Editing part features
Video: Editing part featuresNow that we have a completed part, I wanted to step back for a minute and talk a little bit about editing those features. The one constant in design is change. After completing a part like this, it's common practice to create a prototype or an initial part, maybe do some analysis or testing, and determine whether or not the design works. More often than not, it turns out that changes need to be made. The beauty of Autodesk Inventor is that you can go back and make changes to any of the sketches or any of the modeling features that you used to create this part. In the browser, you see the list of features we've created, Extrusions, Revolves, Holes, and Chamfers.
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This course introduces you to the interface and key processes of Inventor, the parametric design system from Autodesk. Author John Helfen covers sketching, part modeling, assemblies, and drawings. These tasks work in conjunction, allowing you to create parts and assemblies and document them in a way so that the manufacturing process proceeds faster and more efficiently.
- Navigating drawings with the View Cube and other navigation tools
- Sketching geometry
- Dimensioning parts
- Creating parameters
- Drawing circles, squares, and other shapes
- Creating extrusions
- Creating and managing constraints in assemblies
- Setting basic drawing dimensions
Editing part features
Now that we have a completed part, I wanted to step back for a minute and talk a little bit about editing those features. The one constant in design is change. After completing a part like this, it's common practice to create a prototype or an initial part, maybe do some analysis or testing, and determine whether or not the design works. More often than not, it turns out that changes need to be made. The beauty of Autodesk Inventor is that you can go back and make changes to any of the sketches or any of the modeling features that you used to create this part. In the browser, you see the list of features we've created, Extrusions, Revolves, Holes, and Chamfers.
The sketched features, which are indicated by the plus symbol, show both the extrusion or the modeling future that we created, and the sketch that was used to create that. When you create the modeling feature, the sketch gets consumed and linked to that modeling feature. Say, for example, our first change was to go back and make a modification to the original base sketch. If you hover over the extrusion in the browser and right-click, you have the ability to edit the sketch that's driving it or the feature itself. We're going to start by editing the sketch.
When you do that, Inventor put you back in the sketch environment, and you can make changes to the sketch as if it were the first on you are creating it. If we double-click a dimension, we can change its length to 1 and the geometry updates. If we finish the sketch, the model geometry updates to reflect that change. We could also go back, and make changes to the feature itself. If you right-click on the feature in the browser, rather than selecting Edit Sketch, we can edit the feature. Here, you can see we have the option to reset any of the settings that were used when creating this feature.
Rather than Symmetric, we could change the direction of this extrusion. Now I am not going to make that change because I know we specifically picked Symmetric so that we can use the origin geometry to create other features in this model. However, we could change the height of this model. We could change it to 1 inch as well. By applying these changes, the model immediately updates. One of the things we'll notice is that because this part got bigger, this boss didn't change, but it needed to. If you remember, when we created this boss, we dimensioned it from this edge of the part, and it's maintained that relationship. That boss is Extrusion 2 in our browser.
If we hover over it and click the plus symbol, you can hover over the sketch just to quickly review that sketch. In this case, I can see the 0.319 here, and I know this is something I want to change. Instead of making the change from within the browser, this time I want to show how to use the heads-up display to make this change. If I select this face in the graphics window, the heads-up display provides two different options. Just like in the browser, I have the ability to edit the extrusion, or I have the ability to edit the sketch. By clicking Edit Sketch, I get the same result as if I would have selected Edit Sketch in the browser, I am returned to the sketch environment, and I am able to make changes to this geometry.
I am going to go ahead and change that 0.319 to 0.6 to accommodate for the change that we made in the base extrusion. By finishing the sketch, you will notice a couple of things happen. The boss and everything attached to it moved, but not only that, if we rotate, you'll notice that the boss on the bottom also moved to reflect that change. If you remember, when we created this bottom boss, we projected geometry from the top boss, and that intelligence and relationship has been maintained.
If I select this boss down at the bottom and edit its sketch, you will notice there are no dimensions, but the lines are yellow indicating that things were projected. Because those two things are linked, the updates are automatically maintained for you. I am going to go ahead and finish this sketch, and let's look at this model a little more closely. If we orbit around, there is one item that I knew was going to happen, and that is when we change that boss, the distance or depth of this hole has become an issue. Just like a sketched feature, we can go edit placed features as well.
In this case, I am going to select the face of this hole, and the one option I'm offered is the ability to edit this feature, or edit this hole. Because it's a placed feature and not driven by a sketch, the Edit Sketch option is removed. By clicking on that option, we're returned to the Hole dialog, and we have the ability to make changes to this feature. We could enter a new distance, but rather than that, I am going to rotate around to the left side and use the heads-up display to make this change. I know that this hole is required to pass this boss that we just made a change to. I am going to select the arrow at the end of the hole, and use the preview to actually see where this hole needs to end.
At this point at 0.9755, I can see that it's passed the boss, and I can accept those changes, and review them in the graphics window. If I orbit around, you now see that the hole extends past the boss, and the hole that created through it and the model is complete. Now that we've made changes, I think it's important that you understand that at any point in time during the design process, you are going to run into times where change happens. That's expected and Inventor is purposely made for that. At any point in time, feel free to return to your browser or to your heads-up display to make changes to features to ensure your parts meet your design requirements.
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