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3D Modeling & CAD for Motorsport: Analysis Tools

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Analysis Tools


00:00 - Being able to analyse a design is one of the key advantages to modelling it in CAD software.
00:05 Now the reality is that we're generally always going to be analysing our design as we're modelling it.
00:10 But for the purposes of this module when we say analysing, we're specifically talking about using the analysis tools offered to us in CAD software.
00:19 These tools allow us to gain a much deeper understanding of our design by leveraging the computer processing power.
00:26 We use the analysis tools to find areas of a design that can be changed and optimised, making improvements for whatever the intended purpose is.
00:34 We can also identify potential issues before manufacturing saving time and money.
00:40 In performance automotive applications, key aspects to consider are mass and strength which both have an effect on performance and safety.
00:49 We might also be interested in other factors like the stiffness of a suspension arm so it doesn't flex and introduce compliance into the system.
00:58 These aspects relate back to our design fundamentals and of course manufacturability is also an important consideration.
01:05 Before we go any further, it's important to understand that analysis tools can help us review our designs in relation to these factors but they won't just optimise a model on their own.
01:16 That means what really matters is how we interpret the results and what changes we make.
01:21 Let's head back into Fusion 360 and take a look at some analysis tools found under the inspect tab in our toolbar and also in our utilities toolbar.
01:32 We'll start at the top with the interference tool which on selecting multiple solid bodies or components will show us any interference between the selections.
01:40 This is most helpful when we have complex assemblies, possibly with moving components and we want to check if we have any unwanted contact between the components.
01:51 I say unwanted because sometimes we may be designing assemblies which have press fits so naturally we expect to see some interference here.
01:59 When using this tool, we first select the bodies we're interested in and then hit the compute button which will show us any interference.
02:07 As we can see, the bodies are now transparent and the interference is clearly shown in red.
02:13 We're also shown the volume of the interference.
02:16 For cases where there is no interference, but we want to include parts that are just touching each other, like two parts that are going to be bolted or welded together for example, we need to select the include coincident faces box.
02:32 Naturally there won't be any interference volume here.
02:35 Hitting OK will finish using the tool.
02:38 Before we move on, you should know that the interference tool is also really useful for removing interference volumes but with that said, this can't be done while capturing design history which takes place down in the timeline.
02:52 We need to first right click the design file at the top of the browser and down the bottom choose do not capture design history.
02:59 See how the timeline disappears, notice if we do the same process as before with the interference tool, we now get different options when we click compute.
03:08 We can now select remove volume to remove the interference.
03:13 As well as which component we want to cut it from.
03:16 After this we can change our setting back to capture the design history.
03:21 Unfortunately though, as you can see we've now lost all of the previous history in our timeline.
03:26 With that covered, let's take a look at the draft analysis tool.
03:30 As we discussed in the modify tools module in the solid modelling basics section, drafts are most useful for injection moulded or cast parts and due to the relatively high expense of tooling, it's unlikely we'll be using this as our manufacturing method.
03:45 However if we are, this tool is able to show us faces with not enough draft or negative draft, meaning that the surface is angled the opposite way to the direction that the tool would pull away.
03:57 Therefore identifying areas that could make ejection from the tool an issue.
04:02 Moving on, we also have the curvature map analysis tool which displays a coloured gradient of the selected bodies to help us visualise the different degrees of curvature in our model.
04:13 The curvature cone, zebra and iso curve analysis tools are also used for analysing the curvature of surface on our models using alternative illustrations.
04:24 As with the draft analysis tool, these curvature tools are probably of little use to us in most cases.
04:29 They do have their place though in helping develop aero components with complex curves.
04:35 However, thinking back to our design fundamentals module, they can also help identify sharp corners that would cause stress concentrations.
04:43 Likewise with the minimum radius analysis tool, we can quickly identify areas with a radius below a specified value.
04:50 For holes and fillets on internal edges, this is useful for determining the minimum tool sizes for machining.
04:58 The main use for the accessibility analysis tool is also related to machining as this helps us determine whether or not areas of the model are accessible from a certain direction which naturally allows us to undertand if they can be machined successfully and identify undercuts that could cause issues.
05:17 To use this tool, we simply select the bodies we're interested in, in a plane perpendicular to the direction of access.
05:24 The results are just as simple, areas shown in green are accessible and areas shown in red are not.
05:30 Next on the list is the section analysis tool which creates a cut away or cross section view of our model using a plane or flat face.
05:38 To clarify, a cross section is the intersection of a solid body in 3D space through a plane.
05:45 As you can see, we're able to drag the arrow to change the position and enter values to define it.
05:51 This can help us get a good look inside a complex part or assembly to better view an area of interest that we might not be able to see otherwise.
06:00 After clicking OK, we can see that our section, along with the other analysis tools are saved under our analysis tab in our browser.
06:08 Section views are commonly used in technical drawings to help illustrate details for manufacturing and we'll be covering these drawings in more detail in an upcoming module.
06:18 Before we finish up, those of us who are familiar with the term FEA might be expecting it to show up in this module.
06:26 FEA stands for finite element analysis and put simply, this is a method of simulating how a model will react to real world physical effects like load forces or fluid flow.
06:37 Understandably this is a fairly advanced extension of CAD so instead of just glossing over it here, we've dedicated a separate upcoming module to it in the Advanced CAD section.
06:48 OK so let's have a quick recap of what we've covered here.
06:52 With a range of analysis tools available to us in Fusion 360 found under the inspect tab, these help us critique our design and potentially find areas for improvement.
07:03 With these tools, we can find unintentional interferences between bodies or components and remove them.
07:09 Our draught analysis tools can help us identify areas with not enough draft or negative draft that will cause issues with the injection moulding or casting manufacturing processes.
07:19 We also have a range of tools that we can use to identify areas of high curvature or internal corners with radiuses that are too sharp, potentially causing stress concentrations.
07:30 This information can also help determine if we'll have issues with the machining process depending on minimum tool sizes.
07:38 Lastly, the section analysis tool lets us create a cutaway view of our models which means we can see hidden details and illustrate them in our technical drawings.

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