3D Modeling & CAD for Motorsport: Part Drawing Views
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Part Drawing Views
16.18
| 00:00 | - In the previous module, we covered the fundamental knowledge of technical drawings and how to get started setting up drawing templates in Fusion 360. |
| 00:08 | We can now apply this knowledge to produce technical drawings for parts from solid and sheet metal models as well as assemblies which we'll be covering in the next few lessons. |
| 00:18 | As we can imagine, part drawings can dive deep into all the details required to produce their subject. |
| 00:25 | These drawings will more than likely have a series of views to make sure the reader can fully understand the form of the part. |
| 00:32 | Consider parts that have the same profile through the entire depth and that depth is perpendicular to the profile plane. |
| 00:39 | For example, a sheet metal part that would be laser cut and doesn't feature any bends or forms. |
| 00:46 | A part of this nature would only require two views to fully illustrate its form and show all the dimensions. |
| 00:52 | One view would be the base view looking directly at the profile and the other view, a projected view from the side to show the thickness. |
| 01:01 | With that said, I still like to provide an isometric view as well just for reference and clarity. |
| 01:08 | Any 3D part beyond this with variation to the profile through its depth will require at least three standard views. |
| 01:16 | A base view and two standard projections. |
| 01:19 | For example, if the flat sheet metal part we just discussed was then formed with a bend, we now need another view to properly illustrate this. |
| 01:28 | Back in Fusion 360, let's open up the wheel hub model found in the suspension assembly that we were working with earlier and start working on making a drawing. |
| 01:38 | Under the file tab, click new drawing and then from design. |
| 01:43 | In our pop up window, leave the contents as full assembly as we only have one component here anyway and it's active and visible. |
| 01:51 | For drawing, leave it as create new. |
| 01:55 | But for the template we can browse and find the part drawing template we saved from the previous module with our place holder views to save some time. |
| 02:03 | Remember we can only use this template if it's in the same project folder as the design. |
| 02:08 | Once we hit OK we can see that our drawing views have been automatically set up from the placeholder views from the template. |
| 02:16 | Firstly let's just click and drag to move the isometric view to the top right corner so we can free up a bit more space. |
| 02:23 | In the standard view, the hub seems to be missing some detail. |
| 02:28 | The reason for this is a lot of the sharp edges have been rounded with a fillet tool, this results in a tangent edge at the transition between the rounded edge and the flat face. |
| 02:39 | This transition is seamless and therefore in a line drawing it's not shown. |
| 02:43 | If we double click our base view, we can see that the tangent edges are turned off so we can't see them. |
| 02:50 | Let's turn these on to full length, creating lines along the tangent edges and then click OK, notice this doesn't update the projected views. |
| 02:59 | A quirk here is that the appearance preferences in the projected views can be set to copy the style from the parent view but the edge visibility preferences cannot. |
| 03:09 | We could have set these preferences up when creating our template but whether we wanted to show them or not will depend on our model's geometry. |
| 03:17 | To change these as well, we need to click on them individually to make the same changes as I'm showing here with the top view. |
| 03:24 | Or if we deleted the right view and created another projected view from the base view, by clicking the projected view icon in our toolbar or press P on your keyboard, click the base view as the parent view for the new projection, then click to place the view where we want it. |
| 03:41 | If we press escape to cancel the tool now we can see that the new projected view now has the same preferences as the parent base view. |
| 03:49 | Note that the projected view tool allows us to create projected views from the parent view in the basic top, bottom, left and right directions, as defined by our model coordinate system. |
| 04:01 | The auxiliary view tool is very similar but also allows us to create projected views that align with the edges of the parent view. |
| 04:09 | Auxiliary views are still standard views, they just allow a little bit more flexibility if we want a projected view from a different direction. |
| 04:17 | Additional standard views may be needed to show details on different sides, it all depends on the part. |
| 04:23 | We need to use good judgement here to make sure everything about our part is understood while keeping the drawing clear and easy to read. |
| 04:31 | Hidden details like internal constructions buried inside parts for instance will obviously not be visible from our external views. |
| 04:40 | For example, the internal cavity of our wheel hub that houses the wheel bearings, grease and seals as it fits over the spindle on the suspension upright. |
| 04:50 | We can't clearly see any of this yet however if we double click our base view and change the appearances to show the hidden edges, we can now see the dotted lines illustrating the internal structure. |
| 05:03 | This is starting to look overcomplicated and not so easy to read so let's choose not to view the hidden lines. |
| 05:10 | With more complex parts there may be internal features that can't be illustrated clearly by any standard views. |
| 05:16 | You'll notice we have some other drawing view options in our toolbar so let's take a look at them now. |
| 05:22 | In this case, the best alternative is to use the section view. |
| 05:26 | We discussed the section analysis tool briefly in the analysis module. |
| 05:31 | The idea is the same, it creates a cutaway view of our model. |
| 05:35 | Firstly let's delete our right hand view again because we'll replace it with a section view. |
| 05:41 | Now we select the section view icon from the toolbar and then select the base view as the parent view. |
| 05:47 | Next we need to specify our section line through the part. |
| 05:51 | We can actually set a section line that is not a single straight line through the part but a chain of multiple straight lines. |
| 05:58 | Let's try that now for the purpose of this example. |
| 06:02 | Placing the start of the line directly above the part in the centre we then add a point in the centre and then project the line through the centre of the left hand bottom hole, clicking again to place the final point. |
| 06:15 | Notice that it's helpful to hover over the holes and then move the cursor to align with the points, then we can press enter to complete the line. |
| 06:24 | Now we can move the cursor to the side of the model and see our section view. |
| 06:28 | If we move the cursor to the other side of the section line you'll notice that the arrows change direction as these indicate which direction we're viewing the section from. |
| 06:38 | In this case, because our section line actually has two lines at an angle, we can move the part to align with either part of the section line. |
| 06:47 | If we press the shift key, it breaks alignment with the view, allowing us to place it elsewhere if we don't have space. |
| 06:54 | It's not quite as clear this way but because the section view is labelled to match the lines, it's still easy to understand. |
| 07:01 | Let's place the view where we had our right hand view before, directly in line to the right of our base view. |
| 07:07 | We have the same appearance and edge visibility options as before in our pop up window but we also have the section depth preference which as the name suggests, defines how deep our section is behind the cut surface. |
| 07:20 | Think about it as the thickness into the page. |
| 07:23 | The full setting has the entire remaining side of the part behind the section face, whereas slice essentially just shows the face of the section. |
| 07:32 | The distance setting on the other hand lets us define the depth. |
| 07:36 | Let's leave it as full and click OK. |
| 07:39 | The section view has parallel lines which are referred to as cross hatching to show the section surface. |
| 07:46 | That is the area of the part that has been cut through to make the view. |
| 07:50 | Double clicking these allows us to modify the spacing and angle if we need to make any changes for clarity. |
| 07:57 | As you can see, the resulting section clearly shows the internal cavity for the grease and wheel bearing a lot clearer than with the hidden lines method. |
| 08:06 | One last note on the section view is that the top half of the view is perpendicular to the top vertical part of the section line and the bottom half to the other part of the section line on an angle. |
| 08:18 | We can see this by how the bottom hole is shown in the cross section. |
| 08:22 | We wouldn't see this at all if our section line was one vertical line through the centre of the part. |
| 08:28 | This worked well for our example because it's really just the same section revolved about the central axis. |
| 08:34 | But this might not be the case for more irregular parts. |
| 08:37 | Again, what views we use and how we use them will depend on the part and how it can be illustrated in the clearest and most easily understood way. |
| 08:46 | The next view option available in the toolbar is the detailed view. |
| 08:50 | This is most helpful for complex features that are small, relative to the size of the part. |
| 08:56 | It really just allows us to create another zoomed in view on a section of another view. |
| 09:01 | Let's select the icon in the toolbar and choose the top view as the parent view. |
| 09:06 | Now we're going to make a circle that's going to define the limits of our detailed view. |
| 09:11 | We'll select a point on the parent view to place the centre and simply move the cursor to set the circle size. |
| 09:18 | Let's choose to highlight the back curved section to the step in the wheel hub before the wheel mounting flange. |
| 09:25 | Now we move the cursor to place the detailed view. |
| 09:29 | Since the default 1:1 scale isn't much bigger than the parent view, let's increase that to 3:1 and drag the view into clear space, maybe moving the view label as well, keeping it close to the detailed view so it's clear what it represents. |
| 09:44 | Now we have a larger view of a small detailed area, we can clearly see where that view is from on the parent part and we can use this down the track to add some dimensions. |
| 09:53 | The remaining view tool is a new one to Fusion 360, the break view. |
| 09:58 | This just shortens an existing view by removing a portion of the design. |
| 10:03 | This isn't really much use in the case of our wheel hub design so I'll quickly pull up a drawing for the dash bar of our roll cage that allows us to see how it works. |
| 10:13 | For reference, the dash bar connects the two A pillar bars and runs straight across the car under the dash. |
| 10:20 | Looking at this drawing, we have a base view and a projected view of the end of the bar as well as an isometric view. |
| 10:27 | The current scale is 1:10 which makes the end view very small and if we were to increase the scale, the base view would get too large for the sheet. |
| 10:36 | We could use a detailed view of the end view but since this is a long straight part that is mostly featureless through the middle section, using a break view of the base view is the best solution. |
| 10:48 | This will allow us to increase the scale of both standard views. |
| 10:51 | All we need to do is select the base view, choose the orientation of the break section, being horizontal in this case, and then place the start and end points for the portion to remove, which we can place pretty close to the ends here. |
| 11:07 | We'll leave the resulting gap between the break lines as the default of six and hit OK. |
| 11:13 | We can now see our base view has been shortened by removing the middle featureless portion and this is indicated by these break lines which we could double click at any time to edit the break view settings. |
| 11:25 | We can now scale the views up significantly to 1:1, making it much more clear and we can still give the total length dimension across the break, getting the full 1500 mm measurement. |
| 11:37 | OK so moving along our toolbar, the next tools under the modify section are move and rotate. |
| 11:42 | These are simple tools that help us reposition and rotate views if the default orientations aren't ideal. |
| 11:50 | Next we have the geometry section. |
| 11:52 | All of these tools add reference lines to our drawings to help describe the geometry of the part. |
| 11:58 | Centrelines for example are made up of long lines with shorter dashes in between and represent axes of circular features like shafts and holes as well as the centre axis of symmetry for symmetrical parts. |
| 12:10 | These can also be helpful when dimensioning the design as more points of reference. |
| 12:15 | Back to our wheel hub drawing, we can add some centrelines straight through the middle axis of our top and right views as the section for this part is revolved around these axes. |
| 12:26 | To do this we'll select the centreline tool, now we select two of the same points or edges on each side of the part that we're going to place the centreline directly between. |
| 12:36 | We'll choose the outermost edges of the flange for mounting the wheel for both views. |
| 12:41 | After selecting them, the centreline will be placed and we need to press escape to cancel the tool. |
| 12:47 | Then we want to click the line and drag the ends of the centreline to extend it through the entire part. |
| 12:53 | We could also use this to add centrelines to the holes on our section view. |
| 12:58 | For the front base view, let's add some centre marks to represent the points at the centre of the circular features. |
| 13:04 | All we need to do is click the centre mark tool and then select the outer edge of the part to get the reference lines. |
| 13:12 | Finally and ideal for a part like ours with a PCD hole pattern is the centre mark pattern tool. |
| 13:18 | This tool allows us to easily show the centre mark of each hole as well as the circle they lie on. |
| 13:25 | To create this reference line, we select the centre mark pattern tool and turn on the auto complete preference and then just select one of the holes. |
| 13:33 | Let's finish that by clicking OK. |
| 13:36 | Further to these centre lines and marks, under the geometry tool set, we can also extend edges if we wanted to dimension to an intersection of edges that wasn't shown on the part. |
| 13:48 | This can help for example if a part has two machined edges in one process and then the corner between them is rounded in another process. |
| 13:56 | This dimension is going to be useful for the first machining process. |
| 14:00 | In some cases, we may also want to sketch on our drawing to make some new lines that aren't already in the model and we can't create with the other tools. |
| 14:09 | It's not the most refined method but it's there just in case we need it. |
| 14:14 | One last thing to mention is that if we make changes to our design, they won't be automatically carried over to our drawing, just like we discussed with our assemblies, we're given a yellow exclamation mark over the chain icon at the top of our screen if something is out of date and we need to click it to bring the drawing up to date and make sure it's referencing the most recent version of the design. |
| 14:36 | Before we finish up with this topic, let's summarise this module on the different views in part drawings. |
| 14:41 | The minimum number of standard views required to illustrate our design clearly and completely define them is dependent on the model. |
| 14:49 | In some cases, for essentially 2D parts, we may be able to use only two standard views. |
| 14:56 | However more commonly we'll need three and I'd also recommend adding an isometric view to really help the reader visualise the part in the 3D context. |
| 15:07 | We can always add more views if needed as long as we try to keep things clear and avoid overcomplicating the drawing. |
| 15:14 | The appearance and edge visibility settings like tangent edges or hidden edges can be useful to help show the internal and external geometry of parts. |
| 15:23 | In cases where there are details or features that are small relative to the size of the part, the use of a detailed view may be required to create a zoomed in, scaled up view of a particular area. |
| 15:36 | In other cases, there may be hidden detail inside the design from internal constructions that cannot be illustrated clearly from the standard external views. |
| 15:46 | Here we need to use the section view to show a cutaway of the part and include the section lines and arrows on the parent view. |
| 15:54 | We can also add a range of different referencing features such as centrelines through our views that help describe the geometry of the part by showing the centrepoints and axes for circular features as well as axes of symmetry. |
| 16:07 | Just remember, the intent of the views and details is to illustrate our part in the most accurate and easily understood way possible. |
