Hi! This is the short and sweet version of
creating threads in FreeCAD 0.19 pre-release. I'm using the February 14th pre-release of 0.19 I've already created a cylinder that i'm going
to attach the thread to, just to save time. The important thing to know about this cylinder
is that its outside radius is 20 millimeters. Let's create, in the XZ plane, the thread profile. I'm going to create a thread
profile I like to use... ...45 degree angles top
and bottom, in a trapezoid. One millimeter for this middle part. 1.25 millimeters for this part. That is so I can embed this a little bit and still have a millimeter
of thread sticking out. If we make it, the end of the thread, 21
millimeters, that's embedded a quarter millimeter. For this thread, I'm going to make this thread
six millimeters above the base of the cylinder. (renaming the Sketch to 'thread profile') Next we're going to leave the
Part Design workbench where we've been working and go to the Part workbench... and create primitives... We're going to create a helix. It's pitch, that is, the height from one
turn to the next, is four millimeters because my profile is three millimeters tall
and i want a one millimeter space above it. The height, the number of turns, here,
I want to do one and a half turns. That's one and a half times
four, is six millimeters high. I want a radius that puts it in
the middle of the thread profile, which would be 20.5 millimeters, half a millimeter beyond the edge of the cylinder. That's it, right handed. The next thing I want to do is bring
the height up to the right place. In the helix data, here, placement, position, I want six millimeters. Notice how that's in the middle of the thread. The next thing I want to do... is move the thread profile
and the path off the seam. I want to change the helix angle to 2 degrees.
Now the helix is off the seam. I need to do the same for the thread profile, but first I need to change its axis,
because it's in a different plane. Now you can see those two are aligned: The thread profile and the path are lined
up and they're off the seam of the cylinder. Next we need to go back to
the Part Design workbench. …and make sure that the body is the active body. We're going to make a cross reference
to the helix, called a Shape Binder. I'm going to do a Shape Binder to the helix. That lets us cross-reference the helix. It lets us talk about the helix from within this
body, which is necessary for doing the sweep. Now we can select the thread
profile and do the additive sweep. The Object we want to use is that Shape Binder. We want the things to be straight, so
we want to use Frenet orientation mode. ...and we're done! That's our one and a half turn cylinder thread. Suppose we want to do a three turn thread instead. To do that we need to go back to our helix, and change our height to just
less than one turn, like so. Then we're going to go back to the
additive pipe, that loop, the thread, and duplicate it with a Linear Pattern. We want to run it along the Z axis. We want the height to be
three turns minus one turn, so two turns times the four millimeter pitch
is...two times four, is eight millimeters. That looks good, so we click Okay, and there is our three turn thread. If you want to delve more deeply into all this, I have another video that's "Five
ways to Fail" making threads. That explains why Idid all the
things I did in this video. Have a look at that, and enjoy making threads!
