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3D Modeling & CAD for Motorsport: 2D Sketching

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2D Sketching


00:00 - In CAD software, we use sketches as references and to build features from.
00:05 A sketch is a drawing or profile that forms the boundaries of 3D bodies.
00:10 It's possible to sketch in 2D or 3D in Fusion 360 and each has its own uses.
00:16 We'll start by looking at 2D sketches in this module to understand the fundamentals before diving into the slightly more advanced 3D sketches in the next module.
00:26 The datum planes we discussed in the previous module are the groundwork or foundations for our sketches as we mostly create our sketches on these planes.
00:36 We can also create sketches on the existing faces of a model.
00:40 Just know that the process is the same either way.
00:43 Back in Fusion 360 in the design workspace under the solid toolbar, we can find the create sketch button.
00:51 This can also be found under the surface and sheet metal toolbars and they all bring up the same sketch tool, but let's stay under the solid toolbar for now.
01:00 There are two ways we can create a sketch at this point.
01:04 First we can click the create sketch icon, or we can use the shortcut search feature by hitting S on our keyboard and then typing in sketch.
01:13 Now windows have popped up yet but you can see by the cursor that we are being prompted to select a plane or planar face which is really just a flat face.
01:22 Alternatively, if we cancel this, we can actually just right click on the plane we want to sketch on.
01:28 We'll choose the front plane for now and then click create sketch.
01:33 So now we have a new toolbar along the top of the workspace.
01:36 This contains all the tools we use to create a modify a sketch including a bunch of different constraints we can apply to our sketch features to help us get everything where we need it.
01:47 Here on the right you'll also find some inspection and insert tools as well as different options for selecting features.
01:55 There's also a sketch palate with some more tools for changing the line type.
01:59 For example, setting this to construction lets us draw in lines to help create the sketch but not feature in the final profile.
02:06 Essentially invisible lines for construction purposes.
02:10 The sketch palate also has a range of other view options that we can turn on and off.
02:15 So let's quickly turn off the grid setting to make things a little clearer and easier to see.
02:20 "Look at" here at the top is particularly useful because if we move our model around in the space we can click look at and it'll bring us back to viewing our sketch directly straight on.
02:30 OK so let's move on and use some of these tools to start drawing and make a sketch.
02:35 Up in this top create section, we have some commonly used create tools.
02:39 Line, rectangle, circle and so on.
02:43 Under the drop down we have a bigger list with all the different variations of those tools.
02:48 For example, here are the two point rectangle and centre rectangle tools which are just slightly different methods of creating the same thing.
02:55 As you get more familiar with CAD, the names of all of these tools are going to become much more self explanatory and you'll quickly start getting a better feel for what to choose in order to make the sketch process easier and faster.
03:08 Now if we hover over the tools, we get the same pop up that we talked about earlier but you'll also notice that next to the name at the top of the popup window, there's a letter in brackets.
03:19 This is the quick key shortcut.
03:21 If we press this key, it'll automatically select the tool.
03:25 While they're not essential to know in these early stages of learning the software, it's a good idea to keep these quick keys in mind because they can really speed up your workflow once you start becoming more proficient.
03:36 Having a basic list of quick keys next to your computer is never a bad idea and you can look underneath this module where you'll find a handy printable sheet that we've put together which lists all the most commonly used quick keys.
03:49 OK so let's look at creating the sketch for our 3 bolt exhaust flange.
03:53 Working off this real sample we have on hand to see how it all works.
03:57 Although this is a pretty simple part, the sketch to make it does actually require a few different elements.
04:03 We'll start with a simple centre diameter circle, you'll also notice a few more options in our sketch palate that let you change between different circle types but for now, let's just stick to the basic tool.
04:15 Let's place the centre point on the origin.
04:18 Once we click and then move our mouse, we can adjust the size of the circle.
04:22 Using our verniers to measure the inner diameter of our example, we can see that it's 61 mm so let's add that dimension to our sketch now.
04:31 We can hit enter or click to execute.
04:34 If we entered it wrong, or just wanted to modify it, we can also change the size of the circle by clicking the dimension here and changing the value.
04:42 Also, if we select the dimension tool, which is quick key D, we can dimension the circle size if we hadn't already.
04:50 Notice that the outline of the circle is black.
04:53 That means that its size and position are fully defined.
04:56 We always want to fully define our sketches where possible to avoid unintentional changes.
05:01 If features in the sketch aren't fully defined, they'll appear blue which we'll see in a moment.
05:07 OK now it's time to add the three bolt holes.
05:11 Using the same circle tool, if we hover over the centre of the large circle for a moment, and then move the cursor up, we can see that it stays in vertical alignment.
05:21 Then we just click to place the centre and measuring our sample again, we can see that we want these holes to be 11 mm in diameter so we'll drop that in.
05:31 As we add the other two circles in each side down the bottom, we don't want to dimension them.
05:36 Instead, we want to use our equal constraint to make the three bolt holes the same diameter.
05:41 To do this, we just select the equal constraint here, click the top circle and then click a new circle, then repeat for the remaining circle.
05:49 The equal constraint icon appears next to the feature and if we click it, we can also see the constraint icon on the corresponding feature as well as some text in the bottom right of our screen.
06:01 So now we have our three circles for the bolt holes and the diameter is defined.
06:06 If we change the diameter of the top circle, the other two will change to match.
06:10 Now we need to define the position of the holes.
06:13 First, let's use the horizontal vertical constaint to lock the centre of the top circle vertically in line with the origin.
06:21 This isn't 100% necessary in order to make the sketch for this part but it helps keep things in clear orientation and it will allow us to fully define the sketch so it's best practice.
06:33 Since the hole is closer to vertical alignment with the origin, it'll automatically use the vertical constraint rather than the horizontal.
06:41 We can use a horizontal constraint between the two bottom circles.
06:45 You'll notice that our three smaller circles are still all blue, meaning that their position is not fully defined, so let's take a look at using some of the other sketch tools and constraints to get this done.
06:57 The simplest of them all is the line tool and we'll actually turn the line type to construction before we create these lines since we won't actually want to show them in the final profile.
07:07 They're just there to define the position and the spacing of the bolt holes.
07:11 Let's start by adding a construction line from the centre of the top circle to the centre of the bottom left circle and then connect this straight across to the bottom right circle.
07:21 Note that if we're using the line tool, it'll continue to create a chain of lines, nose to tail, until the line finishes on the feature of a sketch.
07:29 However, if we want to finish using the line tool mid way through a chain, this is the perfect time to use the escape key to cancel the command and exit the tool.
07:38 Measuring our sample part again, we can see that the distance between each bolt hole is 80 mm so let's select the dimension tool, or use quick key D to dimension one of these lines at 80 mm.
07:51 Then we can just use the equal constraint between the lines.
07:55 Now we can see that our three small circles aren't equal distance from the centre.
07:59 There's a few ways to fix this but the most efficient is to sketch a construction circle, centred on the origin and through the centre of one of the smaller circles.
08:10 Then we can use the coincident constraint to make the centre of the other two circles lie on the construction circle.
08:17 And now as you can see the entire sketch is fully defined as it goes black.
08:22 This is starting to look like the PCD or pitch circle diameter method where the bolt holes are equally spaced on a circle.
08:30 If there are an even number of bolt holes, four for example, we could easily measure the distance between opposing holes on the sample to get the diameter of the pitch circle.
08:40 This isn't possible with an odd number of holes though.
08:43 We could however delete the 80 mm dimension now and dimension the construction circle.
08:48 We see that this is currently just over 92 mm.
08:52 If we actually change it to 92 mm and quickly check the measurement between the holes again, it's now at about 79.6.
09:01 This is very close and given that measuring between hole centres with verniers isn't the most accurate method anyway, this would be close enough for our example.
09:10 We still need the construction lines though to keep the holes equally spaced.
09:14 This is now what's known as a 3 x 92 PCD.
09:18 Moving on, all that's left to do is create the outer edge of the flange.
09:23 If we measure the thickness of the part between the inside of the centre hole and the outer edge, we get 15 mm.
09:30 We need to deselect the construction line preference so our next lines are included in the final profile.
09:36 Let's use the offset tool from under the modify tab to do this.
09:40 Select the inner diameter as the profile and set the offset distance to 15 mm.
09:45 This creates an identical profile offset from the original.
09:49 Using the same method, we can offset the three bolt holes by 5 mm.
09:54 Next we want to use another one of the modification tools called trim to remove the unwanted parts of the profile.
10:00 If we hover the cursor over the areas of the profile, it'll show the section in red that'll be removed and blue that will be retained.
10:09 In some cases, clicking and holding and then dragging through the profile can quickly remove sections.
10:15 In our case though, we want to remove the areas of the offset circles inside the outer profile.
10:20 But we want to be careful not to trim any of the construction lines.
10:24 Notice how our offset circles change back to blue, that's because they've lost their dimensions during this process.
10:32 This is an easy fix by dimensioning the large outer curve and one of the smaller curves and then using the equal constraint to define the other two smaller curves.
10:41 The final step is using the fillet sketch tool to add a curve to the sharp corners.
10:46 The curve starts at a tangent to both the lines leading into the corner to make a nice smooth transition.
10:52 We can simply do this by selecting the fillet tool and clicking the corner point, setting the radius to 40 mm looks about right when looking at our physical sample.
11:01 With the fillet tool still active, as we click each of the other corners, they'll all have the same radius.
11:08 I'd recommend only having one of these arcs dimensioned then using the equal constraint between the arc and the others.
11:15 That way, if we change one, it changes them all and the sketch remains clear and easy to read.
11:21 Our outer diameter has become undefined again as a result of the fillet tool so we just need to use an equal constraint one more time between the three large curves and then our sketch is complete.
11:32 The last thing I'd recommend is using the show profile preference in our sketch palate.
11:36 This shades the enclosed areas light blue so we can see if we've created a closed loop, suitable for creating a 3D object using the extrude tool, which we'll be covering very soon.
11:48 This basically just allows us to identify if we've made any mistakes and have any unwanted gaps or lines inside the profile.
11:56 As you can imagine, it's possible to make this sketch in a number of ways using different tools.
12:01 The point here, as with most things in CAD, there's usually different ways to achieve what we want.
12:06 Some are faster than others and depending on what references and constraints we have, they could be more or less tolerant to modification without giving us errors or failing to regenerate.
12:16 The more experienced we get, the more efficiently we'll be able to work and the more robust our models will be.
12:23 And that means that making future modifications would be quicker when needed.
12:28 When we click finish sketch, we can now see it in the browser and on the timeline.
12:32 Keep in mind that we can come back to either location and modify the sketch at any point as the model progresses.
12:39 We can also use the sketch to create other features which we'll be doing in upcoming modules.
12:45 Before we move on, it's important that we take a look at some really helpful tools to use when making sketches that reference already existing geometry in the model.
12:55 Let's open the 3D model of the same exhaust flange.
12:57 If we select the top face to sketch on, we can use the project tool found here in the create dropdown, or just by pressing quick key P and project existing features of the geometry onto our new sketch.
13:11 For example, selecting the internal circle brings this into our sketch, then we can make another circle by using the offset tool and selecting the projected circle.
13:20 We can then set the offset to 2 mm and use the flip button to make sure the new circle has a 2 mm larger radius.
13:29 After selecting finish sketch, we can now use this new sketch to make new geometry like the start of a pipe with the extrude tool for example, which we'll be having a good look at soon.
13:40 The project function is ideal for referencing current geometry without doubling up on work and the new sketch will now change with the original feature which saves us a huge amount of time.
13:51 We've covered a lot in this module so let's quickly go back over a few key points before finishing up.
13:56 First, understand that a sketch is a drawing or a profile that forms the boundaries of 3D bodies.
14:02 Sketches are the fundamentals that we build most of our 3D features from.
14:06 We have a wide range of sketch tools available for creating, modifying and constraining our drawings, and it's important that the final sketch is always fully defined, indicated when it goes black to avoid it changing unintentionally.
14:21 It's definitely worth spending some time using these tools to get familiar with how each one works.
14:27 Once you get a feel for it, the names of the tools make their uses pretty obvious but there's always the pop up windows that appear when you hover over the tool if more information is needed.
14:37 Remember in most cases, there are different ways to make the same sketch so with some prior planning to figure out the best way to go about it, we can work significantly faster and make more robust models.
14:50 Learning the ins and outs of everything we've covered in this module is going to give you a very strong foundation for using CAD and the skills will translate to most other modelling processes.

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