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

Ends in --- --- ---

3D Modeling & CAD for Motorsport: Surface Modelling

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

Surface Modelling


00:00 - Everything we've covered up to this point in the course, could be considered the fundamental knowledge needed in order to model most components and assemblies that an automotive enthusiast would be interested in.
00:11 At least at a non professional level.
00:13 Once you have these fundamentals down, most of your further development as a designer will come purely from experience.
00:20 With a little practice, you'll be well on your way to creating some high level designs.
00:25 In this next section of the course, we'll be covering some more advanced topics though not in the same level of detail you've seen up to now as these subjects require some pretty heavy additional knowledge to master that's outside the scope of this course.
00:39 So with that in mind, the next set of modules serves to ensure that you're aware of these more advanced concepts and systems and have a broad understanding of how they work and what they do but stops just short of teaching you the intricacies of how to use them.
00:55 Though we may dig into some of these more advanced skills and techniques in the worked examples library over time.
01:01 As we've progressed through the previous section of this course, you'd have more than likely noticed the surface toolbar and probably wondering why it seems like it's been ignored.
01:12 The reality is, we've been using surface modelling to some degree already in the ways that are useful for modelling mechanical parts like structural components and mechanisms.
01:22 Lofts and sweeps are good examples of modelling where we're most concerned with the surface shape.
01:27 However, as we've used these processes so far, there's always been a thickness to the surface used to create a solid body.
01:35 Surface modelling tools generally create an infinitely thin body.
01:39 The benefit of this is it allows us to create more freeform shapes that would be difficult or maybe impossible with solid modelling techniques.
01:47 Surface modelling is really most suited to creating surfaces that have complex curves which is where the face is curved on multiple planes.
01:56 Therefore when viewing the design from different directions, we always see the curves.
02:01 Surface modelling is also useful where the thickness of the body is very thin relative to the overall size of the body.
02:09 For automotive and motorsport design, a good example of this would be the exterior of the vehicle, such as the body panels and aero parts.
02:16 But could also be useful for dashboards or other components.
02:20 Jumping back into Fusion 360, the surface toolbar features a lot of the same creation tools we've covered already such as extrude, revolve, sweep and loft as well as some other familiar modification tools.
02:34 The key difference here is these tools are creating surfaces which remember are infinitely thin bodies.
02:40 For example, if we sketch a simple rectangle on the top plane with a fillet on one corner and then use the extrude tool under the surface toolbar, we can drag the extrude up to see the resulting body.
02:54 This works just like our solid modelling extrude tool with the exception of the chaining preference which selects the adjoining lines of the profile forming a chain.
03:04 As we can see, our extrude creates a surface projected from each line of the profile.
03:10 We can turn off the chaining preference and only project the surface from the selected lines of the profile.
03:16 This is the same difference for the revolve, sweep and loft tool as well.
03:21 Let's just deselect one of the lines connected to the filleted corner by holding shift and clicking and then select OK to finish the extrude.
03:30 Notice in our browser under the bodies tab, we still have a body as we would with the solid modelling tools, however the icon is different.
03:37 It represents a surface body rather than a solid body.
03:41 Here next to the body, you can see a number In brackets, this represents a number of surfaces in that body.
03:48 Now it's time to take a look at the creation tools unique to the surface toolbar.
03:52 Let's start with the ruled tool which creates a ruled surface from selected edges.
03:58 A ruled surface is somewhat similar to the flange and sheet metal modelling.
04:04 It creates a surface that extends straight out from the edge or sketched line in a specified direction.
04:10 Let's see it in action.
04:12 If we select the rule tool and then the edges of the existing body with the chain selection tool turned on, we can now use the arrow to drag the new surfaces out.
04:23 There are three options for the type setting and these can be used to change the direction that the new surfaces project from the selected edges.
04:31 Notice we don't have the same operation preferences to create a new body, join or cut as we did with the solid modelling tools.
04:39 That means that when we click OK to finish using the tool, we automatically get a new surface body.
04:45 We'll come back and address this soon with the modification tools but first let's use the patch tool which creates a surface within a boundary of a closed loop.
04:54 The closed loop could be defined by a sketch profile or a series of edges from an existing body.
05:01 Let's use this tool and click the outer edges of the ruled surfaces that we just created.
05:07 This generates a patch over the entire boundary.
05:10 The setting in the window next to the chain also allows us to change how the new surface connects to the existing boundary.
05:18 If you think back to the lofts module in the solid modelling basics section, it's similar to how we use takeoff weights which can be a really helpful way of manipulating the shape of the surface.
05:29 For now we'll just leave it as the default setting of connected and select OK to finish using the tool.
05:35 We've used the sketch offset tool multiple times in previous modules to create a new profile based on an existing profile.
05:43 Just spaced off at a specified distance.
05:46 The offset tool in our surface toolbar works very similar to this, creating a new surface at a specified distance from an existing surface.
05:55 Let's use this tool and select the outer surface we've just created in the last step with the patch tool.
06:01 Now we can use the arrow to drag the new offset surface out a few millimetres off the existing surface.
06:07 You can see that we now get a new surface that's the same form as the original, just spaced out so it's like a scaled up version.
06:15 After we select OK to finish using the tool, we now have four surface bodies in our model.
06:21 Next up we have the thicken tool and as you've probably already guessed, it adds thickness to a surface to create a solid body.
06:29 So if we use this on our offset surface, you can see that we get a new solid body and the surface body is automatically hidden.
06:38 This is a key step in working from a stage of just having surface bodies to having a real 3D solid model that can be manufactured.
06:46 For now let hide the new solid body as well.
06:49 Next up we can head back to the surface toolbar and take a look at the modified toolset.
06:55 We can see some familiar tools, shown with the blue icons like press pull, chamfer and fillet, scale and split and they all work much in the same way as with solid modelling.
07:06 Extend is very similar to press pull except that it works by selecting edges rather than faces to extend the surfaces.
07:15 Again, there are some tools here that are unique to the surface modelling toolbar.
07:21 Stitch and unstitch follow similar ideas to how the combined and split tools work with solid body modelling.
07:28 Stitch, as the name implies, allows us to join surfaces together, combining multiple surface bodies into one.
07:35 If we use the stitch tool and then select two out of the three visible surfaces, after clicking OK to finish the stitch operation, we can see in the browser that these two surfaces have been now combined into a single surface body.
07:50 Alternatively, similar to the thicken tool, we can convert the surface bodies into a solid body.
07:56 If we undo this and repeat the process but this time select all three surface bodies, the result is a single solid body because the selected surfaces form a complete enclosure.
08:08 Lastly, unstitched naturally works in the opposite way, splitting the body along the edges into individual surfaces.
08:16 All these processes allow us to create irregular surfaces with more ease than the solid modelling tools.
08:22 We can then turn these surfaces into solid bodies which can be developed into a solution that can actually be manufactured.
08:29 To summarise this module, it's unlikely that we'd be using surface modelling regularly for the kind of common parts we'd be designing and modifying on vehicles.
08:39 But it can be handy when modelling really complex curves or bodies that are very thin compared to their overall size.
08:47 We also have the ability to patch open areas between profiles as well as create ruled surfaces from sketches or existing surface edges.
08:57 The key point is how surface bodies can be thickened or stitched together to create solid bodies and then model parts that can be manufactured.
09:05 It's also possible to use conventional solid modelling tools with these surfaces.
09:10 For example, using the extrude tool to extrude a profile up to a surface.
09:15 As always, it's important to experiment with the different tools to see what you can create.
09:20 As there's a lot of flexibility in these process, there are a lot of different ways to model what we need and there's no right or wrong answer, just some that might be better, more efficient and more stable to modification than others.

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?