3D Modeling & CAD for Motorsport: Dimensions and Tolerances
Watch This Course
$199 USD $99.50 USD
-OR-
Or
8 easy payments of only $12.44
Instant access. Easy checkout. No fees.
Dimensions and Tolerances
11.26
| 00:00 | - In this module, we're going to look at one of the key functions of creating drawings, the dimensions. |
| 00:05 | We use dimensions to define the geometry of our parts on our drawings and while technical drawings are to scale and it may be possible with simple shapes to measure a printed drawing doing it in this way will most likely result in errors. |
| 00:19 | So we add dimensions to the drawing to show the actual intended measurement, taking any guess work out of the equation. |
| 00:26 | Depending on the purpose of our drawing, these can then be used to make the design or to check its accuracy when compared to the finished part. |
| 00:35 | There are some things that need to be considered when adding dimensions though. |
| 00:38 | As we've discussed already, all the information required to make the part or check the finished part must be shown clearly in the drawing but at the same time we don't want to add every dimension we can come up with as this will likely just over complicate things and make it hard to read. |
| 00:56 | Ideally we want to show dimensions that can be measured. |
| 00:59 | For example, we should avoid dimensioning to tangent edges as these are likely not visible on the final part so extremely hard to measure to. |
| 01:09 | Hole centres are useful for manufacturing the part and aren't too difficult to measure to but it could also be handy to measure to the edge of holes if the intention is just to check the part. |
| 01:21 | Under our dimension tool set, found in the drawings toolbar, we have a range of different dimension types we can use. |
| 01:28 | The top icon labelled with just the word dimension automatically creates a dimension depending on what we select. |
| 01:36 | For example, if we select a line we'll get the length of the line. |
| 01:40 | Two parallel lines will give us the distance between the lines, two lines at an angle will give us the angle, a circle will give us the diameter, a curve will give us the radius and so on. |
| 01:53 | If the resulting dimension from this auto dimension tool isn't the type we're after, then we can select from the other dimension tools, specifically the type we want. |
| 02:02 | Most of these are pretty self explanatory but as always, a bit of experimentation with these tools will show you all you need to know. |
| 02:11 | Let's jump back into Fusion 360 and take a look at how all this works by adding some dimensions to our wheel hub drawing. |
| 02:17 | It's always good practice to show the overall dimensions of a part so we can understand its size quickly for purposes such as raw material stock, understanding if it'll fit in our 3D printer, or even shipping. |
| 02:32 | So we'll start with some simple linear dimensions to show the width and depth. |
| 02:36 | Using the auto dimension tool on the top view, we can select the bottom and top edge to get the vertical dimension if 82 mm as our part depth. |
| 02:47 | Then move this out to the side so we can read it clearly and click again to place. |
| 02:52 | We can do the same with the side edges being the outer faces of the flange to get the width dimension of 140 mm. |
| 03:01 | This is actually the same as the height of the part because it's really just the outer diameter of the flange. |
| 03:07 | Since it's really a diameter dimension, we might want to add the diameter symbol to it by double clicking the dimension to bring up the dimension pop up window and then inserting the diameter symbol before the dimension. |
| 03:20 | Now we just click OK to execute. |
| 03:23 | We could also show this diameter on the front view by selecting the outermost diameter of the part. |
| 03:28 | We want to avoid doubling up on dimensions though so it's best to just choose whatever one is more clear. |
| 03:34 | We'll leave the diameter dimension on the front view and delete the linear dimension on the top view. |
| 03:40 | Next let's dimension our PCD holes, starting with the diameter of the holes itself, using the auto dimension tool again. |
| 03:48 | We also want to show the diameter of the PCD so we'll add that in now. |
| 03:54 | We'll leave them as it is for now and come back to it in a moment. |
| 03:58 | Similar to the diameter dimensions, are the radius dimensions. |
| 04:01 | Like we discussed earlier when looking at tangent edges, all the sharp edges of this part have been rounded using the fillet tool to avoid stress concentrations. |
| 04:11 | If we need a refresher on these by the way, jump back to the modify tools module in the solid modelling basics section of this course. |
| 04:19 | Each edge is curved with a relatively small radius compared to the size of our part so it's the ideal time to use our detailed view. |
| 04:28 | Using the auto dimension tool again, we can select the curved sections of the edge of the part showing both the internal and external corners have a radius of 1 mm. |
| 04:39 | Our wheel hub also has a series of angled faces and although they're not overly critical to how our part functions, we'll dimension them anyway for this example. |
| 04:49 | As I mentioned before, if we select two parallel lines we'll automatically get the distance between them as we also would with a point and a line or two points. |
| 04:59 | However, if we have two lines that aren't parallel, we'll automatically get the dimension for the angle between them. |
| 05:06 | Let's use that to show the angle of the internal recess on our section view, again using the auto dimension tool and selecting the two lines. |
| 05:14 | Before we place it, notice how moving the cursor outside or inside the lines changes the angle we're given. |
| 05:21 | We'll place it between the lines just out to the right of the view. |
| 05:25 | Now the ordinate dimension tool found here is slightly less intuitive than the other dimension types. |
| 05:31 | It creates a set of dimensions measured from a 0 point and in Fusion 360 for each view, we can only have one of these 0 points. |
| 05:41 | For our part this can be helpful to show the location of features relative to an important surface like the surface for mounting the brake rotor for example. |
| 05:50 | Let's select the ordinate dimension tool and then on our section view, select a point on the flange surface as the 0 point. |
| 05:58 | Next we can just select the points on our model to dimension to like the two surfaces that the wheel bearings would be pressed up against. |
| 06:06 | We could come back to add to this at any time with the ordinate dimension tool. |
| 06:10 | For this example we've just shown the horizontal dimensions but we could use the same 0 point and also show the vertical dimensions if it suited our model. |
| 06:19 | Now if this wheel hub was going to be machined manually, using only the drawing as a reference then some more dimensions would be required. |
| 06:28 | Realistically though, a part of this complexity would be most likely made in a CNC machine. |
| 06:34 | In this case we'd provide the manufacturer with a 3D CAD file as well as our drawing with the dimensions we've added, allowing them to check the important measurements once the part has been made. |
| 06:47 | While we're discussing checking of the finished part, tolerances are an important factor to consider when it comes to dimensions. |
| 06:54 | Tolerances are helpful for defining the variation between the finished part and the actual intended dimension that's acceptable. |
| 07:01 | It's important to note at this point that although tolerances are generally more suited to a professional environment and mass production where quality control is more relevant, they can still be very helpful on dimensions that are critical to the function of our design. |
| 07:16 | This is so a manufacturer understands it's important and will hopefully take the extra care to make sure the finished part is within our specified range. |
| 07:25 | The acceptable variation ideally would be determined by what's called a tolerance stack analysis. |
| 07:32 | This involves the accumulated variation of parts and assemblies in order to find the potential range of how the final parts might fit together. |
| 07:41 | For example, take a press fit bolt in a hole, if the bolt has a 12 mm diameter, but the tolerance is +/- 0.3 mm and the hole is supposed to be an 11.9 mm diameter, but the tolerance is +/- 0.5 mm, we could end up with an 11.7 mm diameter bolt and a 12.4 mm hole which won't be a press fit at all. |
| 08:09 | If we're ever adding tolerances to dimensions, we need to be realistic. |
| 08:13 | There's no point in adding a tolerance of +/- 0.1 mm to a part that's going to be made by hand because it's highly unlikely that this will be achievable. |
| 08:24 | Setting tolerances requires a good understanding of the manufacturing process so if you're concerned about it, it may be worth talking to the manufacturer about what they think is suitable as you may need to rework your design to account for it. |
| 08:38 | The process of adding tolerances to dimensions is actually relatively simple. |
| 08:43 | Let's look at the overall depth of 82 mm on our top view. |
| 08:48 | This isn't overly critical but we do want it to be somewhat accurate. |
| 08:52 | If we double click the dimension, in our pop up window we can change the tolerance setting to symmetrical and set the tolerance to 1 mm. |
| 09:01 | So we're now specifying that the measurement anywhere between 81 and 83 mm is acceptable for this dimension. |
| 09:11 | Now let's look at something a little bit more critical, our bolt hole size. |
| 09:15 | This needs to be a press for for an M12 wheel stud. |
| 09:20 | Full disclosure, this is just an example, not a real design where I know the actual size of the stud. |
| 09:26 | For a more suitable tolerance for something like this we could use the deviation tolerance setting, specifying an upper tolerance of 0 and a lower tolerance of 0.1. |
| 09:36 | That means this hole can be no larger than 12 mm and no smaller than 11.9 mm in order to avoid the press fit being too loose or too tight. |
| 09:47 | The limit tolerance setting is interchangeable here and will also give a suitable result. |
| 09:53 | Let's briefly run through the key points we've covered in this module before finishing up. |
| 09:56 | Dimensions are a critical feature that show the actual intended size of the geometry in our final product. |
| 10:04 | What dimensions we show can depend on the intention of the drawing as in, if it's going to be used for manufacturing the part, or just for checking the manufactured part. |
| 10:16 | The standard dimension tool goes a long way by automatically generating different types of dimensions depending on the selected features. |
| 10:23 | In some cases though we may need to use the specific dimension tools to get our desired outcome. |
| 10:29 | Also remember that your dimensions should be useful and actually possible to measure. |
| 10:34 | Tolerances are an additional factor to be considered when working with dimensions and are used to define the acceptable variation between the intended dimensions and the actual measurement of the real part. |
| 10:46 | In some cases though, we may need to use the specific dimension tools to get our desired outcome. |
| 10:53 | Also remember that your dimensions should be useful and actually possible to measure. |
| 10:58 | Tolerances are an additional factor to be considered when working with dimensions and are used to define the acceptable variation between intended dimensions and the actual measurement of the real part. |
| 11:10 | Any tolerance should be thought out before being applied and potentially discussed with the manufacturer to see what they think is achievable. |
| 11:18 | Ideally this would be done before the design is finished as it may result in some revisions. |
