how to draw a twist-lock slot?

[cmm]

How do you draw a twist-lock slot (e.g. the kind often used in quick-change tooling)? What I mean is a slot (in my case, one of constant depth) milled on a cylindrical surface that starts out pointing in the axial direction, makes a sweeping 90 deg turn to the right or left, then follows the circumference for some distance.

 

[brengine]

For this Example, I assume a Sketch of a circle on the Top Plane, and Boss-Extruded to desired shaft length. Define an Axis at the intersection of the Front and Right planes, this will also coincide the centerline axis of the cylinder/shaft (but I won't be using that here).

Put a Sketch on one "capped/closed" end of your shaft (probably the Top Plane). This Sketch can be composed of a circle/closed arc at the slot location and its profile, make sure the center of the arc is COINCIDENT with your Right Plane). Cut-Extrude to whatever length you want the slot.

Now for the 90degree portion, put a Sketch on the Right Plane. Again draw the profile of your slot, with the center COINCIDENT with the cross-section line where your first cut ended. Draw a construction line COLINNEAR with the Axis defined above. Now Cut-Revolve the Slot Profile to whatever angle you want.

If you want the end of the last slot "round", then put a Sketch on that Face (at the end of your 2nd slot). Draw 1/2 of the slot profile and Cut-Revolve it around a Reference Line down the Middle of that face.

Is this Close Enough?
Ken

 

[cmm]

Thanks for your reply Ken. This twist-lock slot I have in my hand unfortunately is different than the one you describe. The 90 degree turn is not sudden--it sweeps an arc. Any idea how to do that?

What would really be cool is if I could sketch the profile in 2D (which would consist of a line, 90 deg bend, line) and then wrap the profile around the cylinder. Can Solidworks do anything like that?

 

[BBJT]

You could create the cut in a flat piece and roll it up using sheetmetal. BBJT CSWP

 

[rocheey]

You can "untwist" a helix onto a 2D plane: a standard helix would unwrap to something that resembles an unrolled carboard toilet paper tube. Start with a vertical line, whose length along the Y axis is equal to the part's circumference. Draw 2 lines from there, whose angles are the
helix angle (supplement of the lead angle). Cap off the other end with another vertical line of a circumference's distance.

Since the helix angle is a function of pitch and diameter, any change in either of these changes the helix angle.
For example, to have a constant outside diameter and an ever-changing helix along this diameter, replace the 2 angled lines with arcs, whose diameter is tangent to the start and endpoints of your helix, and tangent at their start and end helix angles (draw a circle using 2 tangency points).

 

[brengine]

O.K. then, try it this way...

1)
For this Example, I assume a Sketch of a circle on the Top Plane, and Boss-Extruded to desired shaft length. An Axis at the intersection of the Front and Right planes would coincide with the centerline axis of the cylinder/shaft (but I won't be using that here).

2)
Put a Sketch on the Right Plane, and then like you said:
"sketch the profile in 2D (which would consist of a line, 90 deg bend, line) ",
make sure you close the sketch lines at the ends, then Cut-Extrude all the way THRU in the direction TOWARDS your desired slot.

3)
Now insert a 3D Sketch (by \Insert\3D Sketch if you've never done it). Looking at your cutout portion, Select each of the line Segments on the SURFACE of the Cylinder, and hit the "Convert Model Edge or Sketch Entity to Sketch Segment" button on the Sketch Toolbar. Close the Sketch. This will be the Guide Path for a Cut-Extrude-Sweep (later).

4)
Create the a Boss-Extrude to fill in everything that just got cutout. I just did exactly the same thing I had done in the first step. Or you could repeat the 2nd step, but Boss Extrude the Profile.

5)
Before you can do a Cut-Extrude-Sweep, you also need to have a Sketch of the Profile. I made a Sketch (another one) on the the Top Plane, that would be the cross-sectional Profile of your Slot (I used a circle) where the center of the Profile COINCIDES with the one end of the 3D Sketch. Close the Sketch. This will be the Profile for the Cut-Extrude-Sweep.

6)
Now insert a Cut-Sweep (by \Insert\Cut\Sweep if your button isn't active on the Features Toolbar). Select the appropriate Profile and Path Sketchs and there you go!

Not the pretty'est, but it should get the job done.
Ken