Utililze appropriate modeling strategies

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Utilize appropriate modeling strategies.

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After completing this video, you'll be able to design an appropriate strategy for modeling a part with complex repeating geometry,

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create models that capture design intent,

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recognize modeling strategies that make a parametric model more robust,

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explain the differences between the available derived style types when editing a derived part,

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and design parts with appropriate reference planes and sketch profiles.

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To get started in Inventor, we need to open up a handful of data sets.

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First, we have Port Plate.IPT, which is located in the top of our project.

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We have Plate Assembly.IAM, which is in the assembly subfolder under bolted pattern.

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We have Plate A which belongs to the plate assembly in the same folder,

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Blower.IAM which is in the assembly subfolder under Blower, and Reference Planes.IPT, which is at the top level of our project.

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We're going to be covering a lot of topics in this video and to get started we first want to talk about order of operations inside of our browser.

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Now often time when we create a design, there may be features such as a fillet

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that really should be part of a pattern or a mirror feature or just have happened earlier inside of the process of our design.

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For example, in this case we've got a port plate which has two ports that need to be identical.

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Instead of applying the fillet to eight corners,

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what we can do here with this simple example is we can pull the fillet up before the mirror

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and then we can modify our mirror feature to change the occurrences.

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In this case, we simply need to add the new feature for the fillet and say, OK.

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Now this is obviously a simple example with a single feature that could be added easily after the mirror,

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but making sure that all of the features are grouped together before features like mirrors or patterns

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can simplify the model and the calculation time required to complete complex models.

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But let's talk about another topic.

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In this case, what if we need to suppress some features based on the overall length of the part?

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There are a couple of ways that we can do this.

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One, if we select the feature, right click, we have some options.

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If we select Suppress Feature, you can see that the feature itself disappears.

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But this suppressed feature only ends up happening when we're talking about suppressing it manually inside of the design.

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If we want to add a little bit more logic, we need to use a couple of other tools.

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If we right click on the rectangular pattern again and take a look at its properties,

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there's a Suppress section where we can say if, select one of our user parameters,

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in this case the overall length, is, let's say, less than 5 inches.

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So, if we go into our user parameters and find the overall length of our part,

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let's go ahead and drag this up to the right and we set this to 4.5 inches,

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it's going to suppress the whole pattern, leaving only a single hole pattern in the center.

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If we increase the length back to a distance of 5 inches,

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you can see that we now have three holes in the pattern and again, 4.9 less than 5,

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it'll remove them and back to the original value 6, it puts the holes back.

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So using the feature properties is a great way for us to calculate whether or not certain features are going to be suppressed.

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But if we need a little bit more logic than that, if we need to add in some additional rules or potentially variations of the design,

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we can configure this as an iPart.

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For this, let's go to Manage and select Create iPart.

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When we create an iPart, we want the pattern quantity, and we also want the length value.

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Because these were custom parameters that were created, they're automatically added to our list.

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What we can do is come down to our table and insert a row.

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For the second variation, if we have an instance where the overall length is 4 1/2 inches, we can set the pattern quantity here to 1 UL.

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We'll say OK, and now we have a table with multiple variations of the port plate.

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There are other ways that we can go about this process,

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but those are just two ways that we can use a little bit of logic

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to determine whether or not we have a certain number of holes or features in a design based on other user parameters.

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Let's go ahead and move to our next example, the plate assembly.

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For our plate assembly, we have two plates, a top and a bottom plate, and the bottom plate doesn't have any holes in it.

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What we can do is first take a look at our inspect tools and measure the size of our hole.

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We can see that the diameter is .266, which indicates that this is a passing hole for a quarter 20.

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Let's go and navigate back to our Assemble tools and then over to Design and use Bolted Connection.

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When we add a bolted connection in an assembly inside of Inventor,

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we have the ability to position the holes based on a couple of things.

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If we select the By Hole option and we select the start plane, an existing hole and a termination point,

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this will allow us to create a hole based on the size that it's measured.

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Now in this case, you can see that it gives us quarter inch as the largest possible size, but we also have some smaller options.

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We could use a #10 or #12 which will create the hole in the bottom plate.

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If instead we change the placement to concentric,

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we can use a concentric reference and then we can pick whichever size hole we want to add.

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In this case, we're not limited by quarter inch. We could go up to a .3125.

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If we say OK, it's going to increase the hole size on the top plate as well as add the hole on the bottom plate.

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Using these options for bolted connections can be a great way to add reference holes between multiple parts in an assembly.

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Let's go ahead and do control Z to undo so we can remove that hole.

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Let's move over to our plate A, which is part of this assembly.

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The plate that we have here looks to be fully defined.

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In the case that we've got an entire design that doesn't have any potential errors or warnings inside of our browser.

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Let's go ahead and take a look at our parameters and note that the overall design is listed as base length 1 1/2,

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and the rest of the dimensions are not created as user parameters.

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If we modify this value to say 2 inches, note that the right hole moves to the correct position, however the left hole is staying stationary.

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This tells us that there's some logic that's missing inside this design

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if we wanted to update properly with these parametric model changes.

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There are a couple ways that we can go about this.

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We can create a new user parameter to drive the dimension, but first we should go back to the original sketch that was used to create it.

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In this case, if we look at Sketch 2, we can see that we've got 1/2 inch distance from the center hole to this leftmost hole,

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and on the right hand side it says FX and .667.

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So this tells me that the right hole was calculated properly, but the left hole is not.

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A couple of ways that we can do this is one, we could take a look at adding a symmetry constraint

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or simply mirroring this hole to the other side.

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That would solve the problem in this specific instance.

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However, if we want to use a bit of logic, we can go back to our user parameters and we can figure out exactly how to drive this.

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This can be done from the user parameters, but it can also be done directly in a sketch by creating your own equation there.

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We can see here that D12 is listed as .266 and Sketch 2 shows D 7 / 3.

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Now 3 is the overall number of instances in this pattern,

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and if we take a look at D7, we can see D7 is a reference dimension which is 2 inches long.

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By using this reference dimension of two inches long and dividing it by three, it'll give us equal spacing for all three of these holes.

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So we could simply reference D12 for the position of this hole, or we can create a new parameter that calculates this for us.

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Let's go ahead and add a new parameter.

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We're going to use hole_space, and this is going to be equal to our reference dimension, which is D 7 / 3.

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That value is .667.

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Now, if we go back into our sketch, in this case Sketch 2,

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we can double click on this dimension, use list parameters, and we can set it to hole_space and say OK.

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Now if we make any adjustments to our parameters, in this case, if we set our base length to 2 1/2 inches,

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the hole should update properly.

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Now if we go back to 1 1/2 inches, that's the first size that we had in our part, the holes go back to the proper orientation.

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Let's go ahead and move on to our next example, which is Blower.IAM.

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When we're talking about an assembly, often times we need to use Derive to take certain components out or simplify them in some way.

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Let's go ahead and navigate through the browser and let's pick this motor as the Derive.

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We're going to go to our dropdown for Create Derived Substitutes and select Component Derive.

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We need to pick a location.

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So in this case, let's navigate to our blower and let's right click and create a new folder.

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We're going to add a new folder and we're going to call this Derived Motor.

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When we open the derived motor, you can see that it is coming in as a specific single body.

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If we expand this, we can see that there are multiple parts that are listed here,

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the AC motor and the shaft.

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If we right click on this, what we can do here is we can edit the derived assembly.

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When we edit a derived assembly, we have several different options.

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First is the derived style.

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We can have a single body which merges out the seams between planar faces.

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We have the option to do a solid body but keep seams between those faces,

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or maintain each solid as its own body, and we can also do a single composite feature which is a surface.

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Then we have some status options.

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We can include selected components, we can exclude the selected components, we can subtract the selected components,

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or we can also do things like create bounding boxes for the selected components.

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So in this case, for the AC motor, we may want to create a bounding box

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and only include the shaft position as that's the critical aspect of driving something with this motor.

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In this case, we could also toggle on some additional options at the top level and we can merge out seams or create a single solid body.

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In this case, what we're going to do is in the AC motor, create a substitute for that, and then we'll select OK.

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So now we have a basic black box with a shaft coming out that has the detail needed for the shaft position, the taper, as well as the key way.

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Using derives and derived substitutes inside of an assembly

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can be a great way to create simplified versions of specific components whose details aren't needed for the design intent.

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This is also helpful when we need to share out designs to 3rd party vendors that don't necessarily need all the detail required.

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For example, we could create a derived substitute for this entire design

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using just this tube at the top and the outlet or inlet on the side of the blower.

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These are great options for us when we're sharing data with third party vendors.

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Let's go ahead and take a look at our last example, Reference Planes.IPT.

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Often times when we're creating complex designs that include things like surface or solid lofts,

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we need to create reference planes along complex curves.

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Creating reference planes on curves generally involves creating a complex path

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and then adding points at reference locations that we can use to drive the planes.

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Keep in mind that those reference planes can lie on sketch points, but they can't lie on the points that are used to define the spline.

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When we go to our planes, we have a couple of options.

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We have the general plane tool, which will be based on specific selections,

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or we can pick a certain type of plane, for example, normal to curve at point.

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In this case, we're going to select our curve and select our point to create a new plane.

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Using the right click menu, we can repeat that option by selecting the curve and the point again, right click and repeat that one more time.

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And if needed, we can add those to the very end and the very beginning of the spline.

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So now we've got reference planes that can be used to create profiles for a complex shape.

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Keep in mind that these planes are linked to the curvature of the spline, in this case,

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and the location of the point.

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If we happen to modify any of these dimension values and update our design,

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the planes will move along with it.

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Remember when you're creating your workplane references to be sure the references that are being used

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are stable and defined in some way.

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You don't want to create planes that are going to be used for complex shapes that are under defined

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because they're likely to move and they will affect your overall geometry.

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Certain other types of planes can be extremely handy.

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For example, options to make planes tangent to a surface through an edge or surface through a point or surface in parallel to a plane.

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It's important to play around with all plane creation methods

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and realize that certain planes are going to be of benefit when you're working in complex shapes.

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There's no need to save any of these designs. We can go ahead and close them all and then move on to our next video.