Summary

Sheet metal components are common place on performance builds as they offer a relatively cheap and effective means to creating light, strong and stiff components. Luckily, CAD software has a range of tools to make design and manufacturing of sheet metal components easy. In this webinar we'll show how to design parts in CAD using sheet metal modelling.

00:00 Hey team, Conor here from HPA.
00:01 Welcome to another one of our webinars.
00:03 This week, we're gonna revisit a CAD topic and we're gonna be talking about sheet metal modelling.
00:09 So, we're gonna start off by just talking about how it's useful for us on our project cars.
00:14 Then we're gonna have a look at how it's done in our CAD software and then how we'd export some flat patterns to use for laser cutting, water jet cutting or something like that so, we can get the parts made for us or perhaps how we'd set it up so, we can make them in a more manual method as well just by cutting it out of some sheet metal.
00:34 So, to start off with, we're all familiar with sheet metal parts.
00:38 The benefits, main benefits of sheet metal parts tend to be that they're relatively cheap to make if we compare it to something like a machined part or if we're talking about 3D printing out of metal or something like that, generally, a sheet metal part's gonna be cheaper.
00:54 It's a good lightweight way of getting good strength and stiffness.
01:00 So, that's kind of ideal for performance applications.
01:04 We can use them to make brackets, braces, chassis structures, heat shields, the list kind of goes on there.
01:12 So, if we just jump onto my screen here and have a look at Fusion, this is something I'm just kind of working on at the moment for our staff race car, which is our little Honda City.
01:25 We had a little bit of an issue where the chassis wasn't really designed for the big slip tires that we're running on it and started pulling itself apart kind of around where the lower control arms mount to and, so on.
01:40 So, what I'm doing here, we've kind of stitched it all back up into place and I'm just designing some, now, this is the very early stages of this, mind you, but just designing some kind of plates to tie everything together a little bit better and reinforce everything around those points so, we don't end up with that issue again.
02:01 So, chassis strengthening, brackets, braces, so on, all really good uses for sheet metal parts, whether we're working with steel, stainless steel, aluminium or whatever, those are the main ones anyway.
02:16 But yeah, so with that kind of covered, let's just jump into a new design here really quickly and we'll just talk through sheet metal modelling a little bit more, understand the basics and then I'll jump into a little bit of an example which will hopefully illustrate some of the points a little bit better.
02:37 So, here we are in Fusion and it's really the same thing for something like SolidWorks or Onshape or anything like that.
02:46 They're all kind of set up very much the same and we have our toolbar here and our sheet metal modelling toolbar as part of one of those.
02:53 So, the sheet metal modelling toolbar really has tools that reflect that of real life sheet metal work.
03:02 So, we have things to make flanges here, hems and do bends and things like that as well, as well as some other stuff for creating holes and threads and then we have some tools to be able to unfold and create flat patterns as well back here.
03:21 So, those are all really important and it's gonna allow us to make some great sheet metal parts for our project cast.
03:28 Before we get into it again, I just want to kind of cover off the basics of sheet metal modelling.
03:34 So, one of the main things of that is the difference between solid bodies and sheet metal bodies.
03:41 So, to illustrate this, I'm just going to start, just make a basic sketch on the plane here.
03:49 We'll just make a rectangular sketch here, doesn't matter the sizes of anything for now.
03:54 So, we just have this rectangular profile.
03:58 So, typically if I wanted to add some depth to that profile and make a 3D body, I would use the extrude tool, which we actually have in our sheet metal modelling toolbar here or it's more typically found in our solid modelling toolbar as well.
04:12 That just selects that profile for me and let's say I wanna make that three millimetres thick, which is kind of the same as having a little bit of sheet metal, three millimetres thick like that.
04:24 Create a new body, select okay.
04:26 So, under our bodies in the browser now, we have this body and I just want you to make note of what this icon here looks like.
04:34 This represents a solid body for normal solid modelling that we do in our CAD, which is great for creating machined parts, 3D printed parts and, so on, but it's not a sheet metal body.
04:46 Sheet metal body is a little bit different.
04:51 If we wanted to make this part a sheet metal body, there's kind of two separate ways to do that.
04:57 If we happen to have already created an extrude like this, or we get given maybe a step file or something like that to work with that comes in as a solid body and we just wanna convert that to a sheet metal body, as long as it's consistent through its thickness, which this is here, it's the same cross section through the thickness of it, we can convert it to a sheet metal body.
05:20 So, that's the option here that we have.
05:23 We can click this and then select the source and that's just going to detect the thickness, which is three millimetres and set up this sheet metal roll here for steel, or we can set it to stainless aluminium or a paper template as well.
05:40 And I'll explain those a little bit more in just a moment.
05:44 So, we're just gonna hit okay there.
05:48 And then you can see in our browser, now, we have this icon for the body representing that that is a sheet metal body.
05:56 And that allows us to then use flanges and bends and folds on it.
06:02 Whereas before, for example, we jumped in here, tried to add a flange to the side of it.
06:09 We can't, but now that it is converted to a sheet metal body, we can.
06:16 So, that kind of just allows us to use those sheet metal tools, put simply.
06:20 The alternative to this, if we're just starting from scratch and we are designing something that we know is gonna be sheet metal, we generally wanna skip these steps cause it's just over-complicating it.
06:35 And, so I'll delete those.
06:37 And the way we'd do it is we'd use the flange tool here.
06:41 And I'll just show that sketch again cause it's hidden itself.
06:44 And what the flange tool is, is it creates a few different features that we're gonna cover all of them today.
06:51 We have a base flange, an edge flange, or a contour flange in the case of Fusion.
06:56 And we're gonna create a base flange here.
07:00 So, that's exactly kind of what it sounds like.
07:02 We'll select that profile and that's just gonna automatically make our sheet metal part for us.
07:08 We've got a few other options here for the side that it kind of wants to add that thickness to.
07:14 Doesn't really matter in this case what we choose.
07:16 And it's just gonna be a new body.
07:18 And don't worry about any of those other things at the moment for now.
07:23 And hit okay.
07:24 And that automatically just creates it as a sheet metal part.
07:28 So, we're gonna see this in a little bit more detail as we move through today.
07:34 But that's just what we wanna start with essentially there.
07:37 Now, something else to consider is when we're working in our CAD models, usually, it's best practice to represent every different component in the real world that would exist in the real world as a different component in our CAD models.
07:54 So, we can come under the create tab here and we see we have this new component icon.
08:06 And we can select that and we can create a sheet metal component from here.
08:10 And that's gonna set that up as a new component that has the rules and everything all involved in it.
08:17 So, that's kind of the best way to set that up.
08:20 And we can set up the sheet metal rule there for it as well, depending on what material we're gonna use and, so on.
08:27 Some of you who might've worked for Fusion before might know that you can usually come down here and you can right click and create a component from the body if you need to afterwards.
08:38 The issue with Fusion is that you cannot do that with sheet metal bodies.
08:43 So, if you wanna create a component that's gonna be sheet metal, a new component that's gonna be sheet metal, make sure you do it from the start before you start modeling it rather than trying to convert it to a new component at the end.
08:57 Just kind of makes it possible, basically.
09:01 So yeah, with that out of the way, the one last thing I wanna talk about before we get into a bit of a, more of a practical demonstration is the sheet metal rules.
09:11 So, we've seen that a little bit here.
09:13 That's captured in the browser here.
09:16 And we can switch the rule to a different one we create, or we can view our sheet metal rules up here and see that we have a library of different sheet metal rules.
09:29 And we have the one that we're actually using for our part here.
09:33 And for example, if we wanted to edit the thickness of the sheet metal we're using for now, we can come in here, edit the rule, change the thickness, for example, to four millimeters.
09:44 And that will sort all that out for us.
09:46 And it also has some stuff in here for bend conditions and corner conditions that we'll see with our rules as we start creating features as well.
09:56 As well as this K factor here.
09:58 The K factor is a little bit tricky to understand without a image to kind of show you what it means, but it basically controls kind of the material usage for different types of materials through a bend.
10:17 So, for steel and, so on, it's set to 0.44 by default there.
10:23 I think aluminum's kind of the same.
10:26 And then you'll see for a paper template, that's not metal at all.
10:29 The K factor is actually one.
10:31 So, I think there's no material usage in that case through a bend.
10:35 But other bend conditions might just be, for example, setting the minimum bend radius to the material thickness, which is kind of a rule of thumb.
10:43 If we try to bend any sharper than that, you get cracking and distortion of the sheet metal.
10:50 But again, we'll look at that a little bit more as we progress through.
10:54 So, I'm just gonna close this one from here, and then we're gonna jump into a little bit of an example.
11:02 So, what I've got here is a 3D scan of the inside of a vehicle.
11:08 And we're looking at the outside there, but the scan was actually taken from the inside.
11:13 And this was taken with the intention to basically design a roll cage.
11:18 So, what we're gonna look at here is just how we might go about modeling some sheet metal roll cage footings.
11:26 And just keep in mind that this is just an example to illustrate how to use these sheet metal tools.
11:31 It's not an example getting perfectly accurate with kind of the best practices for designing roll cage footings.
11:38 I'm just kind of, you know, off the cuff modeling something here rather than really setting it out to the required specs and, so on.
11:47 But it should give you an idea of how we're gonna do that.
11:51 So, all we're gonna do to start with just to make this a little bit easier is just use a section analysis through the top plane here just to cut off the top of the car.
12:02 I'm just gonna drag that down a bit as well just to make it a little bit easier to see what we're doing as we start working here.
12:09 And I've already set up this plane here, which is really easy because as per best practice, the scan is nicely aligned to the coordinate system.
12:20 So, I've just set up a little offset plane down here that is basically at the top of where I want those roll cage footings to kind of sit and intercept the chassis there.
12:33 So, what we're gonna do now from here is start to model those actual sheet metal parts.
12:39 So, I'll just turn that off, tidy some things up here.
12:44 Cool.
12:45 So, what we're gonna do is we're gonna start and this example is actually also gonna give you a little bit of a look at some tools that we can use to work with 3D scans as well.
12:56 So, a little bit of a bonus there, but the main focus is of course on the sheet metal work.
13:01 But what we're gonna do to start with is create a mesh section sketch.
13:07 And we're gonna select the body being our mesh body for our 3D scan.
13:12 And then our section plane, just being that plane that we talked about just before.
13:19 Okay.
13:21 And then now if we just hide the body, we can see, hide the plane.
13:26 We've got this kind of profile here and that is basically where that plane intersects the scan.
13:35 That's created that profile and it's created these two features in our timeline.
13:40 And this sketch here is what we want to work with here.
13:43 So, I'm just gonna edit that sketch and I'm just gonna do the footing in this back corner here kind of for the main hoop.
13:51 This technique we use quite a lot at HPA for making sheet metal kind of footings for parts to go onto the chassis for roll cage footings or for mounting pedal boxes to the floor pan and, so on, it works really well.
14:05 So, hopefully you guys will see a bit of a use for it too.
14:10 So, what I'm gonna do here is just sketch a couple of lines really quickly.
14:18 Just kind of marking out the rough size that I want.
14:25 And let's just also just for reference, drop a construction circle on there that is 44.5 millimeters in diameter.
14:36 So, we can kind of see the size of our tube where it's gonna land on that.
14:42 That's the kind of one of the standard sizes anyway for roll cage tubing.
14:47 And we'll just say maybe this is 60 mils and this one can be 80.
14:59 We'll just drag things around a little bit so, we're happy with the placement.
15:03 I just kind of want these intersecting the sides here and then I'll just turn off that plane so, it's not doing that all the time.
15:11 What I like to do is lock down the position of everything in my sketches just, so it doesn't go moving by accident.
15:18 So, I'm just gonna use this constraint here and just lock those two in place.
15:22 Usually, I'd make dimensions from the origin or something but in this case, I'm just trying to keep it moving along quickly.
15:28 Now, under the create tab, we have this fit curves to mesh section thing.
15:35 So, I'm just gonna select that and that's kind of the second important stage of this mesh section sketch.
15:41 And then I'm just gonna kind of fit this spline tool here along the side of the chassis.
15:49 We're gonna come right around to, oh, just noticed.
15:54 It's trying to do that as construction line so, we won't let that happen.
15:58 All right, just start again here.
16:00 So, just kind of overlapping there, coming around here.
16:03 I'm not actually sure what happens at this point.
16:08 I'm just gonna turn off the, oh, what's going on? I did, I'll just do that one more time.
16:23 Bear with me while it's loading.
16:25 All right.
16:28 So again, just gonna fit a spline along there.
16:33 Jump over this gap, although I just wanted that to be a bit bigger.
16:39 And for some reason, it's not wanting to.
16:43 What if we go back to one? Okay, that's gonna be what it'll be then and then come along there.
16:49 So, let's just fit the spline along the kind of mesh profile there.
16:53 And I think in this corner, it's just a little straight part that kind of got missed when it was being 3D scanned.
17:01 So, just to close that gap and I'm just gonna make that kind of a straight edge there.
17:06 Might be a little bit better.
17:08 But we've got this sketch profile now shown in the shaded blue color that we can use.
17:15 And again, just to avoid anything kind of moving, I'm just gonna lock all those down and go finish sketch.
17:22 And then now we're going to use this if we turn on the mesh body again.
17:29 I'm just gonna create a sheet metal flange.
17:32 So, we've got the top of our kind of box is gonna sit there and it could sit above or below, it doesn't really matter, or in the center of that, just like that.
17:43 Cool, new body, okay.
17:45 So, now we have that, which fits really nicely into the corner there.
17:50 And from here, we're going to use our next kind of use for the flange tool, which you can see at the top here, it says base, edge and contour under that flange tool there.
18:01 We're gonna create an edge flange this time.
18:04 So, I'm just gonna select the two edges that I wanna create those on, and I'm gonna drag those down.
18:10 And those are gonna be at 90 degrees in this case, although if we wanted to, we could flare those out and change the angle from here.
18:19 And of course we can just change the distance.
18:21 In this case, I just want it coming down through the floor, and then I'm gonna trim it back to where it kind of needs to be.
18:27 A few other things to consider here is you can change where the bend position is based on the edges, outside, adjacent, or inside, or tangent in that case.
18:44 Any of them is kind of fine, it just kind of changes the size of the top surface here.
18:50 And then if we want to miter the corners or not, which we want to in this case, if we can get this edge as close as possible, once it's all folded up, that means it'll be a lot easier to run a bead of weld down the side of it, so, that'll be ideal.
19:06 So, the other thing that we wanna talk about here is the rules.
19:11 So, our sheet metal rules have been by default applied to this, and that kind of helps us design something that can be made, which is designed for manufacturing.
19:21 So, it's applied our DFM considerations here, so, the bend radiuses and the clearance around here is all correct or roughly rule of thumb anyway, to make sure it's all gonna work out.
19:35 What I like to do though is just override these rules, and we can change the bend radius from here or bend relief in this one.
19:44 I'm gonna change the two corner bend relief thing here and make the relief shape round, because I find it just works a little bit better, and then just reduce that down to about 10 mils, make it a little bit smaller.
19:59 So, that's just an idea of what we can do to kind of change how those rules actually affect the part, and I'm just gonna hit OK there.
20:10 Now, I just wanna make a note that there's a bit of a wiring harness or plumbing or something running through this part, and that should really have been removed before we 3D scanned this, and it would be removed and moved out of the way if we were going to build our roll cage footing here.
20:30 So, I'm just gonna kind of ignore it and do my best to work around that for now.
20:35 The next thing I'm going to do is just create some mesh sections again through the mesh body, and then just using those surfaces as the plane to cut through it, and then I'm just gonna come into that sketch or hide that.
20:53 What I'll do is project that surface, so, I get a profile of the surface, then jump back into fit curves to mesh section, and then basically gonna do the same thing here, just kind of come along here to here, and then jump up to this bit and come up here.
21:22 That hasn't worked because we've got a bit of a funny overlap.
21:27 Let me just do that one more time.
21:36 That looks a bit better.
21:40 Okay.
21:43 Finish that sketch, and then now what we can do is just use our extrude tool and just cut out what we don't need from there.
21:56 So, two object and just cut through that thickness there, and then if we view the scan again and just ignore where that height is, where that harness is going through.
22:09 Hey guys, sorry, just had a little bit of technical difficulties there.
22:13 So yeah, we'll just jump straight back into it of where we were.
22:16 So, we just extruded and kind of trimmed everything we don't need there, so, just ignoring again this wiring harness.
22:23 We can now see we've got this edge here and this one here, and that nicely just kind of lines up with the floor pan.
22:33 We're just going to do one more of those on here.
22:36 So, I'll just run through this pretty quickly because you guys have already seen it happen twice now.
22:45 And we're just going to create a profile on the side of this here and fit some curves to that.
23:00 Come from here to here.
23:07 Yeah.
23:09 There, okay.
23:10 Finish that off.
23:16 Any of the extrude tools, they all look the same.
23:20 It's all the same tool essentially, and we're going to go to object here.
23:25 So, we've just trimmed that off now.
23:27 Cool.
23:28 So, now you can see we've got this kind of roll cage footing here as a sheet metal part.
23:32 That's just a bit of a box that we can wedge into the corner there, and it should line up really nicely with all the floor pan and everything.
23:42 From our experience of doing this with a few of our projects, it tends to work really good, and we get pretty minimal gap that we can weld around with the MIG, tie it all in.
23:54 So, from here, what does the kind of process look like? The next step would be to basically create a flat pattern of this so, we can get it cut out for us, or cut it out ourselves, and then obviously be able to fold it up and get it into the car and weld it in place.
24:15 So, the main way of doing this is going to be from under the sheet metal create tab here, we're going to create a flat pattern.
24:26 So, from here, we just need to select a stationary face.
24:31 It doesn't really matter in most cases what that is, but just select the top face.
24:37 So, that's just going to keep that one put, keep that one as it is, lined up with that kind of top plane view, and then it's going to unfold these other ones relative to it.
24:47 So, we'll go okay there, and we can see it's just done that.
24:51 So, it's flattened it all up.
24:53 That's our top, front, and our kind of side there, and we can see the bend lines on here as well, and also the extents, the bend extents.
25:03 Those are kind of shown on the body here.
25:05 So, the bend extents lines are basically just what material is actually, surface is actually part of the bend radius, I guess you'd say.
25:18 So, under this flat pattern stuff in here, there are other tools that you can use to kind of modify it even more, and that's only going to be captured in the flat pattern.
25:28 Most cases, you don't really need to do this.
25:32 So, from here, generally, I'm just going to export this flat pattern as a DXF file.
25:38 So, that's just basically going to give the outline, and it might also include the bend lines in it as well.
25:47 And then I can send that DXF file straight to a laser cutter or waterjet cutter, or even a plasma cutter to get this really accurately kind of cut out of whatever thickness and whatever material I tell them to do.
26:02 So, three millimeter steel in this case would usually be the kind of typical route from here.
26:08 If you're working in the free version of Fusion, then I don't think this export, the flat pattern as DXF option is available.
26:17 So, a little workaround for this that I hope still works for you guys is to create a sketch on the flat pattern there, and then just project.
26:30 So, I hit P on the keyboard there, but that's just found from under here.
26:35 So, project the whole surface.
26:38 And what that's going to do if we hide the body now is just kind of give us a sketch that is the outline of the part.
26:48 And then in the free version, you can right-click that sketch.
26:52 You used to be able to anyway, I haven't checked lately, and go export the DXF from there.
26:58 So, that's a little workaround if you can't export the DXF from the flat pattern itself.
27:06 Cool.
27:10 So, that kind of gives us an option if we want to get it laser cut, but of course it's completely acceptable that you might want to just cut this out of a flat sheet, bit of sheet metal yourself with an angle grinder or something.
27:27 You'd be able to do an accurate enough job and do it yourself.
27:32 So, the option from here is essentially to go finish flat pattern.
27:38 And then what I would do is jump up here and go, well, a few options, but new, I think, drawing, create new.
27:56 And then rather than folded model, go flat pattern and just make sure maybe it's a A4 sheet.
28:04 I think it should fit on there of a normal printer like the one behind me there.
28:10 Portrait or landscape, not going to matter and just go, okay.
28:17 Hopefully, this doesn't take too long to load here.
28:22 And then we can just drop our flat pattern onto here.
28:29 But we want to make sure the scale is going to be one-to-one.
28:33 And then something else that's usually worth checking, if we can, it might not be kind of ideal for this one, I'm just going to also just delete the kind of title block there.
28:47 So, it's not in the way.
28:49 What I usually do if I'm going to print something out of a printer is just add a dimension on it.
28:57 Something that we can kind of measure across to check maybe in two different directions just to ensure that the scale is right.
29:06 So, basically I'll print this out.
29:08 I can just export it from here, or I think I can just go straight up here and go print.
29:14 Print that out on the printer, make sure it doesn't scale or do anything weird.
29:18 And then I can just double check those dimensions with a ruler or with my veneers or something like that to ensure it's correct.
29:25 Cut out the outline, stick it on a, with some spray tack or something, stick it on a piece of sheet metal.
29:31 And then we have an outline that we can cut around with an angle grinder, fold it up and we'll be able to get the part there.
29:38 It's usually a bit of a quicker and more accurate way that fits a bit nicer than just doing that all by hand.
29:45 You're going kind of back and forth between the car and our angle grinder or whatever we're working with.
29:52 So, that covers most of the sheet metal rule, sheet metal tools.
29:58 I am going to show you a couple more, but if you have any questions about any of the stuff that's come up, feel free to ask it in the chat and I'll do my best to answer at the end.
30:08 So, I'm just going to hide that for now.
30:12 Okay.
30:14 So, just a couple of other tools that I just wanted to show you.
30:19 I'll just create a new design here.
30:21 Like I was mentioning throughout with the flange tool, there's base, edge or contour.
30:28 So, I'm just going to show you what the contour flange kind of looks like from here.
30:32 So, if I create a sketch and it's going to be an open sketch, so, it's not going to kind of form a loop, it's just going to say, come up and do something like that.
30:47 Then what I can do is use the flange tool there and that's going to automatically create a contour flange and I can just drag that along.
30:57 And what this is doing now, depending on the side that we choose, but it's essentially adding in bends automatically where those kind of sharp corners are with all our bend rules set up and everything and just allowing us to add depth to that profile with a contour flange.
31:16 So, that can be a real kind of powerful tool depending on the type of modeling that we're doing as well.
31:22 And same thing, we can just kind of add our sheet metal rules, whatever we're trying to work with there and maybe change the bend radius to 10 millimeters or something from there as well.
31:35 I'll come back to that note of bend radius and thing in just a moment.
31:39 The other one that I want to mention, if I just delete those, create another sketch on the top plane, for example, and then just sketch kind of a rectangle and make a base, actually, yeah, I'll sketch a rectangle just with a kind of line through it.
32:08 Doesn't really matter where it is.
32:10 And then I'm just going to create a base flange with that again.
32:16 Then from here, we can use the bend tool.
32:19 So, the difference between the flange tool and the bend tool is the flange tool creates the new material or the new face while also adding in a bend, whereas the bend tool kind of needs existing geometry or existing body or material, and then it can add a bend to it based on a line from a sketch or something like that.
32:44 So, that's exactly what we're going to see here.
32:45 Select the bend tool, do it on the bottom side here because that's where our sketch line is.
32:53 Select the surface and then just select the bend line here.
32:58 You can kind of flip it from there, change the angle of the bend and, so on, and then you've got your override rules and, so on, the bend position and everything from there as well.
33:11 So, you can kind of see how that just is maybe a little bit more simple version of the flange tool, but you already need to have the geometry set up there to be able to do that.
33:24 A little bit more of an example of that would maybe be in this part here.
33:29 So, if I just come back a little bit, rewind this a few more steps, we can see that I kind of had to model with this part out here and then come through and add those bends into the part to get it to kind of line up with the chassis from there.
33:49 So, it's just a little bit of a different approach to using a flange tool where with the flange, I would have left the side straight and then added the flange and the bend at the same time.
34:00 Either can work, some are just better suited to different situations.
34:06 The other thing that I just want to talk about is our bend rules help us automatically kind of consider the, or account for the DFM considerations.
34:18 So, we make parts that we'll be able to make accurately and without cracking in the bend radius and, so on, but it doesn't really account for everything.
34:30 We actually need to consider the materials that we're working with and the tools that we have available.
34:36 So, some common examples of this is just ensuring that we're working with a material thickness inside the limits for whatever cutting tools that we're working with, whether that's a laser cutter or, so on, how thick material we can actually cut.
34:54 And then also, if we're talking about how thick material we can bend, if we're just doing this in a vice or something like that, then working with something that's five millimeters thick or something, you might not be able to bend it with the tools that you have, even though you've designed it to kind of work like that, it might need a press or something to bend it.
35:15 And then also, we've talked about the bend radius throughout this and generally rule of thumb is that it really depends on the material, but we try not to make the bend radius any less than the thickness of the sheet metal.
35:32 So, if we have three millimeter thick stainless, when we bend it, we want the radius on the inside of that to be three millimeters.
35:43 If we go less than three millimeters, then we risk kind of cracking or deforming the material through that bend.
35:51 But, you know, we could go bigger and that might not be a problem as long as we've factored that into our design, but actually controlling the bend radius is a whole nother thing.
36:01 So, the tooling that we're using needs to be able to control that bend radius.
36:05 And if we're just bending it around a sharp edge on a table or something, then we're not gonna be able to do that.
36:09 It's probably not going to be that accurate and we might be a few millimeters off on our CAD model by the time we've done a few bends and, so on.
36:19 So, just things to consider really, to make sure we're kind of making something that's gonna work really well for us in the end.
36:27 One last thing that I wanted to show is quite a cool tool that Fusion has.
36:36 So, I'm just gonna delete that and really quickly just set up a offset plane, 60 mils or, so up here, sketch on that.
36:52 And I'll just show that bottom sketch as well and just set up a kind of circle here.
36:57 So, what we have is a rectangle sketch and then on another plane, a little distance away from that, we have the circular sketch.
37:06 And what we can do with those is if we use the lofted flange tool, we can create a loft between them with a sheet metal part.
37:16 So, this is really like a cheap way of creating like sheet metal ducting for plumbing or airflow or something like that.
37:27 And we can control kind of how that's set up.
37:31 So, there's a few options here.
37:34 The forming type, so in a break form, that's just gonna be using a press break or something where we just have straight edges that we're working to, or we can create a die if we actually have, maybe we've 3D printed a really solid plastic die that we can form some sheet metal around so, that can work really well there.
37:57 Or we just have this option where we'll be lining up with some bend lines and kind of bend each of them in and end up with this shape.
38:05 The only thing about this is when we finish up, what we have is kind of a solid sheet metal part and we can't just come in and flatten this out.
38:19 Yeah, it won't do it for us.
38:22 So, a kind of workaround for this that they've added in, and this is kind of in a lot of CAD software, is to add this rip tool.
38:33 I'm just gonna do a really quick job here of just creating a rip down the edge of that.
38:38 That is, say, 0.5 millimeters or something that's gonna be even smaller.
38:43 You could have 0.01, just, so you can weld that up as it kind of comes around or something.
38:49 Now, this part, we should be able to come back in and create a flat pattern on this, say here and like that.
38:59 We'd be able to then get that laser cut, mark our bend lines on it and come around and add all those bends in.
39:06 I would imagine it would be quite tricky to actually do that without kind of trying to make those last bends and without the part actually contacting whatever we're trying to bend with it.
39:17 But again, those are the considerations that we work with around design for manufacturing and, so on.
39:25 All right, so that, I think, kind of covers up everything I wanna look with.
39:31 So, I'll jump into the questions and see what we've got here.
39:36 All right, MrBoss1308, what scanner and processor did we use for the chassis scan? I'm not 100% sure because I didn't do this scan myself, but what I think was used for it was our PL3 3D scanner and then we used PLCAD.
39:58 It's not being scanned on high resolution or with a whole lot of care, but it's perfectly acceptable and really useful for exactly the intended purpose.
40:10 So, it's pretty good, to be honest, it's really good.
40:17 And then using the PLCAD to actually kind of process it and everything is what really allows it to be aligned with the coordinate system really well.
40:28 And in some other cases, you can use a lot of other tools to set up planes and, so on on it.
40:34 But yeah, I think that was with the PL scanner.
40:38 If it wasn't the PL3, it would have been with one of the IonStars, probably the Vega or the original IonStar, but I'm pretty sure this was done with the PL just by how well aligned to the coordinate system I think it would have used the PLCAD processing software to do that.
40:59 Cool, that's the only question we have.
41:02 So, I hope that kind of gives you guys some insight into sheet metal modeling and some considerations around it, as well as at the same time, maybe giving you some ideas of working with 3D scans and making some parts that fit really nicely with the chassis using that mesh section sketch and kind of intersecting the mesh body there as well.
41:23 It works really well.
41:25 So, we'll leave it there and we'll be back next week with another webinar.
41:29 So, thanks for watching.