Sale ends todayGet 30% off any course (excluding packages)

Ends in --- --- ---

3D Modeling & CAD for Motorsport: Flanges

Watch This Course

$199 USD

Or 8 easy payments of only $24.88 Instant access. Easy checkout. No fees. Learn more
Course Access for Life
60 day money back guarantee



00:00 - In this module, we're going to be taking a good look at flanges and the range of ways we can utilise the flange tool.
00:06 Firstly, it can be used to create a base face, which is very similar to using the extrude process from solid modelling to do the same thing.
00:14 But it can actually be simpler because we don't have to convert the solid body into a sheet metal body.
00:21 Next of course, the flange tool is most commonly used to create a flange feature which consists of a face and a bend.
00:29 The bend is connected to an existing face along a straight edge, essentially adding a new section to the sheet metal part with a bend connecting to the original body.
00:39 We can also create what's called a contour flange which can follow an irregular profile rather than a straight edge like a regular flange.
00:48 This can be formed from a series of connected edges around an existing flat section of sheet metal.
00:53 Alternatively we could also make a contour from an open sketch profile that consists of a series of straight lines and curves.
01:01 Lastly, lofted flanges are a recent introduction to Fusion 360 and allow us to create sheet metal variations of the lofts that we covered in an earlier module in the course.
01:12 If you need a refresher on these, make sure you have another look at the lofts module in the solid modelling section.
01:18 But the general idea is that they allow us to merge one profile into another, creating a transitional structure between them.
01:25 Sheet metal lofts can be ideal for creating ducts and channeling air or fluid in different areas of the vehicle, like an air intake or cooling for brake systems for example.
01:37 Crucially when using the flange tool, sharp corners in the profile would become bends in the resulting flange, automatically set to the minimum radius from our sheet metal rules.
01:47 OK so let's jump back over to Fusion 360 to have a look at all these features in practice.
01:53 We'll start with making a base flange as the sheet metal body using the flange tool.
01:58 First, we sketch a simple rectangle, say 150 x 200 mm on the top plane with the bottom corner on the origin.
02:07 Then using the flange tool and selecting our rectangle profile, we can see our 3D sheet metal body start to generate.
02:14 The orientation preference defines what direction from our profile plane we want to add thickness so in this case we can set this to one side so the top plane will be in line with the bottom face of our sheet metal base flange.
02:28 Side two would have the plane in line with the top face and centre, as you might have guessed, would have the plane through the middle of the thickness, halfway between the top and bottom faces.
02:39 Since we have no existing bodies in the model, we'll leave the operation as new body.
02:44 We also have the option to choose what rule set we want to apply because this is our initial sheet metal body.
02:51 Let's set this as stainless steel for now.
02:53 After we hit OK to execute our flange feature, we can always come over to our browser and swap the rules to a different material, steel for example.
03:03 The steels rules are set to 2.5 mm thickness by default so as you can see, our flange base is 2.5 mm thick.
03:11 Let's say we wanted to change this to 3 mm.
03:14 We'd just need to come over to the sheet metal rules in the modify tab and under the rules in this design, edit the steel rule by clicking the pen icon.
03:23 So let's change the name to steel 3 mm and change the thickness to 3 mm.
03:30 SInce the bend conditions are all referencing this thickness, they'll update automatically.
03:35 To be sure, we can quickly confirm the thickness was updated by using the measure tool from the inspect tab.
03:42 All we need to do is click the bottom and top face, this will give us the distance between the two.
03:48 Just like with the extrude tool, there are usually multiple ways that we could have made this first body.
03:54 For example, let's quickly delete what we've done and then create a new sketch on the front plane, consisting of a straight, horizontal 200 mm line from the original along the X axis.
04:05 Now we can use the flange tool on this open sketch profile with a distance of 150 mm.
04:11 Maybe as a negative value depending on which direction we want.
04:15 As you can see, we've made the same base flange as we had originally, basically using a simple example of a contour flange.
04:23 We'll come back to a more complex example of a contour flange soon but for now, let's create another flange on the edge of this base.
04:31 We don't need another sketch for this so let's just select the flange tool and click any of the four edges on the top face to start.
04:39 Using the arrow,, we'll just drag the height up to 40 mm to see the flange.
04:44 We can drag the other point to change the angle of the bend over or under the 90° default.
04:50 Notice as we move it, the original edge we selected for the bend also moves.
04:55 The height datum and bend position preferences also have an effect on this so as always, have a good play around with these settings and see what influence they have.
05:04 Up top we can change the full edge preference in the drop down to define the flange length relative to the edge.
05:11 If we don't want the flange to be along the entire edge, we could change this to the two side setting and bring one side in so it's 30 mm from the centre.
05:21 OK let's rotate the model around to see the other side.
05:24 You'll notice that there's a bend relief.
05:26 This, along with the bend radius is controlled by our rule set and ensures the part won't fracture or deform when being made.
05:35 Remember that we can override the rule set and change the shape and dimensions of these features which by default are functions of the material thickness.
05:43 So why don't we add another edge selection to see some of the other features available when making flanges? I'll choose an edge directly connected to the original edge.
05:52 The flange height and bend angle of both flanges will be the same because we're making them at the same time.
05:59 If we select the mitre option, and we over bend the part past 90°, material is removed to avoid the flanges intersecting each other.
06:08 If we bend less than 90°, material is added to fill the gap in the corner.
06:14 Obviously we can just deselect the mitre option if we want to have a right angle corner here.
06:19 Or we could use the two bend corner override rule to manipulate the relief shape between the flanges.
06:27 This is really helpful if we intend to weld the two flanges together for example.
06:31 So always keep the manufacturing process in mind.
06:35 With that covered, let's click OK as it is and we'll move onto creating an example of a contour flange on one of the unbent edges of the base flange.
06:44 We'll start by sketching on the front plane again and creating an open sketch profile, straight up from the origin, horizontal and then vertical again.
06:53 We'll make each line 30 mm long for simplicity.
06:57 Next, using the flange tool, we'll select this open profile and also the edge of the base flange.
07:04 Now we have a contour flange with the sharp corners automatically set to the bend radius controlled by our rules.
07:10 In this case, you can see that the open profile sketch intersected the edge of the base flange.
07:15 That's not actually required though so if we go back and change the profile so that it's just off the edge of the base flange and then redo the flange tool operation, we can see that the software automatically connects the profile to the edge for us.
07:31 As you can see, there's still the same flexibility as before when using the flange tool without a sketch.
07:37 The last thing we want to look at is a lofted flange.
07:40 For an example, we'll create a sheet metal loft from a square profile to a circular profile.
07:46 Starting with a new design, the first thing to do is make some sketches for the profiles of the loft.
07:53 On the top plane, let's sketch a 100 x 100 mm square, centred on the origin.
07:58 Then on an offset plane, 200 mm above the top plane, we can sketch a 100 mm diameter circle, also centred on the origin.
08:08 From here, it's as simple as using the flange tool, changing over to the lofted flange type and then selecting both of these profiles.
08:17 There are a few preferences that we have with the standard flanges but also some loft specific ones.
08:22 The formatting type options of brake form or die form, define the tooling that we would use to form the sheet metal.
08:30 A brake form gives us a straight fold along the edges whereas the die form can give us a nice curved transition.
08:37 Which one we use would depend on the tooling we have available to us for manufacturing.
08:41 If we do use the brake form preference, then the following facet control preference allows us to modify the size and spacing of the bends to make the curves we need.
08:52 I recommend experimenting with these to understand the subtle differences.
08:56 Leaving these preferences as their defaults and clicking OK to finish the flange tool, we have our resulting sheet metal loft.
09:04 With this being such a new feature in Fusion 360, there's a bit of a drawback and that's the lack of a rip tool.
09:11 The rip tool is required to create a cut down the side of this feature and allow it to be unfolded.
09:16 Or more accurately the opposite, allow it to be cut by something like a laser cutter and then folded up to create this part.
09:24 According to Autodesk the rip tool won't be far away and it might even be available by the time you're taking this course.
09:31 If it's not however, in the meantime, we can use the extrude tool to make a thin cut through one face and then create a flat pattern which we'll be covering in the next module.
09:41 That just about covers all you need to know when it comes to flanges so let's just quickly run over the main points to remember from this module.
09:49 There are really four fundamental ways to use the flange tool.
09:53 Firstly, to create a base flange which is very similar to the extrude process from solid modelling but creates a sheet metal body and therefore doesn't require the conversion process.
10:04 Next we can create flanges on the edges of the base flange, which are like new sheet metal walls connected to the original part by bends.
10:12 We can also use open sketch profiles to create contour flanges of irregular shapes along the edges of our base flange.
10:19 Finally we can now create a lofted flange in Fusion 360 but if the profile forms a complete loop, we need to split it in some way so it can be unfolded and therefore manufactured.
10:31 In our flange toolbox, we have a range of settings that allow us to manipulate the shape of the flange and we can also adjust and override the sheet metal rules, as long as we consider the manufacturing process.

We usually reply within 12hrs (often sooner)

Need Help?

Need help choosing a course?

Experiencing website difficulties?

Or need to contact us for any other reason?