PDA

View Full Version : Small low tooth count gear question.



Ken_Shea
06-23-2010, 10:14 PM
Brians "first gear" has got me to try making a gear for my first lathe, an Atlas 6", never use it any more but have had it for like 40 years, and would like to have it operational again.

I read in a gear book I have where low tooth count on small gears requires additional consideration, nothing more just that.

What additional consideration would that be referring to?

This gear is an 8 tooth with about a .550 OD, it drives the carriage on the rack.

IdahoJim
06-23-2010, 10:20 PM
I think the consideration with those small tooth-count gears is you need quite a bit of undercutting at the base of the teeth....that wasn't a problem with those Craftsman lathes as the gears were cast. I seem to remember that those Craftsman lathes used 14.5*PA gears. As somebody mentioned on the other thread, anything under about 30 teeth at the 14.5 PA needs some undercutting.
Jim

Ken_Shea
06-23-2010, 10:27 PM
Jim,
You may have that right, there appears to be what i would call additional undercut on these teeth, these are not cast.

Ken

Evan
06-23-2010, 10:37 PM
We need a picture Ken. 8 teeth is way below the practical limit for 14.5 pa gears.

Ken_Shea
06-23-2010, 10:39 PM
be back in a few, of what's left of them.

Ken

Ken_Shea
06-23-2010, 10:45 PM
Here it is Evan,

http://i187.photobucket.com/albums/x175/Ken_Shea/ATLAS.jpg

J Tiers
06-23-2010, 10:48 PM
THAT surely has the "undercut" showing in a lively manner...... the teeth look like spoons.

THAT isn't going to be done with a regular circular gear cutter, it needs to be "generated".

Ken_Shea
06-23-2010, 10:48 PM
Pretty sad huh :D

Ken_Shea
06-23-2010, 10:53 PM
THAT surely has the "undercut" showing in a lively manner...... the teeth look like spoons.

THAT isn't going to be done with a regular circular gear cutter, it needs to be "generated".


Not sure what generated means, I am thinking that it can be CNC'd on the mill, drill for the under cut and then use a 32nd end mill for the profile, if..... a 32nd end mill can be found with a 1/4" flute length.

gary hart
06-23-2010, 10:59 PM
This might not help for that gear but John Stevenson helped me solve a low count gear problem.

go down to post # 23 in this thread.
http://bbs.homeshopmachinist.net/showthread.php?t=33136

darryl
06-23-2010, 11:02 PM
Not that I know much about gears, but the first thing that came to mind was to drill a ring of holes first to define the root, then cut the teeth. For only 8 teeth and very slow speed operation, you could file off any edges left after cutting the teeth to leave them all smooth. Should be good enough.

IdahoJim
06-23-2010, 11:09 PM
Not that I know much about gears, but the first thing that came to mind was to drill a ring of holes first to define the root, then cut the teeth. For only 8 teeth and very slow speed operation, you could file off any edges left after cutting the teeth to leave them all smooth. Should be good enough.

Yup...that occurred to me too...should work well enough
Jim

Ken_Shea
06-23-2010, 11:12 PM
Occurred to me too, see post #9 :D

IdahoJim
06-23-2010, 11:18 PM
Occurred to me too, see post #9 :D

LOL...sorry, Ken, I missed that:D
Jim

Ken_Shea
06-23-2010, 11:24 PM
This might not help for that gear but John Stevenson helped me solve a low count gear problem.

go down to post # 23 in this thread.
http://bbs.homeshopmachinist.net/showthread.php?t=33136

Thanks Gary,
Johns a pretty sharp cookie, man that was hard to get out :D

leesr
06-24-2010, 12:25 AM
Hey Guys for low # of teeth it's bad to have undercuts in the teeth.
the adjustment would be to enlarge the addendum (major dia.) of the gear
thus eliminating or minimizing the undercut.

this is also known as profile shift.

or to shorten the addendum in the gear can also be done.
this is also know as recess gears.
this prevents the teeth wearing like it did or interfering & jamming.

I am not in the shop so I will post addendum tomorrow
how ever it would be OK to drill the root except leave stock for finishing.

Quote:
Originally Posted by gary hart
This might not help for that gear but John Stevenson helped me solve a low count gear problem.

go down to post # 23 in this thread.
http://bbs.homeshopmachinist.net/showthread.php?t=33136


Thanks Gary,
Johns a pretty sharp cookie, man that was hard to get out

sorry missed the post the first time.
yes sir Sir John explained it very well as matter of fact best I have seen from reading tons of books & article's
I would suggest for some one to draw the gear out so it can be transfered to the blank, bluing then scribe the profile for a guide.

Cheers
Leesr

Evan
06-24-2010, 01:17 AM
There aren't many programs that will generate such a low tooth count for a 14.5 pa gear but AlleyCad will.

This is what it looks like

http://ixian.ca/pics7/8tooth.jpg

And this is the DXF:

http://ixian.ca/pics7/8tooth.DXF

John Stevenson
06-24-2010, 05:09 AM
Nice flower Evan.

http://www.stevenson-engineers.co.uk/files/8TEETH.BMP

Thats an 8 tooth 14.5 PA gear drawn correctly.

BTW the gear you are looking for is an 18 DP gear.

.

Weston Bye
06-24-2010, 05:41 AM
http://i187.photobucket.com/albums/x175/Ken_Shea/ATLAS.jpg

I'm in the same situation. Followed the advice of another machinist and attempted a "shaper" operation with the Atlas lathe. Good judgement comes from experience. Experience comes bad judgement. The particular gear under discussion here was not man enough for the job. I've made gears from brass and delrin. This will be my first steel gear. When I get around to the new experience, I will post the results of my efforts.

Evan
06-24-2010, 05:48 AM
Yours looks better than the Alley Cad gear but I wouldn't quite say it is correct. I just remembered that I have another program that does draw them correctly at any tooth count down to 2.

This is correct.

http://ixian.ca/pics7/8tooth2.gif

Weston Bye
06-24-2010, 05:56 AM
Being intimately familiar with the application, I suspect that any close approximation will work. The gear engages a rack and is driven by a handwheel. As long as it isn't "notchy" or to sloppy, it will do the job.

John Stevenson
06-24-2010, 07:13 AM
Yours looks better than the Alley Cad gear but I wouldn't quite say it is correct. I just remembered that I have another program that does draw them correctly at any tooth count down to 2.

This is correct.

http://ixian.ca/pics7/8tooth2.gif
BOLLOX.

There is no way that a low count gear in 14.5 PA will have no serious undercutting.
Paint shop pro is not a gear program.

You need Microsoft Paint for that :rolleyes:

.

John Stevenson
06-24-2010, 07:31 AM
Being intimately familiar with the application, I suspect that any close approximation will work. The gear engages a rack and is driven by a handwheel. As long as it isn't "notchy" or to sloppy, it will do the job.

Bang on Weston, so here's an alternative that requires the simplest of tooling.

Please peruse the follow scratching from my CAD program.

http://www.stevenson-engineers.co.uk/files/8TEETH%20both.BMP



Geometrically correct gear with undercutting and if we look we can see that the undercutting is virtually a slot.

So if we cut 8 slots on a dividing head with a 3/32" ball nosed cutter at 0.120" deep we get a very close approximation to the slot shape.

Also not on the drawing that a line A - B has been drawn from where the slot touches the involute to the OD.

A second line has been drawn parallel to that touching on the involute as in C - D

Now those lines A - B and C - D are at 45 degrees, so if we rotate the work in the dividing head 45 degrees we get this.

http://www.stevenson-engineers.co.uk/files/8TEETH%20setover.BMP

The line X to C - D is from the top of the slot to the involute and is 0.034"
So using the side of the cutter remove this 34 thou, index round 8 teeth and repeat.

Set over to the other side of a tooth, remove 34 thou from that side and you have a very very close approximation of the required gear that will probably just need lightly dressing with a fine file around points D - B as it's de-burred.

No gear cutters or microns harmed.

.

Evan
06-24-2010, 07:31 AM
It isn't from Paint Shop Pro.

It was generated by an involute gear plugin for Sketch Up.

The plugin was written by an engineer that knows what he is doing.



Application of Multiparameter Optimization for Robust Product Design

Douglas K. Herrmann
J. Mech. Des. 131, 024501 (2009) (6 pages)
Abstract Full Text: [ HTML PDF (770 kB) ]


http://scitation.aip.org/journals/doc/ASMEDL-home/most_downloaded.jsp?KEY=JMDEDB&Year=2009&Month=2&agg=md

DFMiller
06-24-2010, 07:48 AM
Ken,
What material are you going to use?
looks like a nice job for your shaper and that electronic indexer that I am going to help you with. I think with John's approximation technique it would work. Does Our favorite CAM took not do gear shapes ?
Another approach is wire EDM. I will have to chat up the guy at the workshop with his nicely made one.
Dave

John Stevenson
06-24-2010, 07:52 AM
It isn't from Paint Shop Pro.

It was generated by an involute gear plugin for Sketch Up.

The plugin was written by an engineer that knows what he is doing.



http://scitation.aip.org/journals/doc/ASMEDL-home/most_downloaded.jsp?KEY=JMDEDB&Year=2009&Month=2&agg=md

Ask him why no undercut ?

The truth is most CAD programs approximate the shape, some make a good job of showing what's above the pitch line but the dedendum is a rats next of calculations so they don't bother and fudge it.

It's only pretty pictures after all.

John Stevenson
06-24-2010, 07:53 AM
Just drew it up.

http://www.stevenson-engineers.co.uk/files/kludge.BMP

White is correct.
Green is the kludge.

Could get it better with a 0.188 cutter as the drawing instead of the 0.193" 3/32" cutter

.

Tony Ennis
06-24-2010, 08:13 AM
Is there enough metal to mill the slots a little deeper?

J Tiers
06-24-2010, 08:30 AM
Just drew it up.

White is correct.
Green is the kludge.

Could get it better with a 0.188 cutter as the drawing instead of the 0.193" 3/32" cutter

.

Depending on the amount of clearance in the "correct" one vs the "kludge", drilling out might work fine.

All you need is to "not" have material where it interferes. There is no requirement for the tooth to be attached to the hub, or for there to BE a hub there.

A "lantern" pinion in a clock is made up of rods where the teeth would be, parallel to the tooth face. The hubs are off to the side, holding the rod ends, with "nothing" where the undercut is. it looks more like a cage than a gear, but they work every day by the millions.

OK you don't "have" to "generate" the form (as a hob would) but you have to account somehow for the ends of the mating gear teeth, which will be interfering with teeth cut with an ordinary form cutter.

if you cut a wide enough "slot" with a form cutter, it looks like you would actually be in danger of cutting away the form at the pitch line.

Someone mentioned that it engages a rack...... That would seem to be worst case, as the rack tooth would follow the relative path of a hob or other "generating" method...... It seems that the only way an "incorrect" no-undercut form would work well is if it was widely slotted, OR the "depthing" was way off.

Ken_Shea
06-24-2010, 10:10 AM
Ken,
What material are you going to use?
looks like a nice job for your shaper and that electronic indexer that I am going to help you with. I think with John's approximation technique it would work. Does Our favorite CAM took not do gear shapes ?
Another approach is wire EDM. I will have to chat up the guy at the workshop with his nicely made one.
Dave

Dave,
Our favorite CAD :) does do gear shapes, emphasis on shapes, have heard it is like most, just an approximation, for this application, I believe plenty good as Wes points out. Material will be drill rod.
Johns drawing looks to be very close to what needs to be if that undercut is required.

Wish the actual engagement could be seen but that's all hid once assembled.

Ken_Shea
06-24-2010, 10:15 AM
Is there enough metal to mill the slots a little deeper?
Tony,
Could go some probably, the original gear shows cuts into the 3/8 shaft as it is.

Evan
06-24-2010, 10:15 AM
Someone mentioned that it engages a rack...... That would seem to be worst case, as the rack tooth would follow the relative path of a hob or other "generating" method...... It seems that the only way an "incorrect" no-undercut form would work well is if it was widely slotted, OR the "depthing" was way off.

Undercut or lack of same in not the issue. Undercut is an incorrect shape produced by the involute form calculation for small tooth counts. It can be compensated by modifying the tooth form by replacing the calculated form with a straight line to the centre of the gear. This angle still produces a slight amount of undercut but will never be less than the angle of the teeth in a rack for the particular pressure angle. The issue is the crest of the teeth, not the dedendum. That is why there is a standard modified form for teeth that is a stub profile with rounded corners.

In the calculated profile I provided it will interfere with a rack unless modified, which is exactly what John is acomplishing by trimming the sides from the tooth profile. The easiest modification is to simply stub the teeth as shown in this image. That still leaves the remainder of the tooth with the proper involute shape.


http://ixian.ca/pics7/gears8.gif

precisionmetal
06-24-2010, 11:45 AM
Yep -- a radial line from the point where the involute touches the base circle to the center of the gear is a correct way to handle very low tooth count gears.

From that point, a check of the mating rack or gear to verify that there is no interference and you're done.

Doesn't need to be any more complicated than that. :)

leesr
06-24-2010, 12:54 PM
[QUOTE=Evan]Undercut or lack of same in not the issue. Undercut is an incorrect shape produced by the involute form calculation for small tooth counts. It can be compensated by modifying the tooth form by replacing the calculated form with a straight line to the centre of the gear. This angle still produces a slight amount of undercut but will never be less than the angle of the teeth in a rack for the particular pressure angle. The issue is the crest of the teeth, not the dedendum. That is why there is a standard modified form for teeth that is a stub profile with rounded corners.

In the calculated profile I provided it will interfere with a rack unless modified, which is exactly what John is accomplishing by trimming the sides from the tooth profile. The easiest modification is to simply stub the teeth as shown in this image. That still leaves the remainder of the tooth with the proper involute shape.

No thats not correct, because if the mating part is mating below the base diameter there will be interference, which will not have conjugate action.
it will go clunk as it tries to turn. either the mating part has to be recessed
or the pinion has to be enlarged.

It is true that any thing below the base diameter is non involute there fore can be straight.

Cheers
Leesr

Evan
06-24-2010, 02:13 PM
Formulae for stub tooth spur gears: Note that it is the addendum that is reduced from 1/DP to .8/DP and the clearance increases.

Addendum = 0.8 Diametral Pitch
Addendum = 0.2546 Circular Pitch

Dedendum = 1 Diametral Pitch
Dedendum = 0.3183 Circular Pitch

Working Depth = 1.6 Diametral Pitch
Working Depth = 0.5092 Circular Pitch

Whole Depth = 1.8 Diametral Pitch
Whole Depth = 0.5729 Circular Pitch

Clearance = 0.2 Diametral Pitch
Clearance = 0.0637 Circular Pitch

Outside Diameter = (Teeth + 1.6) Diametral Pitch
Outside Diameter = (Teeth + 1.6) Circular Pitch π

Diametral Pitch = (Teeth + 1.6) Outside Diameter

leesr
06-24-2010, 02:14 PM
Hey Guys for low # of teeth it's bad to have undercuts in the teeth.
the adjustment would be to enlarge the addendum (major dia.) of the gear
thus eliminating or minimizing the undercut.

this is also known as profile shift.

or to shorten the addendum of the mating gear can also be done.
this is also know as recess gears.
this prevents the teeth wearing like it did or interfering & jamming.

I am not in the shop so I will post addendum tomorrow
how ever it would be OK to drill the root except leave stock for finishing.

Quote:
Originally Posted by gary hart
This might not help for that gear but John Stevenson helped me solve a low count gear problem.

go down to post # 23 in this thread.
http://bbs.homeshopmachinist.net/showthread.php?t=33136


Thanks Gary,
Johns a pretty sharp cookie, man that was hard to get out

sorry missed the post the first time.
yes sir Sir John explained it very well as matter of fact best I have seen from reading tons of books & article's
I would suggest for some one to draw the gear out so it can be transfered to the blank, bluing then scribe the profile for a guide.

Cheers
Leesr

corrected my mistake added mating gear

cheers
Leesr

J Tiers
06-24-2010, 10:00 PM
I'd have to check, but the undercut seems to be there to clear the end of the rack tooth as the pinion turns against it.....

Unless you use a "modified rack", with the corners "adjusted", it was my impression that a standard rack and low count pinion had to have undercut past a radial line...... and ends up with the odd-looking shape with a "hump" between the teeth just because of the "path" of the rack corners relative to the pinion..

if you change the shape of all the teeth, you can fix that, but here the poster wanted to match an existing rack, which probably has straight-side teeth..... I doubt the original was cut to that "spoon shape" just for artistic reasons. It appears to go past a regular radial line...... might be an optical illusion.

precisionmetal
06-24-2010, 10:34 PM
Absolutely correct -- if the mating gear (in this case a rack) is fixed/defined, and the center distance is defined, then the design (albeit a poor one) is fixed.

If there was a way to machine off the back side of the rack and get it a bit further away (essentially increasing the center distance to the "infinite" size gear), then 8 teeth could be cut on a larger blank, and the CTT could be fattened up -- both of which would make a considerably stronger pinion.

PM

Ken_Shea
06-24-2010, 11:17 PM
Unfortunately, not much can be modified easily with regard to using a larger gear.
This is the gear form that I am going to try tomorrow as it seems to closely match the original, for what ever that's worth.

Also have to make a new gear carrier as the original is just to sloppy.

http://i187.photobucket.com/albums/x175/Ken_Shea/8-tooth.jpg

Will be drilling the root relief using a #51 (.067), then profiling with a 1/16 end mill.

DFMiller
06-25-2010, 06:43 AM
Why not drill the root relief and profile with a 1/16 end mill then you would not have to find a #51 drill bit. ;-)
Dave

Ken_Shea
06-25-2010, 06:52 AM
Why not drill the root relief and profile with a 1/16 end mill then you would not have to find a #51 drill bit. ;-)
Dave

Ha-Ha, "find a #51 drill bit", inside joke, very funny.

Drilling is much faster.

DFMiller
06-25-2010, 07:06 AM
But Ken,
It depends on what your perspective is. Total time includes finding drill loading it into tool holder, setting TLO, drilling.
:-)
:-)
Dave

Ken_Shea
06-25-2010, 07:13 AM
Well, may have to do that, still have not found either set of drills, I try and avoid plunging, with larger endmills it just does not sound natural, small end mills, too easy to break.
Besides I like watching the ATC change tools :D
It only takes a couple minutes at most to set up a tool in the control.

DFMiller
06-25-2010, 07:24 AM
Ken,
What are your operations planned. Being a noob I want to learn.
Will you rough it out with a bigger mill?
Will you do a rough pass with the 1/16 then how much will you leave for finishing?
What will you use for doc and feeds for both rough and finish with small mill.
I see there is much to learn from this what appears to be a simple profile job.
How will you work hold it. I assume you will bolt it to a table or will you chuck some stock in a chuck mounted to table?
Dave

Ken_Shea
06-25-2010, 07:44 AM
Being such a small area no room for or need to rough it out as a separate operation, but will leave .002 for a final finish profile pass at full depth. Going to try .015 as the DOC at a couple IPM, RPM at the max 6000, and coolant.
I have never cut steel with a 1/16 end mill so that may need to be adjusted.

I could use some advice on the cutting parameters as well.

Haven't decide on the method of fixturing it, likely just use a block reamed to 3/8, (the gears shaft size), and a set screw to hold it fast, clamp that in the vise and use a Blake coaxial indicator to locate the center.

BobWarfield
06-25-2010, 11:17 AM
3-7 IPM for your paramaters on mild steel says G-Wizard.

Beware of runout. Breaks a lot of small endmills. Use your best holder!

Cheers,

BW

Ken_Shea
06-25-2010, 11:24 AM
Bob, if you get a chance, see what G-Wizard says on medium Carbon steel as it will be drill rod.

ME-Consultant Pro indicates 2.8 IPM so I backed off from that.
2 flute Carbide x 1/16

Thanks

brian Rupnow
06-25-2010, 12:50 PM
Having been thoroughly spanked, on the issue of gears--I'm going to stand in the corner with my mouth shut, and watch other folks answers!!!

BobWarfield
06-25-2010, 01:40 PM
Bob, if you get a chance, see what G-Wizard says on medium Carbon steel as it will be drill rod.

ME-Consultant Pro indicates 2.8 IPM so I backed off from that.
2 flute Carbide x 1/16

Thanks

About 2.1 IPM. I had assumed 4 flute in the other as well, so half the feedrate.

BTW, the Beta Test is free if you want to play with it yourself.

Cheers,

BW

leesr
06-25-2010, 03:00 PM
Ken

sorry i dropped out, but been smacked with work.

the Information I have is for 20 deg PA & not 14.5 Deg PA, however
that said I normally don't design gears I just make them.

If you have time, It would be nice if you could post the rack dimensions,
Take measurements from the top the Rack to the bottom
Then from top of the rack to the root diameter, then using a wire as close as you have to .1067 wire measure the wire to the top of the rack
then measure over two wires on the 8 tooth pinion if you can.

Otherwise keep proceeding as you are. all is well.
just wanted to run some numbers.

Cheers
Leesr

Ken_Shea
06-25-2010, 03:58 PM
Having been thoroughly spanked, on the issue of gears--I'm going to stand in the corner with my mouth shut, and watch other folks answers!!!

Ha-Ha,
I know what you mean, stand by :)

This gear isn't going to be made with a form cutter rather milled, so I believe I'm safe, can't do much wrong but break a few endmills, can only find one so I hope that does not happen else it will be on hold for a few day to get more ordered.

DFMiller
06-25-2010, 07:52 PM
Ken,
So what is Z max?
I am interested in your finishing pass and that you are doing it full depth.
That's one of my learning questions and now I have an answer.
I look forward to seeing the item in question in person.
Thanks,
Dave

Ken_Shea
06-25-2010, 09:13 PM
Dave, not sure where I mentioned Z max, but that term could be used to simply mean a finish profile cut at full depth (I.E. Z-Max) from a roughing operation where .003 or a bit more is deliberately left on the walls so the final pass cleans up all around.
Often used also to creep up on a given dimension.


Was there another final workshop today?

Thanks to you, spent quite a few hours cleaning, made a small dent!
It was a dirty job but someone has to do it, no really, I mean it was a dirty job :D

DFMiller
06-25-2010, 09:37 PM
Ken,
Poorly worded question on my part. What is the thickness of the part? I have never intentionally done a full depth finishing pass that exceeded 1 cutter diameter. The question has always been a question as doing finishing passes with less than full depth leaves a crappy finish on most of my projects. It comes down to machining strategies.

Today was another great day at the CNC workshop. The people at the workshop were fantastic and freely shared so much information. It was a reflection of the great people here but with a CNC focus. George and VP did a greet job and I hope they do it again next year. My kid wants to join me next year again but be have sort of agreed we will fly in next year not drive from Surrey BC.

I hope some of the friendships made will continue.Dave

Ken_Shea
06-25-2010, 10:00 PM
You can make a full dept finish pass at virtually any cutter length, I've done many 2" finish passes with a 3/8 carbide.
Almost always do them climb cutting as that gives a better finish, your not re-cutting the chips.

I think that is really cool that your Daughter has such an interest in machining.
Truth is, not really many are interested in it, none of my so called friends or any family members are, they look, ask a few questions and that is the extent of their interest. It will be nice to actually have some one visit that is genuinely interested in machining.

I have more interest then I can possibly find time for, that does not seem to be that common any more.

Might warn you, the place may be so clean that I may have to ask you to take your shoes off, or possibly maybe not :D

Evan
06-25-2010, 10:53 PM
ME-Consultant Pro indicates 2.8 IPM so I backed off from that.
2 flute Carbide x 1/16


Start at 1 ipm and work it up if you think it will take it. At only 6000 rpm it won't be cutting anywhere near the happy zone. Your first clue that it isn't happy will be that the end mill business end just became invisible. At 6000 rpm the sfm is only 100. It would be much better at several hundred at least. I use exclusively carbide cutters for the small stuff because HSS isn't stiff enough. I have lots of broken ones in the drawer that I grind into engraving cutters.

Ken_Shea
06-25-2010, 11:08 PM
1 IPM was my plan to start, I have zero experience cutting any steel with that size cutter and only have one cutter, so I was going to be very cautious.