Making a locking mechanism slot along a cylinder

adam_mercier

Hello all,
I need to make a lock mechanism for a air impact canon for automotive testing. The goal is to compress a O-ring and lock the blue part to the gray canon with quick disconnect capabilities for projectile loading using the red pin. I cant find any way to make a slot with its direction oriented radially to the gray cylinder. I think doing that is impossible without 3D sketching ? 


This is obviously not correct :



I hope there is a way I did not think about

best regards, Adam

Nickolas_Lockard

I have similar struggles. Extrude-remove does some weird artifact faces:
 

I'm trying to compress a washer ring with the yellow locking collar at top (WIP). The only thing I've found works is to manually move faces along new sketches, but it's unreliable, clunky, and slow.

I really would love 3D sketches. It's a constant struggle as most of my tool designs go beyond simple helices. We need to be able to sweep along a complex curved path!

But for yours, if you want the faces to align radially, you can use the move face function (rotate) around an axis that is down the bore centerline. Then just use pattern tool to get more locking pins and slots.

adam_mercier

Thanks for the tip, that worked even if its quite unprecise! Now drawings are giving me issues tying to dimension that correctly for production...

øyvind_kaurstad

This is an interesting case. I was just about to draw something along the same lines (a rotational locking mechanism), but I haven't started on it yet. Then I discovered this thread, and I realize that there might be no precise and good way of doing this.

While the move face function can be used, it involves eyeballing (or calculations of which angle of rotation is needed), it is far from ideal. Is that the only way to achieve this? Would be nice if someone at Onshape could comment.

tom_scarince

The ideal solution would be the ability to do a "solid sweep" of a cylinder along the path of the slot.  I'd venture that most cad packages do not have this ability. 

The alternative in your case would probably be to create the two rounded-end slots parallel to the axis first.  Then create a helical path connecting them and sweep a 2d profile of the cylinder along that path.  The profile has to be perpendicular to the start of the helix.

I'll try mocking it up when I get a chance.   

adam_mercier

Yep I think solid sweep could solve this issue BUT that would involve a way to build the sweep path with 3D sketching, I tried for a while to build a path with multiple sketches and planes but it was quite a struggle to get everything lined  (I did not manage in the end)

Please let us know if you find a solution!

Adam

tom_scarince

I tried it last night, made a mess, and saw where I went wrong.  I think I can get it next time. 

tom_scarince

Ok, got it to work.  Public document here 



Key points are that the two straight slots were created, then a helix segment between the center points of the circular end of each slot.  I then created a "curve point" plane normal to the start of the path by selecting the helix and its endpoint.  A rectangle representing the cross section of the slot was drawn there and then swept along the helix.  

The model is robust - the angle between the slots is driven by a variable and the (fractional) number of turns of the helix  is calculated from that angle.  Offset planes are used to tie the slot end points to the helix cylinder.  

Lemme know what you think.  

øyvind_kaurstad

Good job! Very nicely done!

henry_feldman

tom_scarince said:

Ok, got it to work.  Public document here 



Key points are that the two straight slots were created, then a helix segment between the center points of the circular end of each slot.  I then created a "curve point" plane normal to the start of the path by selecting the helix and its endpoint.  A rectangle representing the cross section of the slot was drawn there and then swept along the helix.  

The model is robust - the angle between the slots is driven by a variable and the (fractional) number of turns of the helix  is calculated from that angle.  Offset planes are used to tie the slot end points to the helix cylinder.  

Lemme know what you think.  

Wow, nice job. This might actually make a nice tutorial video if you could package it up. There are lots of variations of this that would be helpful, since this was a hard-won lesson!

tom_scarince

Thanks for the kind words.  Maybe I'll try to put together a video. 

tom_scarince

Ok, so I'm not gonna be the next viral youtube star, but I hope this helps:
https://youtu.be/zLyrZ6OSUvQ

adam_mercier

That's quite impressive! thanks for your time!

øyvind_kaurstad

Nice that you took the time to do that.

However, while your solution is clearly correct, I find it quite hard to mentally picture why the cut needs to be helical. If the cylinder was just rotated or translated axially, then the cuts would be straight, but when it does both at the same time, the cut must be helical. I see that this is exacly analogue to a screw/threads, but somehow I find it harder to visualize. It might be due to the knowledge that the pin is always normal to the cylinder surface in every position, and therefore is is difficult to imagine that the cut in the sidewalls of the cylinder needs to be helical to fit the pin.

Anyway, probably just some mental defect in my brain.  :-)

marten_hutchison

The key for me was creating the plane at the helix end point - Plane > Helix Vertex + Helix Edge, Curve Point (plane type).  If you have issues with the Sweep not wanting to generate, go back to the Sketch of the profile you want to sweep and eliminate unnecessary constraints.  For instance a Horizontal constraint may conflict as OnShape tries to sweep a line around a helix.