Use scripts to create gears

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Use scripts to create gears.

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In this video, we'll use a python script and we'll use Align.

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In Fusion 360, we want to carry on with our gear reduction housing assembly.

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I’m going to get started by hiding the housing mount.

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And I also want to hide the front cover.

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From here we're going to be creating the gears by using something called a script.

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A script is a program that can be run in Fusion 360 that allows us to make use of some advanced functionality,

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to create complex geometry or even perform simple repetition.

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To do this, we're going to move on to the Tools menu and look for the Add-Ins section.

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This will have something called Scripts and Add-Ins but note there's a shortcut key Shift S.

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Once we select Scripts and Add-Ins, there's a section called Sample Scripts in the Script section.

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Also note there's a tab for Add-Ins that has a couple other things in it as well, such as the sample add-in for the spur gear.

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This can be found in both places for the spur gear script in the script section or in the add-ins section.

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What we're going to be doing is selecting the one that has the blue and yellow icon next to it, which means that this was created using python.

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The other spur gear script is created using C++.

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Now the functionality is the same but we're going to be exploring the python version.

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Note that we can create and edit these directly inside of Fusion 360.

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So if you have programming knowledge and you have access to the list of open API functions,

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you can create your own scripts and Add-Inns for Fusion 360.

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That's a bit outside of what we're looking at here.

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So right now we're going to focus on the functionality of just running an existing script.

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Once you've selected spur gear, let's select Run.

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Notice that it pops up a dialogue box similar to all of the other tools in Fusion 360.

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We have a graphic at the top that tells us hole diameter,

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root fillet radius and pitch diameter as well as the module being the pitch diameter over the number of teeth.

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We can modify some of these values, such as the units, in this case, metric, the pressure angle, the module, the number of teeth and so on.

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Remember that we have our spec sheet that's going to determine some of these values.

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We're going to be using a module of 2.

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For this first gear, we're going to create our 48 tooth drive gear.

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Our backlash value in this case is going to be 0.1 mm.

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Our root fillet value is going to be 0.5.

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But let's also note that some of these values can use our parameters.

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So for example, as we start to type in a value, you'll notice that as we go through here, we have our gear module and our gear thickness values.

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Not all of the values can use those parameters but some of them can.

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For our root fillet, we're going to set it to 0.5 mm, our gear thickness value, we can start to type in gear and select gear thickness,

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noting that it is linking to that parameter.

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And then the hole diameter in the center.

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We can start to type in gear,

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and then as we go through here, you can see that we have idle gear diameter and we have our drive and driven gear diameters.

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So in this case, we're going to be using our drive gear,

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and notice it's telling us that the center is too large and that's because the drive gear diameter was actually our 96 mm.

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So in this case, let's simply enter the value of 12 mm for that internal hole and then we'll say, OK.

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Notice that the new component is created called spur gear 48 teeth and by default it's created on the top or the XY plane.

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Also note that there is a sketch in here that's showing the pitch diameter.

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If we want to modify this, we can expand it and expand the Sketches folder and we can hide Sketch 3.

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We're going to worry about moving this into place in just a little bit, but let's carry on creating more gears that we can use.

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So let's carry on and rerun our spur gear script, noting that it remembered our backlash, root fillet, gear thickness and hole diameter values.

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So in this case, we simply need to switch the number of teeth.

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We'll say OK, and it creates a new gear with 16 teeth.

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We're going to run this one more time.

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And once again it's going to remember those values so we just need to make sure that we set it to 10 teeth.

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Remember that some of these gears will use a different inside diameter, but all of them can be modified later if needed.

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Now that we have each of these as components, they're free to move about because they have their own coordinate systems.

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While it's not strictly necessary that we move them around to different positions,

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I am going to move them around and capture their position which will just temporarily get them out of the way.

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Again, this is not necessarily a step that we have to follow, but it does help us in order to visualize things a little bit better.

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The next thing that I want to do is I want to hide the back housing.

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I'm going to use just the front housing to align everything.

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And to do this, I also want to temporarily lock the front housing in place so I'm going to right click and ground it.

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By grounding the front housing, what I'm telling Fusion 360 is that,

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the coordinate system associated with this is fixed in space relative to the origin at the top level.

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From here I'm going to move back to my solid tool set, and I want to begin moving these gears into their correct position.

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To do this, I can use Move/Copy or I can use another tool called Align.

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Align is extremely helpful because it has some additional functionality.

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First we want to make sure that we are moving components.

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If we move bodies, they will get to the correct place but the coordinate system for each of those bodies will remain in its current position.

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So I want to make sure that we're moving the entire component.

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For this, as I hover over the back face of this gear, there are a lot of different positions that we can select.

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With Align we can actually select just the face,

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or we can hold down the control or command key which will lock the focus and allow us to select various positions.

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I'm going to navigate to the center point of this gear and I'm going to left click on that position.

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So this is where we're moving from.

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I'm going to rotate my design around and I'm going to hover over the back face of this housing.

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I'm going to hold down the control or command key, then I'm going to select this position and that's where we're moving to.

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I want to flip this because I need to make sure that the gear is on the proper side.

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Then I'm going to capture its position and say OK.

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Now we want to repeat that process by using our right click marking menu and selecting Repeat Align.

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This time, I'm going to hover over the smaller gear, go to the center position,

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then I'm gonna move it again, holding down the control or command key to the center position there and flipping if needed.

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We'll capture its position and we'll say, OK.

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Lastly I need to move the idle gear, so once again right click, Repeat Align.

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And I'm going to select the center position of the shaft and then again, I'll hold down control or command.

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And if we need to, we'll flip it to the proper side and we'll select Capture Position.

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At this point in time, the gears are overlapping, but that's okay because we haven't added any joints, they're still actually free to move about.

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Once we move them, we want to revert their position, make sure that they are going back to that original location.

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We're going to deal with getting them into the correct position and rotating them around.

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But let's go ahead and expand each of these and hide Sketch 3 as we don't really need to see that sketch.

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At this point you'll notice that we haven't created all of the idler gears.

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We have an identical idler gear that has 10 teeth on it and then we have one that we need to modify that will be a little bit longer.

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We're going to deal with those in a future video,

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because those are going to be copied components and we're going to talk about Copy and Paste functionality.

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But at this point, let's navigate back to a home position.

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Let's make sure that we save this before we move on.