Utililze appropriate modeling editing and adjusting strategies

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After completing this video, you'll be able to edit parametric values, utilize user place workplanes, axes and points,

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and display a part at its nominal Max-Min tolerance while standardizing interference.

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Inside Inventor, we want to begin by opening 2 supply data sets, diffuser.IPT, which is located in the top of our project

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and Valve Seat Assembly, which is in the assembly subfolder under Valve Seat.

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We're going to be taking a look at a couple more modeling strategies and understand how we can make more robust models.

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First, with the diffuser, we have a couple of things that we see on the screen in Sketch 2,

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and these are going to be used for plane creation in just a moment,

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but we want to get started by first taking a look at sketch one.

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We'll begin by editing sketch one and making note of our sketch.

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Whenever we're creating a design, we often need to think about how it's going to update if any model dimensions change.

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With this diffuser, the main criteria here is the inside diameter, this .250 value.

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When this design was created, no user parameters were created for those values.

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You can see D0 is .25 and the outside diameter is D1 at one inch.

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It's a good idea for us to at the very least name the critical dimensions so we can reference them later.

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To do that, let's go ahead and double click on this quarter inch,

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and at the beginning we're just going to type ID space equals and hit enter.

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Now if we go ahead and take a look at this inside of our parameters,

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we can see that the model parameter name is ID instead of D0.

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Even though we didn't create a user parameter before that sketch was created,

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we can still rename those dimensions.

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We can also add equations inside of this dialogue box.

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In this case, let's go ahead and make the OD equal to the ID times 4.

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We'll hit enter.

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It's still a one inch value, but now if we manipulate or modify the inside diameter,

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it'll maintain the same relationship or ratio as a four to one value for that outside diameter.

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If we go back and finish this and go to our user parameters,

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we can see those values listed at the top of our user parameter dialog.

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The ID is .25 and the OD is now listed as ID times 4.

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If we were to change the ID to a larger value of .5, we can accept that.

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Notice that there are other changes that are problematic downstream.

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This is really based on the way in which the original sketches are defined,

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and often times you need to work through this process figuring out how sketch dimensions and references

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can be used to ensure that your models update properly.

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Taking some time to understand this process is important when creating more robust parametric based models.

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In addition to creating robust sketches and features,

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often times we need to use additional information such as splitting the face of a part

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and adding additional sketch entities for us to be able to create reference geometry.

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In this case, the work features such as planes, axes and points

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can be used to create various additional work planes to define complex features.

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For example, if we need to add a small hole or a boss to the side of this tapered part,

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what we can do is go to our plane option and we can either use the default plane which is based on our selection,

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or we can pick a specific plane.

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In this case, we can see that we can use tangent to surface and parallel to plane,

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tangent to surface through a point, or tangent to surface through edge.

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If I pick tangent to surface through edge, I can pick my surface, pick the edge and create a new plane.

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Right click and we can repeat that process on the inside as well.

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So we'll go tangent to the inside surface. We'll select this edge, and now we've created a new plane that's tangent

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at that specific instance.

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We could also use these reference sketches to add a plane that is normal to a curve at a point.

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Either of these options will work because we were able to add that curve perpendicular to a slice

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through the tapered section of that part.

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Any geometry changes at the sketch level will allow us to update all of these planes individually.

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If we are creating another plane, let's say we wanted to create an offset plane.

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What we can do is we can use the offset plane option

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and we can push this in the negative direction -.625

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Even though this plane was defined as being an offset from that original selection,

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we can always redefine the feature, and in this case, let's select both of these planes

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and create a mid plane.

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Using the redefined feature option or reselecting the references for sketches, and in this case, offset workplanes

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can be extremely helpful to make sure that downstream everything updates properly based on those parametric inputs.

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The big takeaway here is to make sure that you understand how each of these planes is created

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and how they're referenced when geometry changes downstream.

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Next, let's move on to our valve seat assembly.

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When talking about assemblies, we also want to think more about things like tolerances.

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When parts need to fit together, it's critical that we understand how large or small they will be in the manufacturing process.

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For this, we're going to open up our needle component by right clicking and selecting Open.

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Let's go to our parameters and note that we've got a needle D, which is our needle diameter.

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If we select the tolerance and use the pencil icon to edit,

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we can change the tolerance and note that it's symmetric ±.01 inches.

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Using the evaluated size, we can display it at its Max value or its min value.

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If we want to analyze whether or not parts will fit together in the manufacturing process,

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we need to make sure that we analyze these internal parts at their Max value and the external parts at their minimum value.

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Let's go ahead and select done, and let's go back to our assembly.

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When we take a look at our assembly, it might not be instantly apparent that there's some overlap.

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We can use tools in our inspect section to analyze interference between components.

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When we analyze the interference between these components,

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we'll be able to see if there's any overlap.

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We can select OK, go back to our needle part, go back to our parameters,

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and this time we're going to display it at its min value.

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We'll go back to our assembly and run interference detection again.

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You can see that we still have some interference between these,

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but our assembly has not been updated.

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Let's go ahead and make sure that we update our assembly and that all parts are the correct size.

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Then we can re-analyze our interference detection, say OK,

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and make sure that we do have an appropriate amount of interference or small gap if needed.

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Sometimes modifying values to be a little bit larger can be helpful.

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For example, this 30° value

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we can have a ±2° tolerance and we can display it at its min or Max value.

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When we do this, the change will be much more apparent.

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Back in our valve seat assembly, you can see that there is quite a big gap now between the parts because the angle no longer matches.

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We can't make sure that we update the assembly and use interference detection,

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even though we can visibly see that the parts no longer interfere.

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Making sure that your parts are well within tolerance when they're being manufactured

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and making sure that they do still fit together in your digital assembly

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is an important step in the process of designing these parts.

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For this part, let's go back to the needle, go back to our parameters,

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and we're going to set both of these back to their nominal value, select done, and go back to our assembly.

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We have the ability to update this assembly and also note that we can move our parts throughout their travel

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and we can analyze their interference to also get a good idea as to whether or not the Max travel

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or the amount of movement in our assembly is applicable or not for our design.

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In this case, we do want a small amount of extra travel to make sure that the needle and seat are seated properly,

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but the angle between them is the critical aspect.

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So making sure that our tolerance values are acceptable for the angle of the tip of our needle is going to be a key aspect

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in the design process.

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At this point, nothing needs to be saved,

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so go ahead and close all designs and move on.