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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.
In this chapter we've learned how to place views, we've learned a few ways to create dimensions, we've even learned how to control the precision of those dimensions. In this movie I want to turn our focus to Centerline, Center Marks, and Hole Notes. To create those, we're going to go to the Annotation tab, and under the Symbols panel you can see a few different options for creating Centerline and Center Marks. I'm going to zoom in on our front view and start with creating up general Centerline. This command allows you to simply select points in the view that you can create Centerlines from.
For example, if I hover over the midpoint on this side of the part, simply drag to the other side of the part and connect to the midpoint there, I can then right-click and select Create, and I've manually created a Centerline. This can be done with any view and any geometry within that view. The other way to create a Centerline would be to use the Centerline Bisector tool. This tool allows you to select two lines and have Inventor create a Centerline between them automatically. After creating the Centerline we can get out of the command, and we can manually extend that throughout the part. The next item I wanted to cover is Center Marks.
Center Marks are also very simple to create and are required in many drawing documents. The Center Mark tool is also located in the Symbols panel. After launching the command, you can create a Center Mark by simply selecting any circular geometry in a view. Inventor will automatically scale the Center Mark to meet the size of that specific piece of geometry. Now that we've created a few Centerlines and Center Marks, I wanted to turn our attention to Hole Notes. Hole Notes can be found on the Annotation tab under the Feature Notes panel.
The Hole Notes command is also very simple to use, and I wanted to call out some of the benefits of using it. While we were in the part modeling chapter we created holes using the Hole command and during that process I mentioned that we were building a lot of intelligence into the model through that command. Here's where we get to see the benefit of that. When we were creating the holes, the one hole that extended off of the revolve feature was actually a threaded hole. And if I select that hole in our drawing view, you can see that the Hole Note command has pulled the information directly from the model and updated that into our drawing.
In this case, it's an 8-32 threaded hole. Because it's connected to the model, if the model changes the drawing will automatically update to reflect that change. I want to turn our attention to another hole in the Section view. While still in the Hole Note command, we can select part of the circle that makes up the hole in the Section view. Here you can see the Hole Note has created a couple of pieces of information for this. It's pulled the diameter from the model, but it's also pulled the depth as well. Again, using the hole feature in the part modeling environment greatly affects the outcome of drawings that you're annotating.
Rather than having to manually input this information if you had used an Extrude, the information was built into the model and is actually pulled on the fly into the drawing, and it's connected so that any updates will be reflected without any intervention.
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