# Any math (gear ratio) experts out there?



## jhinze1970 (Mar 30, 2020)

I'd have a few atlas lathes, all with QCGB. I'd like to be able to cut a 2.4 pitch metric thread..

Anyone know of any formula's that I could use or extrapolate to figure what gear's I could replace the 40t and 48t with and then determine which lever positions to choose to come close? I'm not a math wiz... in fact I'm mathematically challenged.. but would like to learn.

Any help or pointing toward resources would be appreciated


----------



## Alexander McGilton (Mar 30, 2020)

2.4 mm pitch is very odd. what do you need it for? 2.5mm is very common for a thread pitch, few if any lathe will have a gear combo to make such a thread at the ready. May need to be made on a cnc.
This is from the new southbend tool room lathe.


----------



## jhinze1970 (Mar 30, 2020)

I need it to cut a triple lead .8 pitch thread thread ...


----------



## Alexander McGilton (Mar 30, 2020)

What is the selection of leads of your lead screws of your lathes? Do you have the 120and 127 tooth gear combo? How close must the threads match? can you make do with 10.5 tpi ?


----------



## mickri (Mar 30, 2020)

1/(2.4*0.03937) = 10.5834 tpi  Here is a link for you.  https://www.fastenermart.com/understanding-metric-fasteners.html

The manual for the qcgb on my craftsman 12x36 has a list of every thread that can be cut through the gear box.  10.5800 tpi is the closest.  Attached is the manual which shows the gears and their positions on page 21.


----------



## jhinze1970 (Mar 30, 2020)

Thanks Alexander and Mick(?). I think the 10.5834 might just work, it's 5/16" worth of threads, the error should be almost negligible.


----------



## RJSakowski (Mar 30, 2020)

Gear selection will vary from one lathe to another. My Grizzly G0602 can cut a 2.400mm thread exactly using a =  40t, b = 36t, and position IB on the gear box.
edit:  I do by changing the 48t gear on my input shaft for the gear box with a 40 tooth gear.  The input shaft is now rotating 48/40 times as fast so the setup for a 2.0mm thread will now cut 48/48x2.0 = 2.4mm/rev.


----------



## RJSakowski (Mar 30, 2020)

Cutting a multi-lead metric thread on an inch lathe should prove interesting.  Ordinarily, I would use the thread dial to get the proper clocking but that won't be possible cutting metric threads.  

A work around would be to thread a small section at the .8mm pitch and use that section to visually set up the threading tool when cutting the 2.4mm pitch.  The tool would be set to the .8mm thread and one lead would be cut.  Then the tool would be advanced by one thread on the .8mm section and the second lead would be cut.  Then it would be repeated for the third lead.  

Another way would be to use the compound and do the math.  The half nuts would be engaged , the compound and cross feed would be zeroed and the first lead cut.  Then the compound returned to zero and would advanced by .0315"(.8mm) if the compound was set parallel to the spindle axis or .0640" (.0315/sin(29.5º) if the compound is set to 29.5º. The compound dial would be rezeroed and the the cross feed brought to touch the major diameter and rezeroed and the second lead cut.  The procedure would be repeated for the third lead.


----------



## mickri (Mar 30, 2020)

If you need a refresher on cutting a multiple thread Mr Pete has an excellent set of videos on how to do it.  I just watched them.  Here is the first video of the series.


----------



## Tolerent (Mar 30, 2020)

Just curious what the perspective on making a custom 3 point HSS cutter head and running it at .8 mm? Sorry if this falls in the stupid questions category. I will forgive anyone that mocks this inquiry.


----------



## Alexander McGilton (Mar 30, 2020)

It would work, though you may put more effort in to making the tool than threading three times and doing the trig to offset the single point tool.


----------



## RJSakowski (Mar 30, 2020)

Tolerent said:


> Just curious what the perspective on making a custom 3 point HSS cutter head and running it at .8 mm? Sorry if this falls in the stupid questions category. I will forgive anyone that mocks this inquiry.


Welcome to the forum.  

There was a thread about a month ago where a Russian machinist made a multi-point threading tool from a threading die.  The dialog was in Russian but you can see what he was about.  

As to the operation, you would want to run at 2.4mm.


----------



## brino (Mar 31, 2020)

Tolerent said:


> Just curious what the perspective on making a custom 3 point HSS cutter head and running it at .8 mm?



Interesting idea.......
I first pictured in my mind using a 3-fingered fixed steady, but as a traveling stead (attached to the cross slide) with the work supports replaced by three separate thread cutting tools. 

I also have to wonder if you can't buy a short piece of shaft already made with that special 3-start thread and attach it to the other part (press-fit, loc-tite, etc.)

Not that I'd ever discourage someone from doing something just to prove they can.
But you have to accept that it may not be economical (in time or money).

-brino


----------



## jhinze1970 (Mar 31, 2020)

RJSakowski said:


> Another way would be to use the compound and do the math.  The half nuts would be engaged , the compound and cross feed would be zeroed and the first lead cut.  Then the compound returned to zero and would advanced by .0315"(.8mm) if the compound was set parallel to the spindle axis or .0640" (.0315/sin(29.5º) if the compound is set to 29.5º. The compound dial would be rezeroed and the the cross feed brought to touch the major diameter and rezeroed and the second lead cut.  The procedure would be repeated for the third lead.



Thanks for the info. I have cut multi-lead threads before, but all english. For example, one I routinely cut is a quad 7tpi, finished thread is 28tpi... so thread offset and depth is based off the pitch of a 28tpi thread (.0357 which I round up to .036). 

When it comes to metric, maybe I am confused... but I was approaching it as finished thread pitch of .8 would require three leads cut at 2.4, which would provide the space between leads to stack the threads..


----------



## RJSakowski (Mar 31, 2020)

jhinze1970 said:


> Thanks for the info. I have cut multi-lead threads before, but all english. For example, one I routinely cut is a quad 7tpi, finished thread is 28tpi... so thread offset and depth is based off the pitch of a 28tpi thread (.0357 which I round up to .036).
> 
> When it comes to metric, maybe I am confused... but I was approaching it as finished thread pitch of .8 would require three leads cut at 2.4, which would provide the space between leads to stack the threads..


You are correct.  The gearing should be set up to advance the carriage 2.4mm/rev.  To cut the second pass, you have to either turn the work 120º, leaving everything else as is, or move the threading tool .8mm toward or away from the headstock while leaving everything else as is.  The third pass would be set up by moving another .8mm.

Mr. Pete does a good job of explaining this in his video linked above (there is a small error about 16:30 in the second part where he is explaining why the 29.5º compound angle is used; the tool cuts the mostly on the right flank of the thread but it also shaves the left flank due to the .5º offset from 30º).


----------



## jhinze1970 (Mar 31, 2020)

RJSakowski said:


> You are correct. The gearing should be set up to advance the carriage 2.4mm/rev. To cut the second pass, you have to either turn the work 120º, leaving everything else as is, or move the threading tool .8mm toward or away from the headstock while leaving everything else as is. The third pass would be set up by moving another .8mm.
> 
> Mr. Pete does a good job of explaining this in his video linked above (there is a small error about 16:30 in the second part where he is explaining why the 29.5º compound angle is used; the tool cuts the mostly on the right flank of the thread but it also shaves the left flank due to the .5º offset from 30º).



I gotcha.. like I said, I do it on a regular basis, just with imperial... the root of the question was the 2.4mm pitch on the atlas, which, I think we got a configuration close enough above, just gotta give it a try.

Want to say thanks to all who contributed on this note.. I got a lot of good info in this thread.


----------



## ErichKeane (Mar 31, 2020)

RJSakowski said:


> You are correct.  The gearing should be set up to advance the carriage 2.4mm/rev.  To cut the second pass, you have to either turn the work 120º, leaving everything else as is, or move the threading tool .8mm toward or away from the headstock while leaving everything else as is.  The third pass would be set up by moving another .8mm.
> 
> Mr. Pete does a good job of explaining this in his video linked above (there is a small error about 16:30 in the second part where he is explaining why the 29.5º compound angle is used; the tool cuts the mostly on the right flank of the thread but it also shaves the left flank due to the .5º offset from 30º).



I actually just watched that video independently, and the 1 thing that confused me (until I researched it) is how to figure out cut depth.  He spends about 20 minutes showing off examples, and 30 seconds stating the thread depth   The idea is that the depth is based on PITCH, not LEAD, which makes sense to me. 

A double-start 5/8-12 (PITCH) has the same cut depth as a single-start 5/8-12, except you simply move the carriage toward the headstock at 2x the speed.  So other than the gearbox setting, a double-start thread is the same as cutting a single-start thread in every other dimension.

I DID like the idea of using the compound to advance the cutter.  It is much easier than my original thought (which was backing up/advancing a 29.5 degree compound by a specific amount, then re-touching off with the cross slide).  It seems my way would still let you do the 29.5 degree compound, but the math seems onerous.


----------



## mickri (Mar 31, 2020)

jhinze  One thing that has not been mentioned and you are probably aware of this but when cutting metric or odd threads like 10.58 once you start you have to leave the half nuts engaged or you will lose your sync on the threads.  The manual I posted above discusses this briefly and there are videos on cutting metric threads on an imperial lathe that go over this.  Having said this there is a method that does involve disengaging the half nut.  In my experience it is easier to leave the half nut engaged.


----------



## rjs44032 (Mar 31, 2020)

All depends on your lead-screw pitch. Let us know what the lead-screw pitch is on the lathe you want to use. Also the change gears you have and what you're using for metric transposing gears and I'll tell you how to get there.

Edit: For Example: a 45T and 34T combo will produce nearly perfect 2.4MM thread on an 8TPI leadscrew (less than 2 micron deviation). Need to know your lead-screw pitch and your available gears. 

Best Regards,
Bob


----------



## RJSakowski (Mar 31, 2020)

ErichKeane said:


> I actually just watched that video independently, and the 1 thing that confused me (until I researched it) is how to figure out cut depth.  He spends about 20 minutes showing off examples, and 30 seconds stating the thread depth   The idea is that the depth is based on PITCH, not LEAD, which makes sense to me.
> 
> A double-start 5/8-12 (PITCH) has the same cut depth as a single-start 5/8-12, except you simply move the carriage toward the headstock at 2x the speed.  So other than the gearbox setting, a double-start thread is the same as cutting a single-start thread in every other dimension.
> 
> I DID like the idea of using the compound to advance the cutter.  It is much easier than my original thought (which was backing up/advancing a 29.5 degree compound by a specific amount, then re-touching off with the cross slide).  It seems my way would still let you do the 29.5 degree compound, but the math seems onerous.


The math isn't really that bad.  You have a right triangle with a 29.5º angle.  The compound advances along the hypotenuse but the adjustment needed is in the z direction of the short side of the triangle (opposite the 29.5º angle).  The z axis travel divided by the compound travel is equal to the sine of 29.5º.  You have to remember to rezero the compound and the cross slide.  You can calculate the cross slide adjustment as well since the cross slide travel divided by the compound travel equals the cosine of 29.5º.  It saves you the bother of touching off the tool again to zero the cross slide.


----------

