machined crank slot I tryed a projected curve , it is similar to a ford typ a crank shaft.

svenolov_nystrom · November 2022

Any clue how to make it

svenolov_nystrom · November 2022

I think I made it with a loft on projected curv, It looks ok , will see if it can be used as path for milling.

steve_shubin · November 2022

@svenolov_nystrom

Look through the various tabs in the two documents below

Maybe something in one of these docs will help

https://cad.onshape.com/documents/a4b977957f6c9823b3e6034d/w/65b9d18f8bfae13389db1e7a/e/f9aacfc089b3e7a96eec599e

https://cad.onshape.com/documents/99f6268ff6f2fdab48956e49/w/8d8060ee3e7d269899840f80/e/0051fee4c161a9d223f8f335

svenolov_nystrom · November 2022

The wrap seems to work but I dont have the right feeling, there must be some way get more control over placement, it cant be that difficult. Thank you

steve_shubin · November 2022

@svenolov_nystrom

Take a look at the 3 GIF's below.

The Wrap feature takes sketches with CLOSED shapes, meaning those shapes showing a gray area within a sketch, and places those closed shapes on the side of a cylinder, as if one were placing a decal on a window

Regarding the Wrap tool in general, you could certainly make things easier if your were to sketch shapes on a plane that is out in front of the cylinder. This will likely allow you to avoid having to play with the positioning within the Wrap dialog box, provided you position the shapes within the sketch.

When it comes to ANGLE, U SHIFT and V SHIFT, things can be a bit to grasp depending upon orientation. But once you get the general idea, it doesn’t take all that long to see what is what.

So in the GIF’s with the vertical cylinder centered on origin, and sketch on the front plane, Onshape will initially place this wrapped shape on the back side of your cylinder.

To remedy this, you can reposition the shape within the Wrap dialog. And provided you sketched at the end height you want, then you likely will only have to adjust the U SHIFT and ANGLE

At least in this case, U SHIFT is with regard to the CIRCUMFERENCE. So if the circumference of the cylinder was 6, and you wanted to get a mirror image with reference to the front plane, then you would set U shift to 3, which would rotate the shape half way around the cylinder to the front, and ANGLE to 180° for the mirror effect.

In the 3 GIF’s, I show how one end of the slot was placed in-line with the right plane.

If by chance, you did not want one end of the slot in-line with the Right Plane, then you would distance your closed shape within the sketch however many inches from that right plane.

In the below GIF, I first copy the circumference, then paste it into the U SHIFT field. Then divide it in half in order to rotate it half way around to the front. Then I enter 180° into the ANGLE field to have it mirror the position it was on the back

steve_shubin · November 2022

@svenolov_nystrom

I moved the sketch from the front plane, to a plane I created just IN FRONT OF the cylinder.
In doing so, I eliminated having to do any positioning from within the Wrap dialog box,
as the shape now wraps onto the front of the part from the get-go.

Now you have an easier way of positioning the slot, and all done from within the sketch.

So the key is, to create your sketch on a plane in front of the cylinder you want to wrap.

matthew_stacy · November 2022

svenolov_nystrom said:

Any clue how to make it

@svenolov_nystrom, I approached this part with the intent to manufacture it on a mill-turn type machine, with the workpiece translating and rotating relative to a spinning end-mill. Thus the slot terminates with a radiused end.

Assigning a measured variable for shaft diameter provides a useful parameter for modeling the slot. I used a mate connector to sketch the slot on, properly offset (by 1/2 the shaft diameter, previously captured) and oriented. That diameter variable can also be used to define the extent of the slot based on an angular value rather that a linear distance.