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3D Modeling & CAD for Motorsport: Step 2 - Modelling

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Step 2 - Modelling


00:00 - Now it's time for the core phase of our CAD work, the design and modelling process.
00:05 Because we've already created a model of the battery and measurements of where it'll be mounted, these can be used as the key references that we'll build our model around.
00:15 I want to quickly note that for some applications at this stage, we may be able to use generative design or automated modelling functions to develop our design and guide our design process.
00:27 This application in particular isn't really well suited for either of these and it's relatively simple anyway so let's use it as practice for good old fashioned CAD modelling.
00:39 Naturally, since we intend to use aluminium sheet metal to make our design, we'll be modelling using the tools under the sheet metal toolbar and working with sheet metal bodies.
00:50 This will also involve using sheet metal rules with our material set to aluminium.
00:55 We have some reference features already but we can create additional datum planes that are going to help as well.
01:02 As we discussed in the previous module, we'll leave a small gap around the battery that'll be filled with 2 mm thick foam tape to help keep it snug in the box and minimise vibrations and rattles.
01:16 Let's start by creating an offset plane 2 mm above the top face of the battery.
01:21 We'll use this soon when modelling the top of the box, for now though we'll start by modelling the base.
01:28 For each part of the battery box, we use a separate internal component, that way our model will be better organised and it'll also help with creating drawings in the future.
01:39 So let's first create a new internal component using the sheet metal type and naming it battery box base.
01:47 Let's make sure the activate preference is selected so the new component will be activated when created and we can get straight into modelling it.
01:56 Lastly we'll use the aluminium sheet metal rules.
01:59 Now we need to quickly check our default sheet metal thickness by clicking the sheet metal rules icon in the toolbar and expanding the aluminium rule in this design.
02:09 Making sure it's set to 2 mm.
02:12 If not, we can just edit the rule and change it.
02:15 With that setup out of the way, the first step for modelling is to create a sketch on the top plane.
02:22 A simple rectangle using the co linear constraint to make the top and bottom edge line up with the top and bottom of the battery's case.
02:30 For the width, we'll just make it 10 mm wider than the centre of the mounting points on each side and round the corners with the fillet tool using a 10 mm radius.
02:40 If we set the line type to construction and use the project/include tool to include the circles from the mount point sketch, after changing the line type back to non construction we can now use the offset tool to create new circles 0.5 mm offset to these which means they will be 1 mm larger in diameter.
03:03 This allows us to create 7 mm clearance holes for our M6 hardware.
03:08 The sketch should now be fully defined with all the lines in black.
03:13 From here, under our sheet metal toolbar we can use the flange tool to create our first sheet metal body rather than using the extrude tool to create a solid body and then having to convert it.
03:25 All we do is select the flange tool and then select our sketch profile.
03:30 Setting the orientation to side one so the thickness is added above the sketch plane towards the side of the battery.
03:38 Still leaving a 2 mm gap for our foam.
03:41 After clicking OK to finish the flange tool we now have a main body for the base of the box.
03:48 We'll leave this as is for now and move onto modelling the top section of the box, but we'll come back to the base soon.
03:56 Following a similar process we can now make a new internal sheet metal component naming it battery box top and then sketch a rectangle on the offset plane we created earlier.
04:07 Again, we use the co linear constraint and line up the top and bottom edge with the side of the battery case.
04:15 Let's also do this with the sides as well.
04:18 We also want to add another rectangle centred on the top of the first one with the top edge in line with the top of the battery cover and the sides in line with the edges of the cut outs.
04:30 We'll soon be using this with a flange that wraps around the top of the battery between the terminals to support it.
04:37 We don't need to round any of the corners yet as we'll use the modification tools for this soon.
04:43 The next step is creating flanges from the edges of the existing sheet metal bodies, rather than sketches as we've just done.
04:51 So keeping the top of the box activated for now, let's select the flange tool and then select the bottom edge on each side.
04:59 We'll keep the bend angle at the default of 90° and pulling the flanges down with the arrow until they just touch the base of the box or setting the height to 82 mm.
05:11 We also want the bend position to be adjacent so we get our 2 mm gap down each side of the battery and then select OK.
05:20 Next is the tabs that will extend outwards to the mounting points which we can also make using the flange tool by selecting the outer bottom edge of each of the previous side flanges.
05:33 This time, with the height set to 32 mm and the bend position preference set to inside so the tabs lay flat on the base of the box and extend out to meet the sides.
05:46 These tabs obviously need holes for mounting which we can make using an extruded cut from the circular profiles of our box base sketch.
05:55 Let's also make a 32 mm long flange downwards from the top cover of the battery as this meets the edges of the recesses of the terminals.
06:05 This time though, the bend position needs to be set to adjacent again to give our 2 mm gap for the foam.
06:14 To finish the top cover, we'll use the fillet tool from the modify tab to radius the external corners to 10 mm and the internal corners to 5 mm.
06:24 Coming back to the base of the box, making sure that the component is activated, let's create a flange that extends up the back of the battery 30 mm with the bend position as adjacent again.
06:38 However, this time we'll change the extent setting from full edge to symmetric and set the distance of 90 mm.
06:48 Meaning the flange will only come along the width of the battery and doesn't extend any wider.
06:54 Having this flange along the edge of an otherwise flat sheet metal part will add a lot of stiffness to the base and of course support the battery in this direction.
07:05 Having this feature on the base means it's very simple to bend, as opposed to having this on the top of the box which already has a range of other flanges.
07:15 Adding this extra flange here may cause issues.
07:19 This is the first form we've created so far that requires a bend relief to prevent the part from deforming or splitting when bent.
07:28 A default relief set by our sheet metal rules are these small straight cut outs here but let's choose to override the bend relief rules and change these to round so they look a bit nicer and aren't stress concentrators when the battery is forced against the flange.
07:45 After clicking OK, we'll radius the external corners of the flange by 5 mm using the fillet tool.
07:52 Finally let's add some 10 mm spacers under each mounting point as we discussed in the previous planning module.
08:00 This is going to make sure the base of the box clears the irregular shaped floor pan.
08:05 These don't need to be their own components since they aren't really important and you'll likely not need them for your application.
08:13 They're just here to serve as a reminder for our particular Honda City application.
08:19 If you're thinking the sheet metal parts look a bit bland, this won't be their final form and we'll add a few more details in the next module when we analyse the design.
08:29 Just before we finish up this stage, since we're going to be laser cutting the part I'll add the High Performance Academy logo to the top face which can be etched into the final part.
08:40 You can do the same at this point with your own logo or of course use a sticker or just not brand the design at all.
08:47 Since I have a DXF version of the HPA logo I want to use, the process is as simple as using the insert DXF function under the insert tab.
08:57 From here, we just select the plane we want to add it to, being the top face of the battery box and then locate the DXF file on our computer.
09:07 Leaving the insert mode as single sketch, we naturally get a sketch of the logo which we can edit and use the move tools to reposition it to where we want and then use the extrude tool to make a very shallow cut into the face of the part.
09:22 I've used 0.1 mm as the cut distance here but it's not important.
09:28 We'll address this with our technical drawing in a coming module.

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