna click on this arc and because it's not a full circle Fusion is going to give me a radius I want this to be a diameter so pretty easily I'm gonna be able to right-click and choose the diameter option instead I'm just gonna place that and I'm saying with this diameter be 2 inches so it's gonna be a piece of tubing that's gonna be about 2 inches in diameter now I want to sort of control where this gap is gonna be and the way that I could do that is I could turn on my construction and I could draw a line from the point to the origin and then back to this point and I want to draw one more point from the center or to make that go straight down this is gonna be using my symmetric reference in the next step so I'm gonna add a symmetry constraint between this line and this line and want to make it symmetrical to this vertical construction line okay so now that I've got those in there the next thing that I'm going to do is add a sketch dimension between these two we're gonna call this an angle dimension now for paper you can go pretty thin on this I'm just gonna do like five degrees so you guys can see what's going on here so there's a five degree rip in this piece of paper or in this tube that we're gonna end up with I should say so we'll stop the sketch and now we're ready to do let's go to an isometric view here for a second is we're ready to go and create a flange out of this this isn't called a contour flange I'm gonna go ahead and click on that I dragged this the direction I want to go and tell how long I'd want it to be so maybe I'll say I want this piece to be 5 inches the other important thing that I want to look at is do I want the tubing to go on the outside or on the inside now I want my maximum while the diameter to be 2 inches so you can see it's going on the outside of my sketch so I'm gonna flip it to be the side to snow it's going on the inside and with that we can choose a rule there's my steel inch rule that I've grabbed and we're ready to move on to the next step so I'm gonna go ahead and click OK and now I want to cut the tubing notch on here so I'm going to use a plane at an angle and the I want to use this edge this x-axis edge is my angle and I'm gonna rotate this about oh let's go a negative 20 degrees and click okay so now that I've got that I can go ahead and I can sketch a circle Center diameter circle this is gonna represent my knotch don't trust when you see this origin right there thinking that that's where the origin point really is my origins actually somewhere more to the left and probably down so what I'm gonna do before I draw that circle is I'm gonna do p4 project or you can find that from the sketch menu and go to the origin and I'm gonna find the zero point and click on it and click OK now there you can see that that's the real origin this is the kind of assumed origin of the sketch but that's where the real origin of the part is that so we'll go a circle center diameter circle I'm gonna click that point and drag it out and for the diameter of this I want this to be 2 inches and I'm gonna stop the sketch now I need you to extrude this but I can't just extrude this right now or it's gonna be a solid extrusion that's gonna cut everything so I'm gonna switch to the patch environment for a minute and we're gonna do an extrude here grab this area let's say we want to do asymmetrical extrude and I'll just pull this so it's through everything so now that I've got that done I don't really need to see it anymore I can just go to my bodies folder or my construction folder I guess no bodies and we'll turn that we'll turn that body off that we just created all right so I can I can stay in the patch surface I'd be flying but what I want to do is I want to modify and I want to choose the split the face grab this place and then the splitting tool is going to be that body that I just created go ahead and hit OK now I can right click and choose press pull grab that area and I want to I want to extrude it the thickness or press pull the thickness of my sheet metal part and I know that's negative point one or point one is what the thickness is but I want to go negative point one on that and hit OK and there's part of our split I'll do one more split so we'll say modify split face this time we'll do the outer face grab that same splitting tool click OK and there you can see that we have just that a little bit right there that might need to come off now if you're doing this with for a paper template and you might not even have to go with this step you could probably stop right here and trace your template on there and use the grinder you can be probably as close as you need to get so I'll say - point one again I mean click OK and now we have we have our two knotch coped so we're ready to because we did this with sheet metal tools we're ready to fold this right away so I'm just going to back to the sheet metal and I'm going to use the outside of my stationery face so I'm just gonna choose modify and creat flat pattern fusion wants to know what's my stationery face I'm gonna select that and hit OK and there you see that we get what that cut would look like now I want to caution you a couple things that you need to change about your sheet metal rolls that are gonna be important for this method if I were to go and measure that edge right there my total length is six point one nine five nine - so I'm gonna close that and I'm gonna activate the flop pattern and we're gonna check that same edge again if I measure that edge again you can see it's significantly shorter than what it was in the folded state and that's because fusion is applying a K factor which is how much the material is going to stretch as it's formed into the piece that needs to be in our example we don't need this to be formed at all so instead of having a K factor of whatever the default here is point four four we want to choose a K factor of one so what I've already done is I've already created a rule I'm just gonna go edit it and I have the exact same rule I copied it from it the only thing that changed is I changed the K factor to be one on this part so it's gonna not deform the material at all hit OK and now you can see that my rules updated my flat patterns on a date I can just update the flat pattern and now let's go and activate that so if I inspect this and click on this edge now you see that we get the same six point one nine five nine two that we had when it was folded up I'll exit it let's check this out one more time so inspect click on that edge and there you can see we get the same dimension right there so that K factor one's gonna be sort of critical if you want to get an accurate paper ten Glynn now if you want to print this out you could either export this out to a DXF file if you have access to a program that does DXF s-- or else you're gonna have to create a flat pattern drawing of of this model in the flatten state and you're gonna put it on your sheet in a one to one scale and then when you print your sheet out you'll just have to cut needle cut that little end of the tube out and wrap it around your tube and then go ahead and cut it so I hope that helped stay tuned for a minute if you want we're gonna look at some of the tools that inventor has that make doing this job much easier than what it is in fusion with less thought and less planning ahead ok Here I am an Autodesk Inventor 2019 and let's see how we can draw that same to cope tube and the more robust functional tools that inventor has available for creating the flat pattern of that I'm in an inventor part file and I'm gonna start out by creating a 2d sketch on the front face and I'm gonna start by sketching a couple of circles so I'll draw a circle from the center point out and when I draw another circle that way as well I'm gonna add some dimensions so the outer diameter circle is going to be 2 inches and then between these two circles it's going to be point 1 inches just like we were doing in fusion so I'll stop that sketch zoom out a little bit and I'm ready to extrude this let me start the extrude command click my profile say I want to go the other way and we're gonna extrude 5 inches I need to create a work plane and you'll see in Inventor we have different plane options just like we do in fusion however an inventor if I know how to use the plane command I don't have to choose the specific plane options as long as I know what inventor wants for the inputs it'll create the proper plane that I want so I want to go through in my origin folder and I want to use this plane right here as my guide plane and I want to make it around this edge and I'm gonna do the same negative 20 that I did inside of fusion go ahead and lock that in then I'm gonna create a sketch on the bottom side of this plane illness inventor automatically has an option to project in the origin point so I have to go and project that on my own I'm gonna go lock a circle in on that point and drag this out to be two inches and then I'm going to finish the sketch I don't need to see the plane anymore so I'm going to right-click on in the browser and say visibility and now I can extrude that so I'm gonna start the extrude command infusion Ottoman or inventor automatically found that close profile I don't want it to be a solid I want it to be a surface I'm going to choose that option and then I have other options I can choose like symmetric I could change the length but in this case that's good enough as long as it goes to the part that's all I need I'll right-click on that again and say I want to turn the visibility off so we'll right click on the surface say visibility and now that surface has disappeared we're ready to do some face splitting the same basic concept little different tool names inside of inventor compared to fusion but I'm gonna choose this the split command first thing wants to know is what's the split tool it's gonna be that surface extrusion that I just created and then what are my face is so we'll start out by the inside face and I'll hit OK and now I can go and use the thicken offset command here I need to toggle back and forth between those two for some reason I'm gonna go ahead and click on that face say I want to do a cut and I want to go the other direction with it so we'll click on that option and now when I hit OK you can see I have my my first notch on this tube and then I'm gonna split again using the same extrusion this time we're gonna split the outside face hit ok now we can do the thicken offset grab that little region right there it's going the wrong direction so we'll just flip it in and say we don't want to be a cut and hit OK now we've basically duplicated the example that I had in fusion 360 here's where inventor has some more robust tools that'll help us with the next steps I'm gonna put one more sketch on this part just to help us out so I'm gonna put a 2d sketch on this back face I want these two lines just to be construction so I'll toggle them to construction and I'm gonna place a point somewhere on here now I don't want to put it exactly at that point I'm gonna drag off a little bit so that I can use the vertical horizontal constraint or the vertical constraint in the Venter between those two points and now I have that point locked in now what I'm ready to do is take this part file and convert it to a sheet metal file so I'm going to choose convert sheet metal and in veteran wants me to say what it is what what's the face that I want to make my flat pattern of so I'm just gonna click on the outside face and then what is my sheet metal rule that I want to start out with so I'm just gonna choose default here and the thickness is set to point 1 now I do want to make one small change here I want to edit the sheet metal rule and I'm going to go to the K factor value again and change that to b1 and I'm running at a really weird resolution so there it is so we'll say save and close and apply and cancel that and now I'm ready to do some things to turn this into a sheet metal part to be able to unfold this there has to be a tear or rip going through here so that there's a gap there's a seam so you'll notice that in Inventor we have something called the rip command I'm gonna select rip wants to know what face do I want to rub I don't say I want to rip that face where's my rip point let's use that sketch point that we created now inventor automatically adds a gap between those two faces based on the sheet metal rule I can go ahead and hit OK and now I can simply go and say that I'd like to go and make a flat pattern and then better unfolds my part and there's my flat pattern and then I can make a drawing of or say of DX of DX F of or whatever I want to do so inventor has some more robust sheet metal tools that allow us to do things like sheet metal rip ripping at a minimum or converting a normal part into a sheet metal part so that I can rip it and do some other things with it oh one last part of this video I'm gonna show you where you can go and maybe we can get Auto dust to implement these features with your help and your voice all right so you might be thinking right now great I know how to do this in Autodesk an however I don't have Autodesk Inventor so why did he just show me that the reason I showed you that was I wanted to show you that auto dust knows how these sheet metal tools should work and you you have a voice and how fusion 360 can be developed so everybody can go out to this website called forums Autodesk comm and login you all have a login with your fusion 360 account that will get you in here and if we come through and look at all the products that are just Cavs you're gonna see one called fusion 360 I can go ahead and click on that and then there's gonna be different forms underneath here which are excellent for getting help should you need it but the one that I want to concentrate on is the fusion 360 idea station this is where you can go to submit ideas and other users will can come along and vote on them and as you as ideas get more votes they're more likely get implemented by the developers so what I did is I went out if you filter by the latest ideas I went out and I created a fusion 360 idea already so you go find this idea and I'll put a link or a card in the video here and it's called improved sheet metal tools so while you're logged in with your account all you need to do is go ahead and click on the vote button I'll click on this so we can see what what I wrote inside of here but I just I asked for more robust sheet metal tools to be implemented inside of fusion the ability to convert a part to a sheet metal part a rip tool a corner seem to let cetera you can read the rest of on your own but if we can get some votes on these two three four hundred votes it's very likely that Autodesk will take this more seriously and potentially add these tools in the product that we need so that you all can do things like take coke tubing rip them and create paper templates that are very easy to create instead of sort of the workaround method that I had to show you how to do so I hope you guys found this video useful if you have any questions please leave them below if you like this video give it a like if you didn't like it give her this like and if you found this helpful it'd be great for you could subscribe thanks for watching

Channel: Mechanical Advantage

Views: 50,899

Keywords: fusion 360, fusion, sheet metal, Inventor, Autodesk Inventor, paper template, tube notching, tube coping, coping, unfold, autodesk

Id: mu8rpwqjCcM

Length: 17min 37sec (1057 seconds)

Published: Tue Jan 01 2019