The Insert Part command is used to add one or more solid bodies (parts) into an active part. This is not the same as creating an assembly, although there are certain similitudes about the way the inserted part is oriented using the Locate Part dialog.  The big difference, however, is that what we end up with is a multi body part, that allows no movement of the bodies relative to one another, and that could very well be combined into one single body.

So, how do we insert a part into another part? It’s not really hard, as a matter of fact. I’ve prepared a little example, using one of the screwdrivers from the Indent video tutorial.  I start with a new part document, although it doesn’t necessarily have to be that we insert the part into a new or empty part document, but I thought it would be easier to explain this way.  Anyway, back to the example…  First, you need to open the part document where we wish to insert a part, then select Insert, Part, and browse for the part you wish to insert into the active part document. In this case, I chose a file called screwdriver1.sldprt, which is the largest one of the three screwdrivers. An Insert Part property manager will show up on the left. From this property manager, make sure to select from the list whatever you want to be transferred with the part once it is inserted in the active document.  Your part will be inserted as a dummy part, which means you’ll have no access to the history or the features of the part, but you can still transfer planes, axes, dimensions and even sketches.  Also make sure that you select the option Launch Move Dialog, under Locate Part in the property manager, as it will aid you in the process of orienting the inserted part in the active document.

There are two ways to locate the inserted part, by translating or rotating it, or by adding mates, just the same way it’s done in an assembly.  You’ll have to choose between the two; unfortunately, you can’t add a mate between two planes or two faces, and then go and translate the part. It’s one way or the other.

So, for this example, after selecting everything I need transferred with the part, I simply clicked OK to place the part at the origin of the active part document. You don’t need to do it this way, you could just drop the part anywhere you like, but it’s easier for me to do it this way because I’ll have an instant reference in the origin of the active part and any distance mates or displacements will be easier to appreciate.

OK, at this point, and since I had checked the option to launch the Move Dialog,  the Locate Part dialog opens, usually providing first the option to orient the part by using mates. If you scroll down to the end of the dialog box, though, you’ll find a button that says Translate/Rotate and that will toggle to the explicit translation/rotation method.  This Locate Part dialog is exactly the same as the Move/Copy Bodies dialog, that you can find and use at any time (not only when inserting a part) by clicking on Insert, Features, Move/Copy or on the icon in the Features toolbar, if you have previously included it there, that is.

In this example, using the mate method, I’m applying a coincident mate between the Front plane of the active part document and the Side plane of the screwdriver. 

Next, I move the screwdriver four inches away from the origin by adding a distance mate between the Right plane of the active part and the Front plane of the screwdriver.   Notice that doing this would not be possible if I had chosen not to transfer any planes when I first inserted the part.

If I now press the Translate/Rotate button at the bottom of the dialog, any mates I had applied will be lost and the inserted part goes back to its original location.  Personally, I don’t like this method too much, because you can’t really do a translation AND a rotation in one single step, you are once again forced to choose between both, although it can be useful too.   To translate the inserted part, type the Delta X, Delta Y and/or Delta Z values in their corresponding fields. I typed 5 inches on Delta X, to move the screwdriver 5 inches along the X axis. This value can also be negative, to move the part in the opposite direction.  You can also select an edge to define the direction of translation and a distance or you can choose a vertex in the graphics area, then click on a second vertex and the part will move the direction and distance specified by those two vertices.

To rotate the part,  enter coordinates x, y and z for the rotation origin, that is the point the part is going to rotate about, then enter a value for the rotation angle around either of the three axes (or even all three of them). If you don’t specify any coordinates for the rotation origin, the inserted part will rotate around the origin of the active part document. Either way, you’ll see a yellow dot in the graphics area, indicating where the location of the rotation origin is. You can also select an edge in the graphics area to serve as an axis and specify an angle of rotation around that axis, or select a vertex as the new rotation origin. In this image, I’m applying an angle of rotation of 90? around the X axis. A preview of the image in its new position will show up and you’ll be able to judge if you’ve positioned the inserted part according to your needs or not.

One last thing, if you were wondering what the Constraints button at the bottom of the dialog does… It will toggle back to the mate method.

The rest of the screwdrivers were added in the same way, and located by placing mates between them and the other bodies previously inserted.