Hi all, I've been wrestling with the Swept Cut feature for a few days now and still am not getting quite what I want.
In my past experience making custom threads (using Pro/E), the machinist likes to see two things in the drawing: the thread profile and the thread path. This is because he/she will make a cutting tool according to the profile and use this to follow the thread path on the lathe with whatever settings are required to get the desired pitch.
In SWX the closest thing to a thread path I've been able to find is a Helix/Spiral defined by Height and Pitch (even though the pitch will be constant), wherein I alter the diameter at a given height. This is not only unnecessarily complicated but it doesn't give you much control over the ultimate thread path.
This option is similar to a custom thread path and a step closer to what I'm used to, but there are some inherent flaws:
1. You can't define the geometry at the intersection where the diameter of the helix changes, as depicted below:
2. With Cut-Sweep the cuts can't overlap each other. This seems logical until you think about how the threads will ultimately be formed on a lathe. The cutting tool will actually be wider than the pitch as shown below. Lets say you want your threads to end in a conical fashion. When your cutting tool is coming down (or up) the "ramp" the material behind (or in front of) the form tool will be higher than the thread depth. You really need to allow some "overlap" (i.e. the cutting profile to be wider than the pitch) to overcome this. I'll try to draw something up to illustrate (assume pitch is 1.1 and I haven't drawn the spacing to scale I'm just showing two different threads):
Your cutting profile needs to be wider than the pitch in order to get the desired thread width.
Hence there seems to be no way that I've found, with a conical-tipped screw and variable thread diameter, to model the part the way you actually want it to be machined.
Now below is a screen grab of my ultimate part. This is pretty close to what I want except the teeth should actually be a bit thinner and the bottom flats a bit wider. However I can't model this without running into the problems mentioned above. How in the world do I model this part using the ultimate desired geometry?
Only thing I can think of is to do two cut-sweeps using the same helix but, c'mon SWX there's gotta be a better way.
Thanks to everyone for the contributions. I'm going to step through the solution that I ultimately found to be most elegant.
Briefly I'll follow the method shown in the video here to create an intersection curve to define my path then sweep-cut the thread profile along that.
I'm starting with my screw "blank" solid geometry shown below but I will hide the solid body or make it transparent in some steps to make the other features easier to follow.
1. Sketch the thread path and revolve it as a surface.
2. Create a helix of the appropriate pitch and length and pierce a straight line to it. Use the line and helix to sweep a surface.
Note that to create my helix I made a plane 3mm (same as my pitch) in front of my part which is also where my thread path ends.
3. Create the Intersection Curve (Tools - Sketch Tools - Intersection Curve) and select the swept surface and all the faces on the surface revolve. Once that's done another response recommended turning the 3D curve into a Composite Curve for better results, although either seemed to work fine for me.
4. Now just sketch the thread profile and cut-sweep that along the resulting composite curve. With the path now defined I prefer to delete the unnecessary surfaces (Insert - Features - Delete/Keep Body) but I suppose you could just hide them.
When performing a cut-sweep along the composite curve or intersection curve you must select a direction vector under Options.
Also, in order to get the desired tooth width I had to do two cut-sweeps using the same path. Otherwise the thread profile would be wider than the pitch at the conical portion of the screw resulting in self-intersecting geometry. This may not be necessary depending on your screw parameters.
And that's pretty much it! Seems like a lot of steps just to get a thread path that will update when you change the sketch. Altogether a handful of additional features are required (Surface-Revolve, Helix/Spiral, Surface-Sweep, 3DSketch & CompCurve) but the final design will be more robust and the drawing will be that much easier to make.