Cutting threads

GHamsz

I’m trying to cut a square thread and have come up against a strange issue. If I position the thread profile so it’s coincident with the helix such that the profile is outside the part I’m cutting the thread in, the Boolean subtraction will fail. If I move the profile into the part I’m threading a slight amount, it works. 

The orientation in this picture works, but if I move the profile so that the helix contacts the profile on the upper right point of the square it fails.

matthew_stacy

@GHammsz, I believe that positioning the swept profile (Sketch 3) coincident with the end-face of the part results in a zero-thickness condition at the start of the sweep (which is computationally problematic for reasons that are way beyond my pay grade).

You correctly surmised that moving the profile into the Part alleviates the problem.  My preferred approach is to do exactly the opposite, moving the thread profile entirely outside the part.  I did this by creating the helix on a construction surface that is longer than the part.  There are probably more elegant solutions, but I found this to be serviceable:

https://cad.onshape.com/documents/3054e049decbb2a502a7abcf/w/b55b518b37aadeaf6f4e39e3/e/2c494040ee2b872fc248dd9a

matthew_stacy

@GHammsz, I believe that positioning the swept profile (Sketch 3) coincident with the end-face of the part results in a zero-thickness condition at the start of the sweep (which is computationally problematic for reasons that are way beyond my pay grade).

You correctly surmised that moving the profile into the Part alleviates the problem.  My preferred approach is to do exactly the opposite, moving the thread profile entirely outside the part.  I did this by creating the helix on a construction surface that is longer than the part.  There are probably more elegant solutions, but I found this to be serviceable:

https://cad.onshape.com/documents/3054e049decbb2a502a7abcf/w/b55b518b37aadeaf6f4e39e3/e/2c494040ee2b872fc248dd9a

GHamsz

I didn’t think to move the helix longer than the part. I’ll give that a try.

thank

GHamsz

It worked like a champ, thanks...

doug_curtis

matthew_stacy said:

..........  I did this by creating the helix on a construction surface that is longer than the part. ...........

Matthew,  The technique you have described is exactly what I have been trying to accomplish but for the world of me, I cannot figure out the "construction surface".  I made a copy of your referenced model and I still cannot figure how you made the extrusion as a construction feature.  This would greatly enhance the use of the helix tool.

Any input is much appreciated.

Doug

doug_curtis

Added note, I am also trying to accomplish this on a tapered feature.

doug_curtis

ACK !!   I actually figured it out.  First time using surfaces in this system and a little more investigation into your example and I was able to get it.

Thanks !!

matthew_stacy

@doug_curtis don't you just love those VOILA moments?  We spend so much time beating our heads against the wall to earn them.  I speak from past/present/future experience ... and have the callused forehead to prove it.  A bit of tenacity goes a long way.

BTW, did you notice the #L=25mm variable in that model?  That associates the length of the surface (that the helix is based on) to the length of the shaft (to be threaded).  That trick is slightly more efficient to execute in SolidWorks because every parameter and dimension has a name and is directly accessible in formulas.

doug_curtis

@matthew_stacy    I actually was looking at it again today.  I ended up doing mine a little different. I did a surface offset at zero offset and then an extend boundary at a fixed distance.  I used a #variable for length in a configuration table and worked to calculate my helix based on that variable but the units was screwing with me.

Finally figured it out by making the length variable a unit-less number and adding the unit in the extrusion depth field. I was then able to still use the length variable in the equation in the helix turns field.  So no matter the length of my part, the surface is extended a fixed amount and the helix adjusts to the correct turns for the required threads.

I never used to many variables or formulas in SW as when I was using that, it was always for one off designs.