Start learning with our library of video tutorials taught by experts. Get started
Viewed by members. in countries. members currently watching.
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.
On the screen you see our completed Carburetor Housing, and we're going to use this part as we look at how to work through the process of placing views. To begin, we need to create a new drawing file. To do that we can select the Application menu, and then click on New to bring up the Create New File dialog box. We're going to go ahead and create a Standard.idw file. We'll select that in the dialog box and click Create. By doing this, Inventor creates our first sheet in our drawing for us. You can see that it's preconfigured a drawing border and a title bar on a C size sheet of paper.
There are a couple of ways to begin creating drawing views. The initial view is called the Base view. You can find the Base view under the Place Views tab in the Create panel. But instead of doing that, I'm going to use the Marking menu. You can also right-click and select Base view there to initiate your Base view creation. By doing so, the Drawing view dialog box is presented, and there's a few things in here that we want to talk about so that we better understand the process and how to move forward. First, you'll notice a File dropdown list. This lists all the files that are currently open in the background.
In this case, it's just our Carburetor Housing. If you didn't have a file open, you could select the Open an existing file and select a specific file from your hard drive. Next we have the Representation section. Now, we didn't create any view representations for this model, but I wanted to explain very briefly how that would work. If in our engine assembly we wanted to show a representation of the piston at its fully extended position and a view with it in its fully retracted position, we could do so and they would be listed here. We can then select one of those to create a Drawing view.
Next we have the Orientation section. The Orientation section lists several different positions of our model. If I hover over the graphics window, you'll see a preview of that model in its Front Orientation. We can go back and select a different Orientation if we need to start from a different position. In this case, I want to start with the front, that works for me, so I'm going to leave that as it was. The next thing you might notice is the preview is a little small for the sheet size we have. To change that, we can go to the Scale section at the bottom of the dialog box, and we can select a different Scale for our drawing.
In this case, I'm going to select 2:1, and you'll notice that the preview updates to reflect that change. The other item I'll mention is the Style section. We're not going to change this right now, but I want to call it out because we will later in the movie. The default style is to show Hidden Lines. You also have the ability to show with Hidden Lines Removed and Shaded views. We're now ready to place our view. I wanted to remind everybody that we are in our Base view command. I'm going to go ahead and zoom out a bit and position our sheet so that we can place our Drawing Views.
As I move the cursor, the view follows around. I simply need to find the location that works best for this Drawing view and left-click to place it. In doing so, the dialog box is removed, and we're moved into the Projected mode. You can see on the Ribbon bar that the Projected command is highlighted and active currently. I'm going to go ahead and zoom in a bit, or reposition my view a bit, and as I move my cursor, you'll notice because we're now in Projected, the cursor is showing previews of what a Projected view would look like.
Inventor does this on its own, because the most logical step after a Base view is to create several Projected Views of that model. All you need to do is simply move your cursor to the position you wish to place the view, left-click, and a temporary version of that view is placed on the drawing sheet. As I move my cursor up a little bit further, I get a preview of an Isometric view. I can left-click to temporarily place that, and then I can position my cursor above the Base view for a Top view, and I can left-click one last time to create a temporary version of that view.
Now that I have all my views placed, I want to go ahead and create them and have Inventor actually create the views on the drawing sheet. To do that, you simply right-click and select Create. If I zoom in a bit, you can see what happened. Inventor created my Drawing Views, and because the style was Hidden Line, I can see my object lines, I can also see the hidden lines representing the holes being cut through this part. Now that we have the views placed on the screen, I want to show a little bit about how they're connected. As I mentioned, we created a Base view at this point.
If I hovered over that, you can see that it highlights in red, it's also highlighted in the browser as well. It's important to remember that just like parts and assemblies, the browser in the drawing represents the things are being shown on the screen as well. If I were to hover over this Drawing view and left-click and drag, you'll notice the connection between the Base and Projected Views. As I reposition my Base view, the alignment with the Projected Views remains connected. If you need to change that, in most cases that's going to be perfectly fine.
In certain scenarios you may need to break the link between the Projected view and its parent view. If you hover over one of the Projected Views and right-click, in the right-click menu you have an Alignment option, and you can choose to Break that alignment so that you can reposition it in a location that is not in alignment with the Base view. In this case, I do want to maintain that alignment, so I'm going to skip that for now. Before we move on to our next movie, I wanted to add one more item here. The Isometric view, while not connected to the Base view, is really there to give better visualization to the other three views.
By having an Isometric view, people can more quickly understand the details that are involved in those other views. Earlier in the movie we talked a little bit about the Style section of the Create dialog box. If I hover over my Isometric view, right-click and select Edit view, that dialog box returns, and we can make changes to some of the initial settings. If I wanted to I could adjust the Scale for the Isometric view, but in this case I actually want to change the Style. I would prefer to have this view Shaded to better improve the visibility and understanding of what this design entails.
If you zoom in a little bit, you can see that this with it shaded actually very closely represents the model that we saw on the screen in the modeling view. At this point, we've created our initial Drawing Views, and we can move forward with documenting our design.
There are currently no FAQs about Up and Running with Autodesk Inventor.
Access exercise files from a button right under the course name.
Search within course videos and transcripts, and jump right to the results.
Remove icons showing you already watched videos if you want to start over.
Make the video wide, narrow, full-screen, or pop the player out of the page into its own window.
Click on text in the transcript to jump to that spot in the video. As the video plays, the relevant spot in the transcript will be highlighted.