3D Modeling & CAD for Motorsport: Patterns and Mirrored Features
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Patterns and Mirrored Features
07.35
| 00:00 | - When it comes to automotive parts, it's pretty common to find repeating features. |
| 00:04 | For example, an exhaust manifold flange has repeating holes for the exhaust ports into the head and also the holes used to mount the manifold, both of which are often inline and equally spaced. |
| 00:17 | Another common case would be a wheel hub or spacer, a 5 x 100 stud pattern like the one we have here for example, describes five holes, most likely for M12 studs, evenly spaced on a circle of 100 mm diameter. |
| 00:33 | If we look back at the base structure of the wheel spacer we created earlier with the revolve tool, the next step would be to add the holes. |
| 00:41 | Rather than model each hole individually, we can model one hole and then use the pattern tool to replicate the hole in other locations. |
| 00:50 | Likewise, if a part or feature is symmetrical in some plane, we can model half of the part or the feature on one side and then use the mirror tool to generate the other side. |
| 01:01 | Let's now model the five holes in our wheel spacer that are for the existing studs on the vehicle to get a feel for how this works. |
| 01:09 | Because our stud pattern is 5 x 100, let's just sketch a point on the front mounting face that'll be used as a reference point to position our first hole. |
| 01:18 | We're placing it 50 mm directly above the centre, using the vertical constraint. |
| 01:24 | That's half our 100 mm pitch circle diameter or PCD. |
| 01:29 | Next, let's select the hole tool or quick key H, making sure our placement is on the top face, we can use our sketch point as a reference so the hole is centred on it. |
| 01:42 | We're using a simple counter bore hole with the extent set to through all so the drill point won't matter as the hole is bottomless. |
| 01:50 | To match our physical sample, the counter bore needs to be 23 mm in diameter and 14 mm deep and the base hole diameter is just 14 mm. |
| 02:01 | After finishing with the hole tool, we can add some chamfers to the hole like we did with our revolve face feature with our sketch tool. |
| 02:08 | Chamfers are a short sloped face that breaks the sharp corner. |
| 02:13 | When adding them to an existing 3D body, we need to select the chamfer tool from the modify tool set, all of which we'll be covering in the next module. |
| 02:23 | With the chamfer tool selected, we just select the counter bore edge inside the hole and set the chamfer type to distance and angle, using 4.5 mm and 60° gives us a nice sloping face suitable for our tapered wheel nuts. |
| 02:39 | Then we can add a 1 mm equal distance chamfer to the top and bottom edges of the hole to break the sharp edges and match our sample. |
| 02:48 | Now we're going to select the circular pattern tool from the create dropdown menu. |
| 02:52 | The type preference can be set as faces and then for the objects we will just select the internal face of the holes as well as the chamfer faces we just made. |
| 03:02 | Quantity is of course five and angular spacing is full. |
| 03:07 | This equally spaces the holes around the centre which is our case is the Z axis. |
| 03:12 | OK so let's execute that now and we can see our initial hole has been replicated five times around the centre to achieve our 5 x 100 PCD stud pattern. |
| 03:23 | In this case it might have been just as fast for us to sketch five points and create five holes but you can imagine if we wanted to replicate this hole significantly more times, the pattern tool would make this a lot faster. |
| 03:37 | The same ideas apply to using the rectangular pattern tool but in this case, we can specify multiple directions for the pattern, choosing edges, axes or straight sketch profiles to define the directions. |
| 03:51 | The pattern on path tool allows us to replicate a feature along a non linear path from a sketch profile or an edge. |
| 04:00 | Let's have a look at an example of these tools in action using a simplified model of a pedal. |
| 04:05 | This pedal looks heavy and could do with some weight reduction. |
| 04:09 | Of course we need to consider the strength effects when doing so but it makes for a good example. |
| 04:15 | We'll create some holes on the foot pad and the arm using our pattern tools. |
| 04:19 | First let's sketch a 3 x 6 centrepoint slot in the top left of the foot pad. |
| 04:24 | Positioning the centre 12 mm horizontally and 27 mm vertically from the centre of the foot pad looks about right for this example. |
| 04:33 | Then using the extrude tool, we can remove material to cut a simple slotted hole through the pad. |
| 04:41 | Now we can select the rectangular pattern tool with the type as feature and select the slot. |
| 04:47 | We can use the top and side edge of the foot pad to define the directions of our pattern. |
| 04:53 | For the distance type, we'll use extent to set the overall distance of the pattern rather than the spacing which sets the distance between each feature. |
| 05:02 | For the horizontal direction, let's use a quantity of two and a spacing of 24 mm, being twice the distance of the 12 that our slot was from the centrepoint. |
| 05:14 | For the vertical direction, again 54 is double the distance to the centrepoint to make the pattern even on the pad and a spacing of seven looks good for this example. |
| 05:25 | Clicking OK to finish, we now have our slotted hole replicated in a 2 x 7 pattern. |
| 05:31 | Next up is the arm of the pedal. |
| 05:33 | Let's first make a 6 x 6 centre point slot at the top of the curve in the centre of the part using a sketch and extruded cut. |
| 05:43 | Now we can use the pattern on a path tool, selecting our new slotted hole as the feature and the edge of the arm as the path. |
| 05:52 | We'll change the orientation from identical to path direction so the slots rotate with the curve. |
| 05:59 | Then we can drag the arrow to change the direction and specify eight features to an extent of 350 mm which works well for our example. |
| 06:09 | Clicking OK to finish and we're done with our pedal weight reduction. |
| 06:13 | Before we finish up with this module, let's take a quick look at the mirror tool. |
| 06:17 | Just like with the pattern tool, we can also select faces, bodies, features or components to mirror, we just need to select a mirror plane to define the mirrored feature which could be a datum plane or a flat surface. |
| 06:31 | For example, looking back at our roll cage that we created in the earlier sweeps and piping module, we can use the mirror tool to mirror the body of the A pillar bar that we created through the right plane to get the A pillar bar for the other side of the vehicle. |
| 06:47 | As I mentioned earlier, this is particularly helpful on parts that have a lot of features that are symmetrical. |
| 06:53 | We can then just model half of the part and then use the mirror tool to save time. |
| 06:58 | Alternatively, if we already have a right hand version of a part and we wanted to create a left hand version of the same part, like a steering knuckle for example, we could simply mirror it and then delete the original version rather then modelling the entire part from scratch. |
| 07:15 | As always, take time to experiment with these three different pattern tools and the mirror tool to get familiar with them. |
| 07:21 | Change the objects you want to replicate, the axes direction or mirror planes defining the features as well as the preferences like the spacing and the tool window. |
