Day 12 of Learn Autodesk Fusion 360 in 30 Days — Slotted Screwdriver

[00:00:00] Welcome to day number 12 of learn Fusion [00:00:02] in 30 days. Today, you'll create a [00:00:05] flathead screwdriver as you learn the [00:00:07] three-point arc command, circular [00:00:09] pattern, and more. [music] Let's get [00:00:11] started. [00:00:13] Start a new design file by choosing the [00:00:16] hybrid design intent and save your [00:00:18] design. Use hybrid because our [00:00:20] screwdriver contains one part for the [00:00:22] plastic handle and one part for the [00:00:24] metal shank. [00:00:26] Create a new component for each part. [00:00:29] Activate new component from the toolbar. [00:00:32] Set the type to part as this represents [00:00:35] a single manufacturable object. Stick [00:00:38] with a standard component and ensure you [00:00:40] uncheck external. This creates an [00:00:44] internal component that lives only [00:00:46] inside this hybrid design file. Name [00:00:49] this first component handle and click [00:00:51] okay. [00:00:52] This handle component serves as a [00:00:54] container for everything related to the [00:00:56] handle part. [00:00:59] Press space bar to repeat new component [00:01:01] and set this one to the part type as [00:01:03] well. Name it shank. [00:01:07] Before you click okay, clear out the [00:01:09] parent selector. Select the top-level or [00:01:13] root component to ensure both components [00:01:15] are nested at the same hierarchical [00:01:17] level in the browser. [00:01:20] Very important, remember to keep a close [00:01:23] eye on which component you have active [00:01:25] in the browser. [00:01:27] The radio button icon next to the [00:01:29] component name indicates the active one. [00:01:32] Hover over the handle component and [00:01:34] click the radio button to activate it. [00:01:37] Press C for circle and select the XY [00:01:40] origin plane to sketch the handle as if [00:01:42] it were lying on a table. Start at the [00:01:45] center origin and define the diameter as [00:01:47] 28 mm before pressing enter. [00:01:51] Press E to activate extrude. Define the [00:01:55] length of the handle as 100 mm. [00:01:59] Click OK to save the extrude. [00:02:02] To create the grip cutouts, start a new [00:02:04] sketch on the backside of the cylinder. [00:02:07] Rotate your model, right-click on the [00:02:09] back face, and select create sketch. [00:02:13] Activate the circle tool again. [00:02:16] Start the center circle anywhere on the [00:02:18] edge of the existing cylinder. This [00:02:20] automatically applies a coincident [00:02:23] constraint. [00:02:24] Define the diameter as 6 mm and press [00:02:27] enter. [00:02:28] Notice the circle stays constrained to [00:02:30] the edge of the existing circle. [00:02:33] Click out in space to clear any [00:02:35] selections. [00:02:37] Activate the horizontal constraint. [00:02:39] Select the origin and the center of the [00:02:42] circle. [00:02:43] This forces it to remain in position and [00:02:45] fully defines the sketch. [00:02:48] Let's cut half of the circle out of the [00:02:50] existing cylinder. [00:02:52] Press E to activate extrude and select [00:02:54] the right half of the circle. [00:02:57] Drag the blue directional arrow into the [00:02:59] existing 3D body to cut away material. [00:03:03] Define the distance as -75 [00:03:06] mm and click OK. [00:03:08] This represents the first groove on the [00:03:11] handle. [00:03:12] As a best practice, keep your sketches [00:03:14] simple and manageable. Pattern the [00:03:16] feature instead of sketching five more [00:03:19] circles. [00:03:20] Activate the rectangular pattern tool in [00:03:23] the toolbar [00:03:24] and switch to the circular type. Very [00:03:27] important, be sure to activate the solid [00:03:30] pattern tool and not the sketch pattern [00:03:32] tool. [00:03:33] Set the object type to features. [00:03:36] This allows you to select the extrude in [00:03:38] the parametric timeline as the object to [00:03:41] pattern. [00:03:42] Switch to the axis selector. [00:03:44] Because you started the handle from the [00:03:46] center origin, you can leverage the [00:03:48] center Y axis that runs through the [00:03:51] cylinder. [00:03:52] Very important, our handle component [00:03:54] includes its own origin. Toggle open the [00:03:58] origin folder and select the correct Y [00:04:00] axis nested in this part. [00:04:03] This ensures the part never loses [00:04:05] reference. [00:04:07] Leave the distribution set to full and [00:04:09] define the quantity as six. [00:04:12] Change the compute type to optimize to [00:04:14] ensure the fastest processing and click [00:04:17] okay to save it. [00:04:19] Before we round over the sharp edges, [00:04:21] add the thumb rest on the front of the [00:04:23] handle. [00:04:24] The YZ origin plane splits the handle [00:04:27] down the middle. Right click on the YZ [00:04:29] plane in the browser and select create [00:04:32] sketch. [00:04:33] This allows you to sketch the side [00:04:34] profile and revolve it around the center [00:04:37] axis later. [00:04:39] To sketch the three-point arc at the top [00:04:41] edge, use the intersect command first to [00:04:44] reference the existing edge. [00:04:46] Activate the intersect tool. [00:04:50] Select the 3D body. [00:04:52] Ensure you check projection link and [00:04:54] click okay. [00:04:56] Remember, this creates purple geometry [00:04:59] where our active sketch intersects the [00:05:01] existing 3D body. This edge will [00:05:04] automatically adapt if you change the [00:05:06] size of the handle. [00:05:08] Activate the three-point arc command [00:05:10] from the create menu within the arc [00:05:12] flyout menu. [00:05:14] The three-point arc requires you to [00:05:16] define the starting point, the end [00:05:18] point, and the radius of the arc. [00:05:21] Click to place the starting point [00:05:23] anywhere on the projected line. [00:05:26] And click again to place the end point. [00:05:29] Click a third time to place the radius. [00:05:32] Let's now activate the sketch dimension [00:05:34] tool to dimension the arc. Select the [00:05:37] corner projected edge and then the start [00:05:39] of the arc. [00:05:41] Click to place the dimension and define [00:05:43] it as 3 mm. [00:05:46] With the dimension tool still active, [00:05:48] select the arc and define the radius as [00:05:50] 13 mm. [00:05:53] Notice the sketch is not yet fully [00:05:55] defined as the center point can still [00:05:57] move freely. [00:05:58] Add a final dimension between the corner [00:06:01] projected edge and the center point. [00:06:04] Click to place the dimension to the left [00:06:06] and define it as 9 mm. [00:06:10] This fully defines the sketch and [00:06:11] prevents the arc from moving. [00:06:15] Activate the revolve tool from the solid [00:06:17] tab. [00:06:19] Revolve automatically selects the single [00:06:21] sketch profile. [00:06:23] For the access, select the Y axis nested [00:06:26] inside the handle component as this runs [00:06:30] directly down the center of the handle. [00:06:32] The operation defaults to cut since it [00:06:35] detects the 3D body. [00:06:37] Click okay to save it. [00:06:40] Throughout the design process, you will [00:06:42] often want to alter dimensions. [00:06:44] Intentionally built parametric designs [00:06:46] allow you to simply edit sketches or [00:06:49] features to change the dimensions [00:06:51] without breaking the design. [00:06:54] Double-click the third sketch in the [00:06:55] timeline and double-click the radius [00:06:58] dimension to edit it. [00:07:00] Change this to 14 mm and press enter. [00:07:05] Double-click the 9 mm dimension and [00:07:07] change it to 11 mm. This makes the thumb [00:07:11] rest more shallow. [00:07:13] Once complete, select finish sketch to [00:07:15] exit the sketch. [00:07:18] It's a best practice to keep fillets at [00:07:20] the end of your timeline. This optimizes [00:07:23] processing performance and prevents lost [00:07:26] references or broken geometry that can [00:07:28] occur at the edges. [00:07:30] Let's first add the cutout for the [00:07:32] shank. [00:07:33] Press C to activate circle and select [00:07:36] the front face of the handle to start [00:07:38] the sketch. [00:07:39] Start at the center origin and define [00:07:41] the circle as 7 mm before pressing [00:07:44] enter. [00:07:46] Press E to activate extrude and extrude [00:07:49] this to a depth of -50 mm. [00:07:52] The minus symbol ensures this cuts into [00:07:55] the handle 3D body. [00:07:57] Before proceeding, take a minute to [00:07:59] rename your sketches in the browser. [00:08:01] Click once to select a sketch and a [00:08:04] second time to edit the name. Make the [00:08:07] names descriptive of the task or design [00:08:09] feature. This best practice pays [00:08:11] dividends when you reopen old files or [00:08:14] continue to work on multi-part designs. [00:08:19] Now, activate the fillet command to [00:08:22] round the sharp edges. [00:08:24] Select the two edges of our thumb rest [00:08:26] and define this as 5 mm. [00:08:30] Add a new selection set and select the [00:08:32] front edge. [00:08:34] Define this as 1 and 1/2 mm. [00:08:39] Add a third selection set and select the [00:08:41] back six edges of the handle. [00:08:47] Once selected, define this radius as 10 [00:08:50] mm to create a large rounded end. [00:08:54] Click okay to save these fillets. [00:08:57] Here's a pro tip. When applying many [00:08:59] different fillet radii, break them into [00:09:01] two separate fillet commands. This often [00:09:04] helps the fillets compute better and [00:09:06] makes them more manageable. [00:09:09] Activate fillet again. [00:09:11] In this case, you can select the long [00:09:13] edges in a single click since the [00:09:15] previous fillet connects the edges. [00:09:18] Select all six long edges and define the [00:09:20] radius as 2 mm. [00:09:27] Add a new selection set and select the [00:09:29] arc and short outer edge. [00:09:32] Repeat this for the remaining five [00:09:34] cutouts. [00:09:39] >> Define this fillet radius as 1 mm and [00:09:42] click okay. [00:09:44] This completes the handle. [00:09:48] Click home to reset the view. [00:09:51] Very important, remember to activate the [00:09:54] shank component before creating the [00:09:56] shank. This ensures the sketches and [00:09:58] bodies nest inside the correct part. [00:10:01] You can also close the origin and [00:10:03] sketches folder of the handle component. [00:10:07] Don't forget on day 11 you turned off [00:10:10] active component visibility, so each [00:10:12] component remains opaque. [00:10:15] To create the shank, you could [00:10:17] technically extrude the existing face of [00:10:19] the circle. However, if you reference a [00:10:22] face directly and then significantly [00:10:24] modify or delete the original geometry, [00:10:28] the dependent feature often loses its [00:10:30] anchor. This results in errors and [00:10:33] broken links in your timeline. [00:10:36] View the model from the front position [00:10:38] to right click on the circular face and [00:10:40] select create sketch. [00:10:43] Activate the intersect tool. [00:10:46] Once active, select the inside circular [00:10:48] face and click okay. [00:10:50] This ensures the geometry of our shank [00:10:53] always matches the handle cutout. [00:10:56] Activate extrude and define the distance [00:10:59] as 150 mm. [00:11:03] As a best practice, always test your [00:11:05] parametric designs as you go. [00:11:08] Activate the handle component and edit [00:11:10] the fourth sketch, which contains the [00:11:12] shank cutout. Double click the [00:11:15] dimensions to edit and enter a new [00:11:17] value. [00:11:19] When you select finish sketch, the shank [00:11:21] automatically adapts in size. [00:11:24] Again, you could achieve this by [00:11:26] extruding that face. However, the [00:11:28] intersect command builds in more [00:11:30] intelligence and ensures you never lose [00:11:33] the reference. [00:11:35] Press undo until you return to the 7-mm [00:11:38] diameter. [00:11:40] Let's finish the design with the [00:11:42] screwdriver tip. [00:11:43] Create a new component for the tip, [00:11:45] which allows you to reuse the handle and [00:11:47] shank for different designs. [00:11:50] Here's a pro tip. Right click on the top [00:11:52] level or root component and select new [00:11:55] component. This method remains the [00:11:57] preferred choice as it automatically [00:11:59] selects the root component as the [00:12:01] parent, saving you a few seconds each [00:12:04] time. [00:12:05] Set this one to the part type as well. [00:12:08] Name this component tip and click okay. [00:12:14] Double-check that the tip component is [00:12:16] active in the browser. [00:12:18] This time, reference the existing face [00:12:20] to create the 3D body without a sketch. [00:12:24] Press E for extrude and select the end [00:12:26] of the shank. [00:12:27] Define the distance as 10 mm. [00:12:32] The downside is that you only have an [00:12:34] extrude in your timeline without a [00:12:36] sketch to alter. However, this works [00:12:39] fine for simple use cases. [00:12:42] Toggle open the origin folder for the [00:12:44] tip component. [00:12:46] Right click the YZ plane as it runs down [00:12:48] the middle and select create sketch. [00:12:52] Again, use the intersect tool to [00:12:55] reference the existing edges. [00:13:01] Activate the three-point arc tool. [00:13:06] Start the first point near the front [00:13:08] edge. [00:13:09] For the second point, click where it [00:13:11] snaps to the top purple edge. [00:13:14] Click anywhere to place the third point. [00:13:17] The first end point can still move [00:13:19] freely. [00:13:20] Activate the vertical constraint and [00:13:22] select the end point and the top edge. [00:13:26] This forces it to remain on the front [00:13:28] edge. [00:13:30] Activate sketch dimension. [00:13:32] Select the center point and the first [00:13:34] end point of the arc. [00:13:36] Click to place the dimension and define [00:13:39] it as 0.5 mm. [00:13:42] Add a dimension between the corner edge [00:13:44] and the second point of the arc. Define [00:13:47] this as 9 mm. [00:13:51] Lastly, add an 18 mm radius dimension to [00:13:54] the arc. [00:13:57] If you hide the tip body, you will see [00:13:59] that you need to fully close the sketch [00:14:01] profile. [00:14:03] Activate line and sketch a line between [00:14:06] the corner edge and the start of the [00:14:08] arc. [00:14:10] Press E for the extrude command and turn [00:14:12] the 3D body back on. [00:14:15] Since you sketched in the exact middle, [00:14:18] change the direction to symmetric. [00:14:21] Let's build intelligence into the model [00:14:23] in case the shank and tip diameter [00:14:25] change. Update the extent type to all. [00:14:29] This ensures the tool always cuts all [00:14:31] the way through the existing 3D body. [00:14:34] Click okay to save the extrude. [00:14:38] Let's now mirror this to the other side. [00:14:41] Activate the solid mirror tool. [00:14:45] Use the features object type and select [00:14:47] the extrude in the timeline. [00:14:52] Switch to the mirror plane selector and [00:14:54] select the XY origin plane inside the [00:14:57] tip component. [00:14:59] Once again, use the optimize option for [00:15:02] the fastest performance and click okay. [00:15:06] The screwdriver model offers a fun [00:15:08] opportunity to experiment with [00:15:10] appearances. Have fun trying different [00:15:13] plastic appearances on the handle and [00:15:15] remember you can apply appearances to [00:15:17] individual faces. [00:15:20] Great job completing the screwdriver. [00:15:23] I'll see you on day number 13 where [00:15:25] you'll take a close look at why fully [00:15:28] defining your sketches is so important. [00:15:37] >> [music]