How to mate between a sphere ball and a rounded sphere groove in a cylinder

omri_r

Hi!

I'm trying to mate between a sphere ball and a rounded sphere groove in a cylinder in a way such that the ball would slide only within the groove.

Both the ball and the groove have the same radius.

I tired to use the tangent mate, but it does not do the work (I'm not sure why).

It seems there is some overlap between the ball and the groove (see images below)

Any ideas how to accomplish that would be very appreciated.

https://cad.onshape.com/documents/c1fb23babb4668e97ce5a361/w/8cd120f13393056585a21bf4/e/74d56c1158535498da0cb145

Thanks!
Omri

owen_sparks

*Edit for rubbish terminology used. 

I'd suggest 4 mates and 3 relations.
One revolute for each shaft and a slider for the ball followed by:-
(1) Rack and Pinion from Shaft 1 to Ball, exactly like above.
(2) Gear Mate between Shaft 1 and Shaft 2
(3) Gear Mate between Shaft 1 and Shaft 3
Cheers,
Owen S.

John_P_Desilets

@omri_r I would avoid using any tangent mates for this example. @owen_sparks and I are on the same page for using a combination of gear, rack and pinion, and slider mates.   I made another example for you to take a look at. In order to properly position the screws at the right timing, you will need to edit the individual mate that was used to create the relationship. 



Offsetting the ball to the centerline of the screw. 



Adjusting the timing for the screw. Rotate around the Z axis. 



This workflow should give you the proper result you are looking for. 

https://cad.onshape.com/documents/4bfd3fda008625fceced4150/w/752f205a6eba08f9e1d5fd88/e/320f6ce5bc5588cd5af81110

John_P_Desilets

@omri_r I would recommend sketching it all out first. Properly align the helix to the correct starting point for each screw. Take some measurements and use 2D sketch entities for reference.  A layout sketch will help your features to regenerate when small changes need to be made. 



Starting point for each helix is timed correctly.  



Proper timing of the screws at the assembly level. 

John_P_Desilets

@omri_r It might be easier to try and use a rack and pinion relation. Below is a quick gif of what I am referring to. 

https://cad.onshape.com/documents/cefa2aff693213e49c73600e/w/c23e3a714b33eceace9f7ead/e/1a26b46dc5d55658f8df5884


I created a revolute mate for the screw and mated it to the origin. 

Next, I created a slider mate from the center of the ball to run parallel to the screw. The ball needed to be offset to the thread depth. 

After I created a rack and pinion relation between the revolute mate of the screw and the slider mate of the ball. 

Hope this helps!

omri_r

Thank you John.

I'm newbie and tried to repeat what you did with minor tweaks to the depth of the groove and the pitch of the helix, and I don't succeed to achieve the same thing.

See here...

https://cad.onshape.com/documents/c1fb23babb4668e97ce5a361/w/8cd120f13393056585a21bf4/e/74d56c1158535498da0cb145

The above is the first step of what I want to achieve in the end: This is three threads that revolve in a synchronous way and hold a ball between them like in the image attached below.

Do you think the slider + rack and pinion mates done on all three threads would assist me achieve that?

Thank you!
Omri



https://cad.onshape.com/documents/c1fb23babb4668e97ce5a361/v/345c1518ef86fd9edbcfbf07/e/74d56c1158535498da0cb145

(the above link is done with the tangent mate but it does not work all the time and not accurate since there is minor overlap between the ball and the groove)

owen_sparks

*Edit for rubbish terminology used. 

I'd suggest 4 mates and 3 relations.
One revolute for each shaft and a slider for the ball followed by:-
(1) Rack and Pinion from Shaft 1 to Ball, exactly like above.
(2) Gear Mate between Shaft 1 and Shaft 2
(3) Gear Mate between Shaft 1 and Shaft 3
Cheers,
Owen S.

John_P_Desilets

@omri_r I would avoid using any tangent mates for this example. @owen_sparks and I are on the same page for using a combination of gear, rack and pinion, and slider mates.   I made another example for you to take a look at. In order to properly position the screws at the right timing, you will need to edit the individual mate that was used to create the relationship. 



Offsetting the ball to the centerline of the screw. 



Adjusting the timing for the screw. Rotate around the Z axis. 



This workflow should give you the proper result you are looking for. 

https://cad.onshape.com/documents/4bfd3fda008625fceced4150/w/752f205a6eba08f9e1d5fd88/e/320f6ce5bc5588cd5af81110

owen_sparks

Nice ^^^

omri_r

Thank you @owen_sparks and @John_P_Desilets!

I really appreciate your response and time you put to answer my question with much details!

The timing is a big issue.

I can "guess" what should be the timing for each screw. But it's a guess and it would never be accurate.

Initially, when I tried the tangent mate, it (almost) solved for the right timing. And as you can see in the image below, the solution for the timing is some kind irrational phase between the screws.

I want to be accurate since the next step would be fit a cogwheels on the shafts that would create this synchronized movement. 

Do you have an idea how the timing or phase can be calculated from the assembly w/o guessing?

Omri

owen_sparks

There might be easier ways to calculate how to click the mates to bring the assembly into alignment but instead of that could to use the same ball profile  in the partstudio to sweep the profile of the shafts and build them with the correct initial orientation? Or at least build some sort of helper part that the shafts initialy mate to, to set the orientation, and then suppress that temporary mate?

John_P_Desilets

@omri_r I would recommend sketching it all out first. Properly align the helix to the correct starting point for each screw. Take some measurements and use 2D sketch entities for reference.  A layout sketch will help your features to regenerate when small changes need to be made. 



Starting point for each helix is timed correctly.  



Proper timing of the screws at the assembly level. 

omri_r

@John_P_Desilets, This is really amazing what you did here!

Thank you very much! I really appreciate that non-trivial help.

Can you share a link of the above so it would be easier to me to understand what you did? 

John_P_Desilets

@omri_r  Here is the link to the document 
 https://cad.onshape.com/documents/a6e7be729c745ccfdc726535/w/640755938ea1d07b729e7d25/e/1b66f8404dc6f8d7b70bb968

This is a rough mockup of what you are looking to do. Please let us know how you made out!

omri_r

This is really great!

I followed it step by step. Currently just trying to understand what you did.

Learning tons of new techniques and ideas how to accomplish things   

How did you calculate an offset value of 46.5mm?