Sheet Metal Modeling In Fusion 360

hello i'm steve olson I'm the manager of training services for Mesa in this video I like to share a tutorial on how to model up a component using fusion 360s sheet metal modeling tools before I dive into fusion and start modeling I like to just show you what part we're going to create here in fusion so it's just basically a simple little bracket it's basically 65 by 65 with some flanges and a couple holes and a slot in the top so I just want to kind of give you an idea of where I'm headed so you can see how all these features fit together to generate this part before I dive into modeling I want to share a couple concepts that I've learned fairly quickly when I was trying to use the sheet metal functions in fusion 360 first off it's his own workspace so we'll change over the sheet metal workspace secondly I'm very familiar to inventors sheet metal modeling workflow where we have faces flanges and contour flange features that we use to create our part here in fusion everything's going to be a flange again if you're familiar with face flange and contour flange this one command will be able to create all those types of features and you'll see how we can use this command to create those types of features as we build the part that we're going to make and then lastly here under modify you'll see that we have sheet metal rules inventor has the same type of concept where we create a rule and it says what material and what material thickness we're going to use as we create our part here so under the library you can see I have a sheet metal millimeter defaults you can see it's got a thickness of two millimeters which happens to be the way or the type of file that we have here if I need to make any kind of edits I can hit the little pencil here and say edit rule it will open up a dialog box and if yours is set to something else feel free to set it to two millimeters because that's what we're going to use I think out of the box I think mine was set to two and a half so you might have to change yours I'm just going to cancel this I'm gonna close this one more setting I need to change before I start modeling and that is underneath my document settings I want to make sure I'm set two millimeters as well because I usually have mine set to inches and the file I'm going to be working with here is in millimeters I don't want to have to convert the units as I work on it so I'm gonna go ahead say okay here and now we're ready to begin modeling just like standard modeling I'm gonna begin modeling with a sketch so I'm gonna go up here to create sketch I'm gonna pick what happens to be my X Z plane as the plane I want to sketch on my go up here to sketch and I want to create a center rectangle and I'm going to start on my origin come out you can see it's waiting for values from looking at my drawing the main little top section that I'm gonna try to create here is 30 by 60 so I'm gonna go ahead and use 30 and 60 so there's my profile I want to stop my sketch I'm gonna go up here to create and flange I'm gonna click on my profile you'll see that it adds that profile to this dialog box it's asking okay how do I want to add the material thickness to side one I actually wanted to add it downward so good aside to you can see it's using my sheetmetal default rule which is two millimeters thick it's gonna create a new body everything looks good there so I'm gonna go ahead and say okay so now I'm gonna add the two flanges that can I come down the sides so here I'm gonna go to create I'm gonna flange notice I don't have any sketch whatsoever I'm just gonna hit the lower edge here because I want the flange to come down and I'll flip over the other side click over here you might be thinking why is it not showing anything right now the height is set to zero I can click and drag you can see it's gonna add some sort of height or material there I know how far I want to go so I can just even key that in here I don't have to drag I'll go into this dialog box and say when I go 65 you might be thinking well how does it know how to measure what 65 is is that the inside height the outside height you can see here I can say outer faces interfaces if I go to interfaces you see it adds a little bit of length to that I do want the outer faces in this case because that's the the 65 is the outer dimension that I have and everything looks pretty good there now one thing is also real quickly the bend position so you can see I have inside I have outside I have adjacent so realistically here I went inside meaning where this would have been the 30 width that we had was where this edge would come out intersect with this one I'll say okay and just to prove that concept real quick if we did a quick inspection I should say this face to this face is 30 like we like we asked it to be and then this face to this face to restart this may restart my selection none of this face it's 65 like we asked it to be real quickly before I start the next feature I just want to point out what I'm going to be working on is I'm going to work on these two flanges here and this is a little bit of a different type of feature a little bit maybe a little bit more complex because you'll see here that it's five millimeters from this end of this flange to where this bracket is or to that face the overall width is 65 I only did 60 across the top because of this value here when we create this flange by default it's gonna try to run the whole width here I'm gonna have to make sure I keep this 10 millimeter by keeping a specific offset and you'll see that when I create the feature I'm going to create this feature by sketching a very specific profile here so I'm gonna kind of orbit around at the bottom and create a sketch basically down here at this bottom feature now I need to know where to connect into so I'm going to use my project include project to project this edge into my sketch which will give me basically just a point so now I'm gonna sketch a single line that comes up and then over so we know that we need to have the outside dimension here b5 so when I go to do my dimension here from this point to this point it's gonna be five millimeters and in our drawing we have from this face to the end of the flange being 18 millimeters so that looks pretty good I only need to sketch this once the software is going to be able to identify how to attach it to this edge into this edge over here so that's really all I need I don't need a closed profile this open profile is gonna work just fine for this flames I'm going to make here in just a second so I'm gonna stop my sketch so now I'm gonna go up to the flange command I'll basically pick this profile and I'll have to tell which edges to attach to so I'll pick this edge here now I hit the plus tell it to add to this edge here now everything is working out well except for the fact that the flange is too long I need to make sure that it stops ten millimeters from this face so right now it's on full edge over here if I change this full edge down to two offset that lets me define how far from each end of that edge that that flange goes now in our case that's not quite exactly how we want this to be what I need to do is I need to change this second reference to this face and then specify a ten millimeter offset so I'm going to clear the selection for reference number two I'll select this face you can see now it's brought it all the way out to the two being in line with that now change the value to negative ten you'll see I'll push it back that distance so I'll do the same thing with the second edge I'll say two to offset clear the second reference select this face use negative ten and now we have what we need now that I've got the basic shape of my bracket I just need to go back and add the features like the holes there's a couple of chamfers here and then there's a slot at the top so let's go ahead and add those sonner Neath modify here is the chamfer and and basically I'll hit this edge here and this edge here we need equal distances and from the drawing I can tell it's 45 millimeters and it's a pretty simple feature right there now we have a hole that runs through this component so we'll go ahead and tell it to create a hole it resides on this face the first reference is 40 millimeters from this edge second reference is 40 millimeters from this edge and the hole is supposed to be 20 millimeters in diameter and I want the distance specifying the distance being a certain value I'm just gonna say through all that way if we ever changed the geometry of how wide this is we won't have an issue with this hole maybe not cutting the whole way through everything anymore say okay and there we go I haven't saved this yet so I'm gonna go ahead and save it let us call it sheet metal example I think I've already saved once I'm going to call it sheet metal example 2 now I don't create the holes in these brackets here so I'm gonna go ahead and create a sketch on this face and actually I can create them on this side and this mirror them over this it's probably easier thing to do I'm just lay out a couple points that will mark the Centers where those holes should go and the dimensions that they give us in these in this case is from this edge that face into the hole should be 10 millimeters and I'm gonna use a vertical alignment to align these two holes so I use the horizontal vertical pick those two points and it vertically aligns them then dimensionally from the bottom I have 12 and 1/2 and then Center to Center should be 30 so I'm going to finish this sketch and I can create six millimeter holes big sausage center points i'ma go to hole pick these two centers then the 20 there is way too big I want them to be six millimeters in diameter I'll set my distance to all there we go and now I'll just mirror those to their side so underneath needs to create is Mir I'll just basically tell it I want to use features I find that easier I'll pick the last feature in my timeline which is the holes my mirror plane I'll use one of my origin planes that's one of the benefits of keeping your components centered around the origin that looks pretty good say okay and there are those holes one last feature to create and that's the slot on the top here so we'll create a sketch this could be no different than anything else we've done is just create a sketch and then create an extrusion so we need a slot base off the dimensions we have probably the center to center slot would be best so I'm gonna and just sketch it not even quite even centered just gonna off centered here shouldn't be fun it'd be a big deal to get it centered I can use a coincident constraint that takes the center line and makes a coincident with the origin of my sketch which happens to be over the center of the part now dimensionally I have a dimension that from the end to this center point should be twenty Center to Center is 25 and then there is a four millimeter radius on the slot so now I'm fully constrained fully sketched now just come back here I'll just do the normal extrude grab that profile tell it I'm going to cut I need to flip it over and go the other direction so I'll say direction - just grab the arrowhead pull down tell it distance all and cut we're in good shape so there's a component let's go ahead and save it one last time here one of the benefits of using the sheet metal functionality is that we can then generate the flat pattern that flat pattern is very important to generate the CNC programming whether that's being a laser cut or a monitory press to create this shape out of the raw material so underneath modify I can say create flat pattern I'll tell what face I want to remain stationary I'll pick this one right here I'll say okay and it will then flatten the rest of the component around it you can see here at the top I can then export the flat pattern as a DXF which is very common depending upon what tooling program you're sending it to there are ways to modify it but those modifications won't show up in your folded component there's those changes don't flow back upstream to the folded component because here I can create some additional features if I need to clean up my my flat pattern because of the way some of the corner reliefs worked or whatever you can't adjust and modify those here to go back to the folder model I just hit exit flat takes me back to the folded model and then it does show up here in my browser and I can activate that whenever I need to share one last thought on this component and that is fusion 360 does have its own cam environment so how would you work with the flat pattern of this component in the Kaman environment so I want to show you that real quick so note that I do have a flat pattern of this file we've just created it so I want to make sure that that's you're aware of that because this is going to be critical when we get in the cam environment so I go to the cam environment you can see here underneath my cam component one you can see I have the formed model and the flat model so that's kind of how you make sure that you're using the the flat pattern is you come into the cabin environment and you make sure that's what's selected or active when you're working with the cam I want to thank you for watching this video if you have any questions or comments please feel free to email one of the email addresses on the screen and again thank you for watching

Channel: itsaCADworld

Views: 26,713

Rating: 4.9526067 out of 5

Keywords: Fusion 360, Sheet Metal, 3D Modeling, Autodesk, Tutorial

Id: OcC_qm6UpI8

Length: 16min 53sec (1013 seconds)

Published: Wed Oct 10 2018