3D Modeling & CAD for Motorsport: Extrudes and Holes
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Extrudes and Holes
09.10
| 00:00 | - The extrude tool might be the most useful and commonly used tool when creating 3D solid models and if you're at all familiar with the extrusion manufacturing process then you might have a good idea of how this tool works in CAD. |
| 00:12 | For those that haven't dealt with extrusion before, let's take a quick look at how this functions now. |
| 00:18 | In CAD, the extrude tool is used to add depth to a sketch or a profile, creating a 3D solid or surface. |
| 00:26 | In the same way, it can be used to remove material from a model with an existing solid body. |
| 00:31 | The basic process is quite simple, given we've already done our ground work in the form of datum planes and sketches. |
| 00:38 | Let's open our earlier model again with our previously made sketch of the 3 bolt flange. |
| 00:44 | Just looking at our sketch first, we can click the different areas of it which turn a darker shade of blue, these are the different profiles we have in our sketch that can be used to create 3D bodies. |
| 00:55 | When we select the extrude tool or hit E on our keyboard, the pop up window for the extrude tool appears on the far right. |
| 01:02 | In the popup box we are prompted to select the profile so now we can select any of these profiles we just discussed or even multiple at once. |
| 01:11 | For now, we'll just use the standard profile for the flange without any of the holes. |
| 01:16 | Alternatively we could also select the profile first in the model space and then click extrude. |
| 01:21 | Using the arrow, we can drag and add some depth and now you can see we're able to visualise the solid body. |
| 01:28 | We've extruded a 3D body from a 2D sketch. |
| 01:32 | If we head over to the popup on the right and swap between extrude and thin extrude, we can see the difference in the resulting model. |
| 01:39 | It's essentially either an extrude of the entire area inside the sketch profile or thin extrude just the borders around the edges of the shape. |
| 01:49 | Notice here that with the thin extrude we also have the option to change the wall thickness. |
| 01:55 | In this case, the thin extrude would give us five new bodies where the normal extrude tool would give us just one. |
| 02:01 | Either is fine, depending on what you're trying to achieve so it's just something to keep in mind. |
| 02:07 | OK so let's check out our options in the pop up list from the top. |
| 02:11 | First we can set the start point which is the base of the extrude to either the profile plane, an offset distance from the profile plane or an existing object. |
| 02:22 | Next we can extrude in either one direction, two directions, or two directions symmetrically with specified parameters which are referred to as extents in Fusion 360. |
| 02:33 | When specifying the extent, we can set a distance for the extrude, or extrude up to a selected surface, or use the through all preference which I personally find the most useful when removing material as it makes cuts through entire bodies. |
| 02:49 | As you can see here, we can also set the taper angle for the extrude. |
| 02:53 | Note that making it a negative number reverses the taper angle. |
| 02:58 | Finally we have the operation preference. |
| 03:00 | Here we set whether we want to create a new body, join to an existing body, remove material or use the intersection preference to keep only the body where there is an intersection between the new extrude and the existing body. |
| 03:15 | I know that sounds a little complex for now but we'll be taking a closer look into it in just a moment and it'll make more sense. |
| 03:22 | In this case, we don't have any existing bodies so our only real option is for a new body. |
| 03:27 | So let's execute that with an 8 mm distance as the extent with the start point as the profile plane. |
| 03:35 | The result is a 3D model of our flange that looks just like the real sample we took our measurements from in the 2D sketching module. |
| 03:42 | OK so let's right click to edit the extrude feature in the timeline and also select the three bolt holes as profile so they are filled in. |
| 03:50 | This lets us experiment with some other settings and understand the changes they'll make. |
| 03:55 | Now if we select the extrude tool and make our sketch visible again in the browser we can select one of the bolt holes as the profile. |
| 04:04 | You'll see we also have the option of a new component now which just means a new part. |
| 04:08 | We can also add new components from the browser and the tool bar to form our assemblies. |
| 04:15 | This is something that's specific to Fusion 360's top down modelling method and we'll come back to cover this in more detail in the upcoming assemblies module. |
| 04:24 | Rather than join, if we use the cut operation preference and drag the extrude through the part, we can remove material. |
| 04:31 | Using the intersect preference, we're only left with the body at the intersection between the extrude and the existing body as you can see here. |
| 04:40 | And lastly we have the new body preference which is pretty self explanatory. |
| 04:45 | Let's choose to cut the existing body to make a hole with the extent setting as all. |
| 04:50 | Now that we have an understanding of what the different extrude operations do, let's take a closer look at making holes in the an existing body. |
| 04:59 | The extrude tool allows us to remove material and it's one of the easiest ways to create a hole in our model by using it on a circular 2D sketch like we've just done here. |
| 05:10 | However if the hole we need is a little bit more complex, it may require a few additional tools and processes to achieve what we want. |
| 05:18 | This is where the hole tool comes in handy because it has the ability to generate different hole types with countersinks, taps, clearances, tapered holes and a range of other options. |
| 05:28 | We can spec the hole dimensions and exact thread designation and the tool will create it automatically for us. |
| 05:34 | It's just a matter of understanding the requirements and selecting the preferences to match. |
| 05:39 | For example, let's select the holes tool or use quick key H. |
| 05:44 | The hole tool does require the use of some references so let's leave our sketch visible to use it to position the holes. |
| 05:52 | First let's select the centre points for the two remaining uncut holes. |
| 05:57 | Then set the extent as all. |
| 06:00 | We'll need to flip the direction to cut through the flange. |
| 06:03 | With the hole tap type set to simple, we can fill out the dimension preferences as we like, setting the diameter to 11 mm to match the existing hole. |
| 06:12 | But if we change it to a clearance, tapped or tapered hole, we get a range of drop down lists we can use to spec the hole to common standards. |
| 06:21 | For example, we could create a tapped, full thread, flat bottom hole with an M10 x 1.5 right hand thread. |
| 06:30 | We can also choose to model the thread but be aware that this can increase the file size substantially, potentially slowing down our processing speed. |
| 06:39 | Most designers avoid this and instead add a note on the final technical drawing, stating the thread type for each hole so it can be programmed by the machine operator when it comes time for manufacturing. |
| 06:50 | This is what makes the hole tool so good without it we'd have to start with the extrude tool to create a basic hole and then use a combination of chamfer, revolve and sweep tools to cut the countersink and threads. |
| 07:03 | We'll be looking at these tools in coming modules as they each have their own valid uses but as you can imagine, the hole tool saves us a huge amount of time and brainpower by automatically generating these features. |
| 07:15 | One thing to note is that the thread tool can be used to add threads to an existing cylindrical surface if we don't need to model the hole. |
| 07:25 | For now, let's change our example back to a simple 11 mm hole through the part and finalise our model by pressing OK. |
| 07:32 | Now our 3D model for our exhaust flange is complete, the next step might be creating a technical drawing or DXF file to get it manufactured, or using it in an assembly model, all of which we'll be covering later in this course. |
| 07:44 | OK so let's recap, in this module we've covered two different tools. |
| 07:48 | The extrude tool allows us to add depth to our sketches and generate 3D solids and surfaces, add and remove material from existing bodies or generate new bodies. |
| 07:58 | The process of cutting and removing material from existing bodies with the extrude tool can be helpful for creating simple holes but as these hole features become more complex, it's best to use the hole tool where possible to automatically generate the more complex elements. |
| 08:14 | This is going to save a lot of time and avoid simple mistakes caused by human error. |
| 08:19 | As with everything in CAD, there are usually multiple different ways we can create the same model and while there's no wrong answer some methods will be a lot faster and tidier than others. |
| 08:30 | Forward thinking and of course more experience will speed up the process. |
| 08:34 | While we'll be covering some of the more important tools for creating 3D solid bodies in upcoming modules, there are so many useful tools that we can't look at every single one. |
| 08:44 | So as always, I recommend experimenting with every tool you come across and seeing what's possible. |
| 08:50 | Most of the tools found in CAD software are based on real world manufacturing processes so you should be able to model anything that can be manufactured and potentially things that can't, so with that in mind, it's always good to keep the important lessons learnt in the design fundamentals section in mind. |
