Link parameters and dimensions

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Link parameters and dimensions.

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In this video, we’ll link model and user parameters in the parameters dialog.

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We’ll link user parameters to a sketch dimension.

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And we’ll identify a fully defined sketch icon.

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

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If we had any difficulty, you can also go in and upload the supplied data set, gear reduction housing V2.

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This should contain all of the user parameters that were created based on our spec sheet.

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You can see here that this also includes our mounting bolts, idle gear shaft, mounting bolt flange as well as our gear clearance value.

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To get started, we want to begin by creating a new sketch and we're going to be selecting the XY or the front plane.

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We're going to begin by using our center diameter circle.

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I'm going to draw a large center diameter circle and you'll notice that the dimension box is currently highlighted in blue.

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If I begin to type in a value, I can enter for example G or I can enter the letter D.

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And it brings up all of the various user parameters that we created.

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You will note that it doesn't show the actual value of these, but it does show whether or not it has a value or if it's unitless.

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So in this case, we're going to be creating our drive and our driven gear both at the center or the origin.

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So I'm going to start with the drive gear and then I can left click to place it.

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This will allow me to stay on my circles tool, I can draw a second one and I can hit the letter D.

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And this time I'm going to be using my driven,

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and again, I can left click to place that value and then I want to begin drawing a few additional circles inside of here.

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These are going to be my idle gear diameter.

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Going to draw another one inside of here.

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And if you forget to place that dimension, that's okay.

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We can always go back and add it.

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This outside one here and then I'll hit Escape to get off my circle tool.

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If we need to go back and place a dimension, we can use the dimension tool, select and then as it's asking for our input,

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we can hit that I on the keyboard and have it automatically linked to that idle gear diameter.

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The next thing that we want to do is we want to apply a few constraints.

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I'm going to begin by using horizontal, vertical, this is between my origin and the external idle gear.

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Next I want to go to my tangent constraint and I'm going to make all of the idle gears and the gears on the inside tangent.

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You'll notice that when I do this, I'm going to have to make sure that I hit Escape on the keyboard to get off my constraint tool,

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and make sure that things can still move around.

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Once they are able to move around, I'm going to go back left click to make sure nothing selected,

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go back to my tangent tool and then I'll place a tangency between the outside here.

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Hit Escape on the keyboard and notice that it's still free to move about.

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I haven't actually created a fully constrained sketch yet.

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If I expand the sketches folder, let's make note of the icon next to sketch.

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I'm going to take the center of my second idler.

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I'm going to control or command select the origin and then I'm going to use my horizontal vertical.

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As soon as I do that, all of my sketch elements turn black and the icon changes from a pencil to a small lock.

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This is telling me that I have a fully defined or fully constrained sketch.

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From here I'm going to finish the sketch, I'm going to go back to a front view and I want to talk for a second about each of these gears that we drew.

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These are going to be placeholder positions to get us a good idea of where all of our gears need to be.

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We have our drive and driven gears at the center.

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Our final assembly will have a common shaft that allows us to drive one of the gears and then have a bearing so that the other gear is free to rotate.

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We’ll transfer power from the center here moving over to our first idler gear which will change its direction to counter clockwise.

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As we move to the second idler, this one will change to clockwise.

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And as we get to the third idler, it'll change again to counter clockwise.

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As this one is rotating counterclockwise, it will rotate the large gear clockwise.

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So using this idler strategy and having three separate gears allows us to create the correct rotation of our input and output.

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Remember that we are talking about our drive gear being our large gear and our driven gear being our small gear.

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But it is important to note that this type of assembly can work in either direction.

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We can have our input beyond the smaller gear which would allow us to reduce or increase the torque and speed.

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Now I say reduce or increase is because depending on which side is our input and which side is our output.

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We're either going to be increasing torque in reducing the speed or we're going to be reducing torque in increasing the speed.

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So again, it's important to note that the input and the output can vary depending on how we want to use this assembly,

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but we are considering our large gear to be our drive gear and the small gear is going to be our driven,

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and all the smaller gears here are going to be our idlers.

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So from here we want to rename our sketch,

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we're going to do this by selecting it, left clicking on it one more time and we're going to call this our Layout Sketch.

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Renaming our sketches is an important step in the process, especially once we get a few sketches inside of this folder,

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it's going to be much easier for us to identify what that sketch was used for.

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If we hover over the sketch icon that's inside of the timeline at the bottom, you can also see that the name does appear.

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Layout Sketch is shown there and it's inside of our gear reduction housing.

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From here let's make sure that we do save this design before moving on.