I receive infrequent questions on how to perform advanced features such as seen on some of the models I've made. Of them, the most common is how to feature threading, coils, and helices. This page explains how to place them on your models.
I will explain the process using Solidworks 2006 and Autodesk Inventor 10. Generally speaking (in my opinion) Inventor has an easier interface for commands and operations, however Solidworks seems to be a bit less discerning on thread errors (as explained).
There are many ways to get the same job done in both programs; the path I follow on this page is just the one I use to modify the parts. For the most realistic appearance, you will want to "remove" material from the solid model instead of adding to it. The program will give you the option of adding the threads if you want but this isn't how the actual parts are made in reality, and as a result won't look right. I've noticed most people find it easier to imagine adding the thread to the part at first (myself included), but it's not as realistic so I suggest avoiding it.
Additionally, for realistic purposes, the thread shouldn't be placed in 100% engagement on the hole. Meaning, not all of the thread is applied to the hole when finished. This is due to tolerancing and surface finishing reasons. Whether or not you will want to do this depends on the scope of the model you're making, whether it's supposed to be more realistic, or show more of an example thread profile.
Solidworks:
For the purposes of this I will just use a sample part with some "holes" drilled into it, ready for threading. The part looks like this:
I cut the part in half to show the threading plane easier. You can do this while performing the operation then delete the extruded cut feature afterwards if it helps. Otherwise, switch to wireframe view.
The hole is drilled up through the bottom of the part and has a chamfer on the end. The chamfer isn't required but it's more realistic to the machine threading process, and also looks better in the end. You can add the chamber by using its command in the features menu.
To create the thread, you need to make a sketch profile for the material to be removed, then sweep/cut it on a helical profile. The thread sketch should be a triangle if the threads are standard, or a trapezoid if ACME, etc. Most threads tend to be standard, which are usually an equilateral triangle (which you can draw with a line using a fixed relation parallel with the hole, and dimension the other sides to be 60º). The height of the triangle depends on the thread pitch, or threads per inch.
(Please note that the 60º triangle isn't totally accurate to the real thing, however it's pretty close. In reality the triangle is shifted to the side so it "wraps" around the center axis. You can imagine it as being 59/61 degrees instead of 60/60.)
After the sketch is made, you'll need to apply the helical profile for the sweep cut. If you don't have the Helix command in your taskbar (or other toolbar) then you can find it under the Insert menu.
You will then be prompted to choose a plane for the helix. This plane is where you will place a circle to show the shape of the helix. For instance if the hole is on the bottom of the part, then you will want to insert a circle on the bottom face of the part, with center point in the middle of the hole.
After the plane is established, you will be presented with the helix profile shape options. These determine the pitch and length of the helix, amongst other things. The helix pitch is the distance it takes for the helix to circle all the way around once; you can think of it as the width of the threads.
When you're done adjusting the helix profile, click on swept cut on your toolbar or in the menu. The box "profile and path" pops up. Click on the thread's 2d sketch first (profile) then click on the helix you just made afterwards (path). You can go back and edit the operations you want to use if you click on the wrong part.
After the two have been selected, you'll see a 3d plane showing the result of the helical cut. It looks something like this...
Then, when finished, you end up with this:
Nice!
Inventor:
For this I'll use another sample part to show the threading operation, looking like this:
Again cut in half...
I did something different here. I applied the chamfer within the revolved feature on the bottom of the part, instead of using the chamfer feature command to add it later on. Doing this reduces the number of features on the part so I prefer to do it.
The threading process in Inventor is similar to Solidworks, however a little bit streamlined. You will make the same thread profile sketch for the thread to be removed. Then you'll use the coil command to wrap it around an axis. The shape of the thread sketch will be the same as described above (triangular, dimensioned the same, etc).
After the thread profile is made, you have a choice. The axis for the coil command can be sketched into this operation, or you can make an axis for it afterwards. It doesn't matter. I choose to make the axis part of the thread sketch, which you can do by drawing it in with a regular line. Use the Project Geometry command to pick out a background feature, then object-snap the axis line to its centerpoint.
If you don't do this, you can exit the sketch then click on the axis command on the toolbar or under the menu. Click on the hole you want to add the threads to, and the axis will appear.
Either way, when you're done, click on the coil command on the toolbar or the menu. You'll be prompted to select the profile and the axis; if the only closed profile you have is the one you just made, then it'll be selected automatically. Click on your axis after it, either the one you drew into the thread sketch, or the axis you made using the axis command.
After you've selected a profile and axis, a preview of the thread shape will appear. Be sure to select the "subtract" option or you'll end up adding to the profile instead. Click on the coil size tab to adjust the thread pitch and length, as described in the above SW instructions.
When finished, perform the command and you'll end up with this... (which are 10-32 threads, by the way)
If you received an error about self-intersecting profiles after trying to apply the thread, go back to the thread sketch and move the inside edge of the triangle closer to the wall of the hole. The problem is the edge of the triangle is overlapping with itself when it coils around, so you have to remove the excess part of the triangle and make it so it won't intersect itself. This is the problem with making "realistic" threading that doesn't cut from the whole thread profile, but is better overall. Solidworks doesn't seem to mind these intersections much, if at all.
