Curve Pattern - feature pattern including full part

itai_ofir

Hi all,

I am struggling with using Curve Pattern, maybe someone here can point out what I'm doing wrong - I want to pattern a gear tooth along a spiral curve. When I use "feature pattern" however, it looks like it's patterning the whole spiral part that the tooth was extruded on:

(I first had a spiral created, and then extruded the gear tooth separately as an "add")

If i choose "reapply features" then it does pattern only the tooth, but it is offset the same distance is the whole part (like shown above in red):

(see the floating tooth on the right)

If I increase the instance count then the offset becomes very clear:

link to document (first time sharing so hope this works):
https://cad.onshape.com/documents/7fa1e1f24aa60458338eec80/w/2577a64410c0efdb24cdc536/e/d20de3024538f88b7750edbc?renderMode=0&uiState=67766a111955952905a9765b

All help appreciated 🙏 I just want to make nice spiral gears 😶

glen_dewsbury

I got the tooth pattern working sort of. but not able to get position correct. Notice the drift as it approaches the center due to the curve tightening up.

https://cad.onshape.com/documents/3d6ccb7b2779ba46705e31f0/w/44009d17253b47d6f6fc285f/e/fcedf40f7acde6e400d1b1e9

glen_dewsbury

I got the tooth pattern working sort of. but not able to get position correct. Notice the drift as it approaches the center due to the curve tightening up.

https://cad.onshape.com/documents/3d6ccb7b2779ba46705e31f0/w/44009d17253b47d6f6fc285f/e/fcedf40f7acde6e400d1b1e9

MDesign

That's interesting. looks like its slowly losing it normal to the curve.

glen_dewsbury

There is no normal or tangent to the face because the curve as tightening. Another way has to be found for tooth definition.

MDesign

right I wasn't suggesting to make it normal. just an observation

glen_dewsbury

Unfortunately the curve pattern only allows normal or tangent. I've made an over lap to compensate. Also because of the tightening curve the teeth are getting closer together.

This looks better but if it's supposed an actual gear tooth wellll… keep working on the tooth sketch.

https://cad.onshape.com/documents/3d6ccb7b2779ba46705e31f0/w/100c2221673a48779a4dfe94/e/fcedf40f7acde6e400d1b1e9

itai_ofir

https://forum.onshape.com/discussion/comment/111596#Comment_111596

Thanks for the tip! So extruding the tooth separately paired with 'part pattern' is able to actually follow the curve, then 'merge all' takes care of connecting all the instances cool cool cool

The orientation not matching is kind of a bummer, but i think I have an okay workaround for now - I set the 'distance' param on the curve pattern so it doesn't go all the way down the spiral:

Up to the point I stop at the teeth are still aligned close enough, and it ends about where is practical for a gear so I guess this is okay for now.

Like in Glen's post the missing orientation also created gaps between the teeth and the spiral, I was able to work around this by adding to the original tooth extrusion so that it has some extra material to fill the growing gaps:

Would still love to have 'feature pattern' working for the curve with correct orientation but with some more tweaking this should be good enough for my purposes right now.

glen_dewsbury

Setting distance and count kooks like a better option. This part pattern is using an overlap of the tooth to compensate for the tightening curve.

I suspect that if you want to use as a gear that each tooth profile needs adjusting to suite change of radius. Maybe some one that has more experience with odd gears can help with that. I haven't done odd gear shapes since a project in school (1979). Made elliptical gears to get change in velocity during each rotation. Made my model teeth from plastic and a file.

itai_ofir

Wow getting good gear teeth with a file sounds like intense work! I'm very interested in the effect odd gear shapes have on motion (which brings us here),
I played around a little and think I got something that might work, will have to print to test it out:

Tried the same technique to make some ridges through the spiral but that doesn't work nearly as well. Besides the fact that patterning doesn't adjust the length to fit in the spiral, the offset seems even more pronounced here:

I should probably find a different approach for these ridges…

glen_dewsbury

I the ribs are to be matched with the curve then this works. Still has some drift of course.

https://cad.onshape.com/documents/3d6ccb7b2779ba46705e31f0/w/100c2221673a48779a4dfe94/e/fcedf40f7acde6e400d1b1e9

itai_ofir

HI, wanted to give updates on further experiments with the curve pattern:
After some lots of tinkering I was able to get a parametric curve of a line (using the parametric curve FS: https://cad.onshape.com/documents/578ff8b3e4b0e65410fcfda3/w/d33395f174e5b38f4abd6097/e/cc0c3d5644a78b1b64d6c3b4 ) by using the same functions used to make the spiral but with only 2 points (so a bridge is created between turns of the spiral). After looking through some tutorials on variable pattern features, I was able to set up the variables for the functions such that the curve pattern changes the length of the line to match the decreasing spiral radius.
Tutorials used were the Pretty Pattern document and the Variables In Patterns from Tech Tips:
Pretty Patterns | Variable Patterns Tech Tips

Even more exciting when I project the parametric line into a sketch and add a mid-line with variable distance, the sketch is able to follow along with the curve pattern in feature pattern:

This is with using 'feature pattern' when including all variables, parametric curve, and sketch together with 'reapply features'. The instance variable increases with each reapplied pattern, moving the parametric curve down the spiral with corrected length, and the patterned sketch moves along from the new projection.

My current block is that as soon as I add curves to the projected rib sketch, which I would eventually want to sweep to form the ribs, the sketch patterns incorrectly:

Even though it looks like the parametric curve still patterns correctly. What's also interesting is that the inner ribs seem to realign at some point.
My alternative strategy would be to create a parametric curve like the straight ribs, but one that is curved as desired. After a while spent with chat-gpt and a graph visualizer the only thing I earned was a headache so going back to trying with patterning a sketch.

I'm assuming that something in sketches is incompatible with feature pattern, things always go bad as soon as I add a curve of any kind (spline, bezier, conic, etc..) leaving link to the doc in current state:
https://cad.onshape.com/documents/7fa1e1f24aa60458338eec80/w/2577a64410c0efdb24cdc536/e/103d3131ad09160a8b7879b6?renderMode=0&uiState=6779649bd3518f0be5096c51

itai_ofir

Hi all, haven't made too much progress this week but found further odd behavior with curve pattern - when I "skip instances" the sketches are patterned differently:

Maybe if I skip the right combination of instances I might get something close to right but this feels like just working around a bug 😅

Can someone tell me how I can open a support ticket?