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3D Modeling & CAD for Motorsport: Drawings Notes and Other Specifications

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Drawings Notes and Other Specifications


00:00 - Sometimes after we've dimensioned our designs we still need to add some extra information for completeness or clarity's sake.
00:07 This is where notes come into play as they give information that can't be represented in pictorial views or by dimensions.
00:16 These notes are useful for communicating additional design intent to help explain the fit, form and function.
00:23 There are various types available to use in Fusion 360 like unattached notes which as the name suggests, aren't attached to any feature and are essentially just floating text positioned on the drawing.
00:35 We simply need to use the text tool to create these.
00:38 Leader notes on the other hand, are attached to a feature via a leader which is just a line with a dot or an arrow.
00:46 These are commonly used for hole and thread notes as well as bend notes.
00:51 Our note tool works similar to the dimension tool, automatically creating a particular note type depending on the feature we select attached to the leader.
01:00 If the resulting note type isn't what we need, then we can cancel and use one of the specific note tools that suits.
01:08 Let's fire up our hub design again and take these note tools for a spin.
01:11 Looking back at our PCD dimensions on the hub with both these diameters shown and the top hole sitting on the centreline, we actually have enough information for these parts to be machined.
01:22 However we may want to add a note for clarity.
01:26 Depending on the text we want to add, we could double click on the hole size dimension, press shift and enter to create another text line and add our text.
01:35 In this case, a hole specific note might be more effective than our current hole dimension.
01:41 Let's select the note tool and select one of the five holes.
01:45 We get an automatic hole note saying five times holes with 12 mm diameter.
01:51 Let's add to this with the text equally spaced on 100 mm PCD.
01:56 Unfortunately we can't add a non symmetrical tolerance to this note so we'd need to leave the original tolerance dimension for the hole as is.
02:04 Obviously we don't have any bends on this part to add bend notes so let's have a quick look at a drawing for a simple sheet metal part that's been made on a sheet metal specific drawing template, you'll find this file available for download below if you want to follow along.
02:20 On the second sheet we have the flat pattern which shows our bend lines.
02:24 If we select the note tool again and then click the dashed bend line, we get the bend note which tells us the bend direction, being up in this case, the bend angle, being 90° and the bend radius of 2.5 mm.
02:39 We also need to dimension this bend from the edge of the part to completely define the feature.
02:45 After we've added a note and dimension to the other bend line as well, it's good practice to add a bend table as the design has multiple bends.
02:53 This is done by just selecting bend table under the tables tab here and positioning it on our sheet.
03:01 This basically just captures the same details as the notes but the important addition is the bend ID number.
03:08 This number is also added to the view on the drawing but unfortunately in this case, is in the same position as the bend note so we just need to move that for clarity.
03:17 The big advantage of this ID number is that we're able to individually identify bends of the same radius, angle and direction.
03:25 Also, to help us define the order the bends should be formed in, when that's critical to the part being made successfully, as we discuss in our sheet metal modelling lessons.
03:36 Moving on, in some cases there may be a feature that's not too critical to your intent but seems to be missing information as we aren't familiar with the manufacturing process.
03:46 For example, punched text into sheet metal part for identification.
03:51 It may be worth adding a note here that simply says, manufacturer to determine, as they will have a better understanding of what's suitable.
04:00 Next we have weld notes.
04:03 While these are most common on assembly drawings where different components are welded together, they can also be used on part drawings with sheet metal parts that require welding between the flanges of the same part.
04:14 Like on our sheet metal drawing for example.
04:17 Looking back at sheet one now, let's add a weld note instructing the manufacturer to weld these two flanges together.
04:24 First we select the welding tool from the symbol section of the toolbar, then we need to click the edge we want to attach the leader for the note to.
04:32 Which we'll do on our isometric view because the edges to be welded are best shown in this view.
04:37 After selecting the edge, we can click again on the screen where we want the note to be positioned.
04:43 This generates the leader, then we hit enter to place the note.
04:47 Now we can see that we get a pop up window with preferences for our weld note.
04:52 For our simple example, we'll leave the weld type as fillet and the size at 3 mm.
04:57 There's a fair amount of additional symbols and preferences to choose from here to cover all kinds of welds.
05:04 As you might have guessed, you're going to need a decent understanding of the welding process to create weld notes that are useful and to also understand what weld symbols represent what types of welds.
05:15 If you want to learn more about the art of welding, I highly recommend checking out some of High Performance Academy's motorsport fabrication courses.
05:23 OK let's move on and discuss material specifications.
05:27 The intended material for a design always needs to be specified on our drawings.
05:32 This can be noted in the title block but often the material information we want to include won't fit here clearly so we'd simply note something like, see material spec table and then of course create this table.
05:46 The material specs should really be shown on the drawing for each part, therefore on an assembly drawing, we could add a note saying refer to parts in the title block.
05:56 As with dimensions, defining the material needs to be clear with enough information to fully understand the spec and stopping short of adding too much info that it's just not necessary.
06:07 I'd recommend simply including the name of the material and maybe a short description and it can also be helpful to include the grade and potentially the strength specs like yield and tensile strength, if we have access to them.
06:21 Creating a table is relatively simple, just select the empty table icon from the table section in our toolbar.
06:28 Drop it onto the sheet where we want it and then we can move it, add and delete rows and columns, drag them to change the width and height and enter all the necessary information.
06:39 To sum up what we've just covered, there are going to be some cases where the information we're trying to communicate can't be clearly shown on our views or dimensions.
06:48 In these cases we'd use notes and these come in a wide variety.
06:52 This could mean just adding some extra text to a dimension but most commonly we'll be using attached notes on leaders pointing to a specific feature.
07:02 Weld notes, bend notes and hole and thread notes are some standard note types that are used often and have their own dedicated tools in the Fusion 360 drawing toolbar.
07:12 With some knowledge of the manufacturing process, we can use these to define features clearly.
07:18 Further to this we always want to clearly define the intended material specifications.
07:23 This can be captured simply in the title block but in cases where we can add a bit more detail, the material spec would ideally be captured in a dedicated table on the drawing.
07:34 With some knowledge of the manufacturing process we can use these to define features clearly.
07:39 Further to this, we always want to clearly define the intended material specifications.
07:45 This can be captured simply in the title block but in cases where we can add a bit more detail, the material spec would ideally be captured in a dedicated table on the drawing.

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