Create parameters

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Create parameters.

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In this video, we'll learn to create a list of user parameters and add them to our favorites.

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To get started, we want to make sure that we have Fusion 360 open as well as our gear reduction parts and specs spreadsheet.

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Before we get started creating any detailed drawings or models,

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we want to make sure that we understand some of the nomenclature of what we're working with.

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So to get started, let's take a look at the three areas in our reduction parts and specs, first starting with gear parameters.

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There are a couple values that we need to make sure that we understand as they'll be important later when we begin to create our gears.

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The first value is our module.

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This module value is a size ratio between our pitch diameter and the number of teeth in our gear.

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For example, the module of 2 and the number of teeth of 48 is going to give us a 96 mm diameter gear.

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As we look through here, we have our drive driven in two different idler gears.

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When we look at these values, we can see that the number of teeth is giving us a 3:1 ratio.

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The idle gears are not going to affect the overall input and output ratio but they will affect the direction of travel.

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So these are things we need to keep in mind as we begin designing our own reduction assembly.

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We have a backlash value which will give us a small amount of space between gears.

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We have a root fillet which is the rounded corner where the tooth of the gear actually enters the main body.

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And then we have our thickness value and the hole diameter in the center.

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The next section we have is for user parameters.

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The user parameters are going to be values that we create in Fusion 360 that can be linked to various parts of our design.

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We have our drive gear teeth, our driven gear teeth, the idle gear teeth, our module,

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the drive gear and driven gear diameters, our idle gear diameter.

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And then we have some various parameters for things like the mounting bolts, the flange and the gear clearances.

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We also have a section called cots.

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These are common off the shelf parts and these are all make master car part numbers for things like bearings or hardware that we’ll look at later on.

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So make sure that you have this list available as we begin to create our models.

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In Fusion 360, we want to make sure that we have a project and a location to store all our data.

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I've created a new project called 21 Modeling and Design for MFG or manufacturer.

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I've also created some sub folders, basics of modeling and basics of assemblies.

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We're going to get started on a new untitled document and we'll be saving it inside of our basics of modeling.

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You want to check to make sure that you are using metric units and we'll get started by going to Modify and selecting Change Parameters.

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Parameters are extremely helpful whenever we're starting a design that relies on external data.

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When I say external data, what I mean in this case is the fact that we know the size of our gears, we know various parameters about them,

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and some things like the amount of clearance we're going to need.

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So having these values predefined will make it much simpler when we start creating our models and also it will help us update the design later on.

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To create these parameters, we’ll get started by selecting the plus icon next to User Parameters and begin entering a new value.

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First we'll start with the name and in our case, we're going to start with our Drive_Gear_Teeth.

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This is coming directly from our user parameters on that spec sheet.

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It's important to note that teeth in the context of our gear is unitless.

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It's not going to be a metric value such as a millimeter.

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It's going to be a numerical value that represents the number of teeth.

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So make sure that we do set the units to no unit and the Expression is going to be 48.

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We'll select OK. And we'll create another user parameter.

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Next we'll be creating our Driven_Gear_Teeth.

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Once again, this will be unitless but in this case, I know that I'm working with a 3:1 ratio.

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So I'm going to begin typing the letter D and then I'll select my Drive_Gear_Teeth and simply divide that by 3.

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This is a wonderful way for us to create this parameter.

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That way, if we decide to change that 48 tooth gear to something larger or smaller, then we can keep that 3:1 ratio.

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Let's go ahead and add a few more user parameters.

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Next, we're going to talk about the idle gear teeth.

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So once again, Idle_Gear_Teeth, changing the unit to unitless or no unit.

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And then setting this to a value of 10.

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Now we have a couple of these values, let's go ahead and add our gear module.

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Once again, we're going to start typing this in with an underscore,

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making sure that we set any of these values that have no units as no unit and we're going to enter a value of 2.

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We'll say OK, and now we've created our first four user parameters.

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The next thing that we want to do is we want to start to create some relationships between some of these values that we've already entered.

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As I've already mentioned, the gear module is a ratio between the number of teeth and the pitch diameter.

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So number of teeth of 48 and a pitch diameter of 96 will give us a gear module of 2.

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Let's test that out by making a user parameter.

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In this case, we're going to start by typing in Drive_Gear_Dia for diameter.

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This will be a metric value so we're gonna leave the units at mm.

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I'm going to get started by placing to open brackets and I want to start by typing the letter D and I want to select my Drive_Gear_Teeth.

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Remember this is going to be a 48 and it’s unitless.

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I then want to multiply that by my gear module.

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Once again, I'll start to type G.

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Going to close my brackets off, but we're multiplying a gear module and a number of teeth, both of those are unitless.

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So I'm going to multiply both of those by 1 mm and then close my brackets.

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This is going to give me a value of 96 and because we multiplied it by 1 mm, we're going to have 96 mm.

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This is going to represent our drive gear diameter.

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Let's go ahead and create another one and this will be our Driven_Gear_Dia.

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Once again, the units are metric, I'm going to start with those two brackets and we’ll start to type in driven,

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making sure that we have are Driven_Gear_Teeth, multiply that by our gear module.

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And if you make a mistake, you can always back up by using the backspace and again, we'll start to type in G for gear module.

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Close the brackets, multiply it by 1 mm and close off our second set of brackets.

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You have to make sure that you do include the asterix for multiplication.

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That way it knows that it's multiplying it by that value, simply putting it in brackets will not have it multiply those two together.

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Once again, we can check this with our spreadsheet, making sure that we are seeing 32.

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Let's go ahead and do this one more time.

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This time it's going to be for our idle gear.

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So Idle_Gear_Dia for diameter, two brackets and we're gonna start with our Idle_Gear_Teeth.

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We're going to multiply that by our gear module.

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We're going to close our brackets and multiply that by 1 mm and close off the final bracket, giving us a value of 20 mm.

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So again, we can check those values and take a look at our spreadsheet to make sure that all of those values are matching.

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At this point, I want to make sure that you carry on with some of those other values in the spreadsheet adding the values for our mount bolts,

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our idle gear shaft, our mount bolt flange and our gear clearance diameter.

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Those are all going to be metric values so make sure that you use the units mm.

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Before we go on to the next video, I also want to talk about creating favorites.

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As you begin to create complex designs, especially with large numbers of user parameters can be hard to keep track of them.

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Every time you create a sketch or some sort of feature, model parameters will begin to populate.

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So we'll have our model parameters as well as a large list of user parameters.

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So I like to use the Favorites option by left clicking on the star next to my User Parameter and that will put it up in a Favorites category.

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This makes it a little bit easier to find when I come back to my parameters list.

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There are a few things that are going to be important to us.

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Things like the drive and driven gear values, our idle gear value, our gear module as well as the various values for the diameters that we've created.

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Now in this case, I've added everything from my initial list to my favorites.

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That doesn't necessarily mean that you have to add all of them,

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but it is a good idea to make sure you understand how to filter and work inside of the user parameters.

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So that way you can make it easier to come back and change those values.

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These values will end up getting linked to sketches as well as feature diameters and distances.

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And these different values can be manipulated and modified directly in here.

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For example, if I decided I wanted to use a 60 tooth gear, you can see that that changes my Driven_Gear to 20,

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and it also modifies things like the diameter of my drive and driven gears.

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If I reset that back to 48, everything goes back to those initial values.

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So it is extremely important that we understand that we can modify these values in here,

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and they will affect all of the different sketches and features that we're using.

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The last step here is to make sure that we do save this design.

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I'm going to call this my Gear Reduction Housing.

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And I want to make sure to put it in my 21 Modeling and Design for Manufacture,

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and I'm going to stick it inside of a basics of modeling sub folder and select Save.