Cutting out or creating the shape of a rack through a moving roller pinion

[fusion1BXBB2]

Hello guys,

currently i am working on a project where i want to use the roller pinion and rack system (e.g. Nexen rpg) instead of a standard rack and pinion. Unfortunately, to create the correct rack i would need a script or so to do the math. I am not able to do that by myself. I have found 2-3 people who seem to have created such scripts. One can be found through the thingverse page (https://www.thingiverse.com/thing:1013816), but i get a error message when loading the script.

So, my question is: Is it possible to do something similar in Fusion 360, e.g. to cut out a shape of a body through a moving object? More specific: I want to move the pinion along a path and automatically create the correct shape of the rack.

In case thats not possible, are there any alternatives for someone without any coding knowledge?

Ps: I am in contact with someone from US who can create the shape of the rack for me with his script, but due to the fact that i have to play around with the pinion size, i would need to ask him many times to create the rack for me. He is in US and i am in Europe, so i believe we will exchange a mail once a day, but i am a bit in hurry. (i am still very thankful that in case i will not get it done by myself i still have someone who can help me out, but of course i dont want to use his time)

Thanks in advance!

Best regards,

Denis

[MRWakefield]

After a very quick Googling I found this page where it explains how to draw a cycloid (this is what you need for your roller pinion rack) here.

I replicated this in Fusion to produce this:

I've just entered some arbitrary values in my example and it might break if you enter wildly different values. Anyway, I've attached the file in case as you might be able to use it as a starting point.

Hope this helps.

[CGBenner]

@fusion1BXBB2 

Welcome to the forum!  And thank you @MRWakefield for offering some help on this!

[fusion1BXBB2]

Hello,

thank you very very much for that. It might be exactly what i need. Unfortunately i now need to go to the vet with my Dog, but later on evening i will try it out and hope it will work, but it looks like its exactly what i need.

I just need to figure out the parameter screen that is on the screenshot nr.2

I will post again after i have tried it out.

[MRWakefield]

No problem, I like trying to solve things like this. It might not be perfect and I'm sure someone else could come up with a more elegant or simpler solution but I hope it helps.

[MRWakefield]

Ok, so checking this over I think there might be something wrong with the model I posted (too hasty as usual!!). I've drawn in a circle where the adjacent roller is and I would have expected it to contact the profile of the next tooth flank. However as you can see below it doesn't:

I'll keep looking at it and see if I can find out where it has seemingly gone wrong.

[fusion1BXBB2]

Once again, thank you very much for helping me out with that.

I just wanted to post about a problem i have and now i see that you also have found a problem in your drawing. 

I thought that if i compare your drawing i will find the problem, but i measured and it didnt make sense for me.

I will explain what i dont understand on the tutorial (http://www.practicalstudent.com/subjects/td/basiccycloid.shtml):

There reads: 

"Taking the distance between any two of these points with your compass mark 12 off these distances along the base line along which the circle will rotate. Lable these points 0 to 12 as shown. When taking the distance between any two of the divisions of the circle you should add a little bit to the distance on your compass to account for the curve of the circle."

So, my pinion diameter is 29.50 mm with 14 rollers. The distance between 2 points is 6.564 mm. If i do understand correctly, i should take this distance and mark 14 points along the line on which the pinion travels, BUT what does this mean: "....you should add a little bit to the distance on your compass to account for the curve of the circle."

I am confused, because i cannot just "add a little bit" to the distance :D.

Maybe i do understand something wrong, but i hope you know what i mean. In machining i just cant add a little bit here and there.

I will now just use the distance without "adding a little bit to the distance" and then i check what comes out.

Here a drawing of my pinion.

[MRWakefield]

Ok, so I've redone it from scratch using my own method and it looks better than the first attempt using the earlier instructions I found on the web.

You can see the adjacent roller now sits against the flank of the next tooth. I've attached my new model so you can plug in your own figures. I can't vouch for it being perfect as I haven't done much double-checking but it certainly looks to be much better than the first.

[Warmingup1953]

A triple treat?... The real cleverness of the Nexen RPS/RPG is the elimination of backlash and close-to-lossless transmission. I imagine the geometric solution will involve 3 phases that solve as well as high rigidity (perhaps not?) and high precision. How will you manufacture?

[fusion1BXBB2]

Thank you.
I opened it and i am trying to understand how i can use that for my measurements of the pinion and for now i dont get it, but i will continue to try to understand it :D.

About how i want to machine it: I will use a rotary axis (4th axis) for the pinion with a harmonic drive. First i will machine the pinion "stock" and later mount it on the 4th axis. With a 50:1 ratio i will have a resolution of 0.009° degree, which is about 0.003 mm on a small pinion of about 30mm. I will just rotate the axis and drill the hole for the bearing. (first drill, then use a reamer)

When it comes to the rack then i have a idea, but i am not sure if it will work out: On my CNC Lathe i want to machine a grinding disc in the shape of the cutout for the roller. I will make one cut, and then move the rack by the specific distance and then do the next cut and so on. I believe that is the most accurate way at least in my situation. I have a very precise and rigid diy CNC Lathe, and also a very precise diy 4x8 CNC router, but if i would use CNC for machining the pinion and the rack then i will not achieve the accuracy it needs i believe. 

That are just the ideas i have at this moment, but first i need to know how i create the perfect rack for the specific pinion i draw.

[MRWakefield]

What you need to know is this:

• PCD (Pitch Circle Diameter) of the rollers
• Roller Diameter
• Number of rollers in pinion

Plug these values into the parameters dialogue:

You'll need to size your rack in the second sketch to suit your application and do some tidying up. This is not really an 'end product' but hopefully gets you somewhere close.

[fusion1BXBB2]

Thanks! I have managed to change the parameters accordingly to my pinion.

But, somehow the 2 rollers next to the lowest roller are "inside the body", so something is wrong.

I will continue but please see the picture below:

EDIT: I have reversed the changes of your original file and it seems that yours is correct, but after i changed the parameters the roller touches the rack.

[MRWakefield]

I've used your figures together with a 3mm roller and if I measure the distance between my '2nd' roller and the flank of the rack I get 0mm:

If however I check for interference I get a value of 0.691mm³ which to me is probably insignificant:

I'm not sure why there's disagreement between the two methods but this might be due to approximations in the modelling kernel. The cycloid in the first sketch is an approximation so some deviation from the perfect curve is to be expected. If we need it to be more accurate we'd need to add more points.

If you can attach your model with the pinion I'll take a look.

[fusion1BXBB2]

I attached my pinion and the rack that i created through your file with the correct parameters of my pinion.

The interference on my roller and the rack is a lot higher (0.271 mm^3).

I will continue to play around in about an hour. Need to eat something and go for a walk with my dog.

Thank you for helping me out with that.

[Warmingup1953]

10 or 12 Rollers appear to be the only options.

[MRWakefield]

The PCD of the pinion in your file is 27mm. Change your 29.5mm to 27mm and make sure the roller diameter value in the parameters is set to 2.5mm then see whether it fits better. I can't plug these into your file as it just contains 'dumb' (non-parametric) bodies.

[MRWakefield]

I've plugged in the 27mm PCD, a roller dia of 2.5mm and set the number of rollers to 14. I've also edited my model and increased the number of points that define the curve. It is still an approximation but it's much closer to 'perfect'. Obviously the more points you use the more accurate it becomes.

I'll be busy cooking dinner soon so it might take a bit longer for me to reply.

[fusion1BXBB2]

Bon apetit!

I am now back and i have checked your answers while walking the dog.

So, it looks like its possible to use 14 rollers? Not sure why Nexen has no 14-roller pinions, but 10, 12 and then 16, 20, etc.. Before i went out with the dog i saw your reply with the PDF file, and while walking i was thinking that it doesnt make sense for me. Its a circle and the pitch does not change between the rollers - its always same, but i am not a engineer, just a hobby machinist and also by the way, i am not the most experienced Fusion 360.

Edit: Before i posted my answer the file v3 from you was crossed-out so i couldnt download it. Now it is somehow possible. I will check it now.

Can you tell me how you created more points? Did you use the circular pattern? Right now i dont know how you created the second roller (which is marked as construction), but i will continue to try it out.

[MRWakefield]

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@fusion1BXBB2 wrote:

Bon apetit!

I am now back and i have checked your answers while walking the dog.

So, it looks like its possible to use 14 rollers? Not sure why Nexen has no 14-roller pinions, but 10, 12 and then 16, 20, etc.. Before i went out with the dog i saw your reply with the PDF file, and while walking i was thinking that it doesnt make sense for me. Its a circle and the pitch does not change between the rollers - its always same, but i am not a engineer, just a hobby machinist and also by the way, i am not the most experienced Fusion 360.

Edit: Before i posted my answer the file v3 from you was crossed-out so i couldnt download it. Now it is somehow possible. I will check it now.

Can you tell me how you created more points? Did you use the circular pattern? Right now i dont know how you created the second roller (which is marked as construction), but i will continue to try it out.

---

Yes, it is 'possible' to use 14 rollers but they have to rationalise their range so inevitably there will be some 'missing'. I don't remember posting a PDF but we won't worry about that 😉. I'm not surprised that my sketch is difficult to follow, it is a bit busy to say the least! I'll try to explain how it works...

Each of the large circles represent the pitch circle of the rollers at different locations along a 'half-roll' (180°). Initially I positioned the circles at 45° intervals (then later inserted the additional circles to create 22.5° intervals) starting with a roller at the 6 o'clock pos'n. I then drew a line from the centre of each circle out to the PCD circle perimeter coincident with where the centre of the roller would be after rolling this distance. I then drew a fit point spline between all of these points. This curve was then offset by half the roller diameter. This gives the path of the roller surface and therefore represents the face of a tooth. This was then mirrored. I also added a circle that represents the roller at the start pos'n. This together with the offset curve (and a line to enclose the sketch profile) is used to cut the block that represents the rack body. This cut was then 'Rectangular Patterned' an arbitrary number of times with a pitch which is calculated from the pitch circle circumference divided by the number of rollers. I also drew circles representing the next two rollers in the same sketch and used these along with the small 6 o'clock circle to extrude the three rollers.

Hopefully this makes sense and helps you see how it all works.

[fusion1BXBB2]

It took me about 15 minutes, but now i get it. Very good explained. Thank you!

I think its fine if not all rollers are full in contact, as long as the pinion runs perfectly and has no backlash.

About the pdf:  I mean this one: Precision-Motion-control-21282.pdf  , from your message nr. 15 .

You have spent almost the whole day helping me. I would say that my problem is solved. Also i think that i am able to create my own rack for different size pinions (with the help of your drawing and the formulas), but on today i noticed that my Fusion 360 skills are really low. I have to learn to use all the drawing functions, learn to use formulas and so on. Now i need to go to sleep, but i can continue my project.

Thanks!