Modify parts and assemblies parametrically

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Modify parts and assemblies parametrically.

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After completing this video, you'll be able to modify an existing 3D part using the parameters table,

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update drawing views following a change in parameters,

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confirm that a drawing accurately reflects the model after altering a parameter,

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link a parameter to another part or assembly, export a parameter to an iPart,

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check the Parameters table, change your parameter expression and change the parameter unit,

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and ink the parameters from an Excel spreadsheet, a part, or an assembly.

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In Inventor, we want to begin by opening up a handful of data sets.

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We've got engine_case_rear.IPT, which is in the assembly subfolder under Engine MK2,

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as well as the carb.IAM assembly in the same subfolder.

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We also want to open up link_parameters.IAM, which is in the assembly's parameter subfolder, and hole_pattern.IPT in the same folder.

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We're going to be taking a look at parameters and expressions inside of a design.

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We want to figure out how we can link them between parts and how we can export them.

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To get started, first we want to focus on engine_case_rear.IPT and select the FX icon at the top of our screen.

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Let's go ahead and expand this window vertically so we can see a lot of the parameters.

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When we take a look at a Parameters window, we can see that we've got our Model Parameter name.

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In most cases this will be D0 for a dimension.

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And as we move over, we've got the Consumed by, which tells us which sketch is using it, the unit type, and then we've got our equation.

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Now if we take a look at some of these values and we scroll down,

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you'll notice that some of the Consumed by columns will be empty.

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This often times happens whenever we have a dimension that's no longer needed,

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either the feature that it was referenced by or sketch element that it was referenced by is removed.

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In most cases, you can use the Purge Unused and clean out your parameters file, unless you want to keep those.

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In some instances, you might notice that they'll be displayed in red if there's a potential problem.

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In this case, you can see that we've got a unit mismatch.

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The units in this case are listed as millimeters, but the units in the equation are listed as degrees.

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We can simply change the units in this case, removing the degrees, DEG.

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We can add millimeters, MM, or we can use another unit type that can be easily converted.

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For example, if we put IN for inch, Inventor will automatically convert the millimeter unit into the inch unit

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and allow us to just simply input those values in those default units.

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Let's go ahead and select Done and move on to our next file.

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We want to take a look at our carb.IAM.

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When we take a look at the carb.IAM parameters, you can see that there are not nearly as many parameters in this list.

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Let's go ahead and shrink our Parameter window down.

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One thing that we want to identify is the ability to select Key for specific parameters we want to identify

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and then selecting a Key at the top will allow us to sort and filter these based on that selection.

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You can also select the filter by parameter name, consumed by, the unit type, and even the equation.

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Keep in mind that using Key does have additional functionality downstream for things like creating iParts.

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But for right now, just make sure that we can identify the ability for us to filter and work through a parameters table

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to simplify it by using those keys as well as other values.

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Let's go ahead and select Done and move on to linked parameters.

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In some instances, you may have multiple parts in an assembly that you need to have share a common parameter.

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This can be done in multiple ways, for example using associativity.

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However, in some cases, you have designed the individual parts and you simply want to share a parameter from one to the other.

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In this case, we want the hole diameter and the pin diameter between the base and the cap to be the same.

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To do this, we're going to double click on the Base component, go to its parameters,

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and we're going to identify the parameter called Hole.

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We're going to select the Export option and Link.

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From here, we can either select an Inventor IPT or IAM or link to an external Excel file.

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For our purposes, we want to make sure that we link this component to the Cap part and select Open.

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We want to left click on the hole, say OK, and then say OK.

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Notice that the hole is now displayed here as hole_1 because it shares the same name as the user parameter inside of this design.

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To link these together, all we need to do is use the right arrow, List Parameters, and select hole_1.

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Now, the hole in our design is going to be listed as quarter inch and the designs are going to update appropriately.

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Let's go ahead and select Return and let's double click on the cap.

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If we expand the parameters for the cap, notice that the hole is listed as .25 here.

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If we increase it to half inch, it's going to update not only the pin size, but also the hole in the base component as well.

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So being able to link these parameters between multiple parts in an assembly can be a handy design tip,

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especially when you're creating the parts individually with no context inside of the assembly.

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Next, let's take a look at the hole_pattern.IPT.

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In this design, we've got a hole pattern on our part that has a specific dimension from one edge,

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but you can see that it's further away from the other edge.

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We're going to use parameters and specifically creating an equation in our parameters to drive the pattern spacing.

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Currently, you can see that the pattern spacing is set to 1 inch.

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We're going to practice creating a new numeric parameter, and we're going to call this one hole_spacing.

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The hole_spacing is going to be in the inch unit system but, you can select the units and change this if needed.

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For example, the units for a pattern are often unitless.

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We're going to select OK using the default inch unit system here.

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Next, what we want to do is create an expression that we can use to drive the overall pattern spacing.

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To do this, we need to begin with some brackets “[”.

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We can start typing in a specific user parameter or we can use the List Parameters option,

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and we can start by using “Plate_Width”.

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The plate width is going to be 4 inches.

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That's the overall width of our plate.

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And what we want to do is subtract out the hhole LOC, or location, which is a quarter inch from either side.

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So we'll use minus bracket, and we can manually type “Hole_LOC”, as long as we make sure that it's case sensitive,

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“* 2”, and then we'll close those brackets.

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This is going to give us a dimension that references the plate width minus the spacing on either side,

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so essentially a 3 1/2 inch dimension.

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The next thing that we want to do is divide this, and we're going to start with another pair of brackets,

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by “D8”, which is the number of patterns that we have for, and “- 1”, and we'll close that bracket.

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Now, the main reason that we do this is because when we have a number of patterns,

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in this case four instances, the spacing is actually the distance between each of these,

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not accounting for the space at the end.

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So we have 1, 2, and 3.

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Next, let's go ahead and edit the rectangular pattern feature.

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And inside of our Spacing, we're going to select List Parameters,

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and we're going to use the new hole spacing parameter that we created.

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To verify this, let's go back and let's modify the plate width down to three inches.

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We can see that the hole spacing updates properly.

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We can even go down to 2 inches and see that it's always staying 1/4 inch from both sides.

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If we go back up to 4 inches, the hole pattern updates properly.

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Let's go ahead and take a look at what happens with these specific parameters when we try to author an iPart.

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Let's navigate to Manage and select Create iPart.

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Any time that we have parameters in a design that have a unique name,

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these parameters that were created by the user, these will automatically be added to our parameters list when authoring an iPart.

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You can of course select other parameters and push them over,

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but for the main purposes here,

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we want to make sure that we identify the fact that any time we've got a parameter that is named something custom,

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it'll automatically be included.

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Now, in this video, we're not going to be authoring an iPart,

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but it is important to understand that the way in which we build these files can have downstream implications,

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either making your job easier for things like authoring an iPart,

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or sometimes making it harder if you have to navigate and find those individual dimensions that are needed.

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The last thing that we want to do is take a look at what happens when our parameters are updated in a detailed drawing.

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So let's go ahead and create a new detailed drawing using the default template.

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We'll start a base view and make sure that our scale is set to something like 2:1.

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We can determine what we want in terms of our view, for example, setting up a raster view.

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But in this case, let's just say OK, and create a projected view out to the right and an isometric view so we can see the holes.

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Right click and Create.

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If we navigate back to our hole pattern part, go to our parameters.

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Let's change this to something a bit more extreme.

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We'll select Done and notice that the part itself has updated automatically,

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and the hole pattern drawing has updated automatically as well.

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Notice that we have a slash through indicating that this is a raster view, and when we select the view, we have the option to update.

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Even though the view has been updated automatically, we are able to push an update if we need to.

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We can also go back and modify our drawing views at any time,

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toggling off our raster view option for example, and when we select the view we can update again.

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Making sure that parts are updated based on the user parameters

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is an important step to make sure that your detailed drawings are up to date.

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By default, all the settings will automatically push the updates from the part or assembly into the detailed drawing.

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Just make sure that you identify whether or not an update is required by the lightning bolt icon,

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either over your drawing view or shown at the top of the screen.

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At this point, let's make sure that everything we've done is saved and we can move on to the next step.