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Already up and running? This course is the next step in building your Autodesk Inventor skillset. Author John Helfen takes you through the interface and key processes of this parametric design system, including sketching, part modeling, assemblies, and drawings. Each process works in conjunction with the rest, allowing you to create parts and assemblies and document them in a way that they can be manufactured. Learn how to set up your project file; create and modify geometry; create extrusions, sweeps, and lofts; build parts with placed features and patterns of features; and create iParts and iFeatures. John also covers assembly visualization techniques, drawing views, and balloons and parts lists.
The course was created and produced by John Helfen. We're honored to host this training in our library.
We're now ready to begin looking at how to actually create the iPart. On the screen, you see the door handle we looked at when introducing eye parts, but it hasn't been turned into an eye part yet. At this point, it's simply a part that I've already created. It has a sweep, and it has a couple of holes that are threaded on the back that will allow us to attach this handle to a door in some fashion. What I do want to do before we actually begin creating it is cover some of the set up work that I did on this part in order to prepare it and make creation of an iPart a little bit easier, and that has to do with the parameters.
In the sweep feature, if you click the plus symbol to the left, and double click on sketch one, you can see the overall shape of the part, and some of the dimensions I used to create it. What I want to call out here is that I've actually named these variables or these dimensions with specific names that mean something. If you right click in the graphics window and select dimension display and select name, you can see that I've named it radius, height and length. I also have another one set up in sketch two but the point is, is I've actually labeled these.
Now, you don't have to do this, you could use the variables that Inventor creates automatically. If you remember from our parameters movie, Inventor will start with D0, and then continue incrementing it D0, D1, D2 for every dimension that's created in Inventor Model. So, what I've done is name these something meaningful so when I get to creating the eye part it makes it a lot easier to actually see what I'm working with in the table. I'm going to go ahead and right click, go back to dimension and display, and set this back to value, and then I'm going to hit finish sketch to return to the model.
We're now ready to actually create the eye part. To do this, we'll go to the manage tab, and we'll go to the author panel, and within the author panel, you have a create I part button, that'll bring up the I part authoring window, and this provides a lot of capabilities that we won't cover here completely. Really for this essential course, I want to just make sure you understand how to create an I part and some of these things you can do with these different tabs, but there's a significant amount of power here that we won't be able to cover in an essentials course completely.
What you can see is on the top, you have parameters and properties, work features and threads, and we'll cover threads a little bit but the remaining items won't be covered in this course. On the left here, you see the part along with it;s features, and you'll notice that the variables or dimensions that I renamed are listed here, Diameter, Height, Length, and Radius. Here's D4 as well, so even those variable that have not been renamed will show up. What happens though, is the items that have been renamed you'll notice have been moved automatically to the right hand side, and are represented in the table down below.
This is important because you can use this movement back and forth between these two panels to control the order of items within the table. For example, because I know I really want to be able to pick this part based on length and height, I want to have the length and height at the top of this list. So I'm going to go ahead and select Radius, and then I'm going to use the double arrows to select it. And then I'm simply going to select it again and move it with the double arrows to put it back over to the right hand side. What you'll notice is now I have length, height, diameter and radius in order just like they are from top to bottom: length, height, diameter and radius, and the reason for this is just for organization.
It, it just makes it a little easier as we start adding different rows to this table to be able to have em in the order most important to your design. The other item as I mentioned, since length and height are the most important, I'm going to go ahead and flag these as key items. You'll notice that the keys here on the left are grey. What I want to do is, I want to right click on length, use the key flyout and select 1. You'll notice that it becomes blue, and a key is added to the table down below, and you'll see why we're doing this in a moment. In the intro video, you saw me selecting things based on length and height, and hopefully you saw that video, and you can understand this already, but otherwise I'll, I'll circle back and show you when these keys come in handy when we are finished here.
Next I want to right click on height and do the same thing. I'm going to select the key fly out and look at key number two. You'll notice key number one is in hard brackets or square brackets which indicate it's already assigned to another item, so, I'm going to go ahead and select Key 2. Now that we have the keys set, we're ready to begin adding additional items to this part. If you right click on row one and select Insert Row, Inventor will automatically create a new row with the exact information that you had in the previous row with one exception, or a couple exceptions.
You have a member name and a member number. You'll notice that Inventors use the name and a sequential number to identify each of these items. Now, in a commercial market, most of these parts are going to have a unique part number that you might want to make as a key. In this case I don't have a unique partner number, so I'm going to leave the number inventor has put in for me. But just know that you can highlight these and change these part numbers to identify unique part numbers. What I want to do now is update some of these values while the names of the variables aren't going to change, the sizes will based on each variation.
So I'm going to go ahead and set the length of the second item to 2.5. I'm going to set its height to 1 inch, I'm going to go ahead and bump the diameter up to 0.5, and I'm going to bump the radius to 0.325, so I now have two variations. I've got handle one and handle two that are slightly different in size but generally keep the same shape. I'm going to continue on by right-clicking again and selecting Insert Row, and this time, I'm going to leave the 0.25 length.
But I'm going to change the height to 1.5, and I'll go ahead and I'll leave the diameter and the radius the same. Let's do this one last time. I'll right click on row 3 and select Insert Row, and I now have handle 4. I'm going to bump this length up to 3 inches, let's bump this up to a two inch in height, and we'll leave radius and diameter alone. So I now have all of the variations that I want in this table, and there's one item remaining that we need to do to complete this.
Now this might be going a little bit beyond an essentials course, but I think it's something that you may run into fairly quickly with parts like this, and I want to call it out here just so you are aware that it can be done, and that is, talk about the threats. As the size of this handle increases, the diameter increases a little bit and the radius increases a little bit and because of that I'm going to go ahead and bump up the thread size in the holes in the back of the part to accommodate that larger size.
So, I'm going to go to the Threads tab by left-clicking on it and you'll notice that I have a hole designation already called out because that hole is already threaded, it knows that the designation is currently a quarter 20 UNC. I'm going to go ahead and select that by left-clicking on it, on the left side of the window, and use the double arrows to the right, to move it into the table itself. By doing this, you can see whole designation has been added to our table, and we have quarter twenty unc listed for all of this. Now, based on this diameter, I know that these remaining three wholes on the bottom are actually going to be a little bit larger.
So I'm going to change the whole designation for those, I'm going to set these to 3 8ths 16. Let's go 3 8ths, and let's change this to 16. Now that I have that code set in, I'm going to highlight it in the table, use Control C on my keyboard to copy it and then simply paste it into the remaining items. Because I know the first hole is going to be a quarter twenty and the remaining are going to be larger. With that said, I can hit ok, and you'll notice that in the browser now at the top, we have a table.
And the reason this is important is because this part is now officially an iPart. This table at the top of the browser, if you hit the plus symbol next to it will list the variations we have, and you have the ability to double click on each of these to switch between the different values. And inventor is automatically updating the dimensions in the background based on the values that were in that table. Now the one thing that's different at this point from what you saw in the previous introduction movie, is that right now inventor is listing these items based on the member name in the table, handle one, handle two, handle three, handle four.
Now, in a commercial environment, this is probably the way you're going to want it because you're going to look up a unique number, and based on that unique number, you know the sizes already. In my case, because I'm not a commercial market, I'm more interested in the key values that I set, I want to be able to see the length and the height when I'm selecting this part. To make that change, all you have to do is simply right click on the table, and select, list by keys, and that's simply a toggle. If I right click on it again, you'll see, list by member name, so, at any point, you can toggle back and forth, as needed.
I'm going to go ahead, and hit list by keys, and now you can see we have length, which was key one lifted first, and, you can see we have a two inch, a two and a half inch, and a three inch model. If we expand each of these, you can see the variations that exist for key two, and, the length 2.5 version, we have two variations. We have one with a height of 1 inch, and one with a height of 1.5 inch. If you right click on the table and select, edit table, we can bring that dialog box back up, and you can clearly see how these are related.
In the length column, we have a 2 inch, 2, 2.5 inch, and a 3 inch, and within the 2.5, here's the 1 and the 1.5, and you can see that those all line up perfectly with what you see in the browser. So based on a little work, you can actually use one part to actually generate multiple variations of the same type of part. When placing this part into an assembly, you'll have the ability to use these values from the table to select which part you wish Inventor to place in the assembly.
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