PDA

View Full Version : Cutting gear rumors



Stepside
12-10-2012, 10:38 AM
I am in the midst of cutting several spur gears. Because of the purpose I need them to be done "by the book". The book being Machinery's Handbook or similiar. In my career there have been many discussions of making spur gears. Some say that you must cut them in a single pass, giving no reason besides "thats how I was taught". Others state that you must cut them by climb milling also giiving the same reason or stating "thats how I always do it".

I would like any thoughts or facts that either substantiate or debunk those ideas. If you have other ideas to share that would be welcome also.

Thanks in advance

Pete

Deja Vu
12-10-2012, 10:41 AM
My thought is to get it done however you can to required specifications without destroying your tools.

Gunsmithing
12-10-2012, 11:25 AM
My self I will do two to three pass. If you are making a lot of gears it is faster to make one pass.
I never climb milling, I just debur the gear. Climb milling is good for only new mills, as the mill gets old the screw wear in the center not end.

Here is list for making 1 to 3 gears the same.
1. do at less three pass note: lass pass cut .005"
2. DO NOT Climb mill

Dave

Mcgyver
12-10-2012, 11:31 AM
I share your frustration.....be wary of people who's main reasons are how long they've been doing something or it was how i was taught. If they can't justify what they're saying or haven't learned the physical why & how, you have to be suspect of the credibility.

Advise like climb milling is usually because its expected to give a better finish but unless the machine was made for it or it is a very light cut, is a dangerous proposition. I would avoid it. So what gives a good finish? sharp cutters, a light finish cut and flood coolant/oil. That and a material that machines well.

Do it one pass has merit from a productivity standpoint, but depending on the setup a finish cut is preferred; ie spring in the system. Other than more time/wear on the cutter, I don't know why a finish cut wouldn't be recommended from a finish/accuracy standpoint.

Bill Pace
12-10-2012, 11:58 AM
First off, let me join the chorus in saying that I cant imagine any circumstances to using climb cutting - it just dont make sense.

Next, are you gonna use a hand ground single point cutter? If so then multiple passes are probably gonna be necessary.

My method has evolved into - yes, its 'just the way I do it' but it works well so here it is.

I have DRO on my mill, I have power feed on the table, and I go ahead and spring for the 50 or so dollars for a dedicated gear cutter. I determine DOC - (depth of cut) and set the blank up to meet the cutter at that depth, I get every thing locked down except the axis Im using to cut (this is critical to maintain the same depth of cut on multiple passes), I set the mill in back gear at about 150-200rpm and the PF at a slow speed, (determined by ear and how large/deep Im cutting) and start the feed. I then make one pass and on the return climb cut I listen for the cutter only making a slight ticking sound indicating Ive made a clean 'to depth' cut.

Jaakko Fagerlund
12-10-2012, 12:42 PM
First off, let me join the chorus in saying that I cant imagine any circumstances to using climb cutting - it just dont make sense.
Rigid machine/setup. Climb milling saves your cutter and thus makes it live longer AND the surface finish is just much more better.

People tend to advice against climb milling just because they always think the maker has only a clapped out crappy mill but don't even bother to ask. Many manual machines have ballscrews and there can always be the unusual CNC user (especially when asking if you can cut something with multiple passes).

Tony Pratt
12-10-2012, 01:03 PM
Without doubt as in all machining you really need to rough and then finish cut to get the best results, obviously a sharp cutter and rigid set up are also necessary. I didn't know many manual mills had ballscrews but I stand to be corrected! Climb milling will give you a superior finish but if your mill has normal Acme screws don't take a full depth climb mill cut.
Tony

Black Forest
12-10-2012, 01:14 PM
My manual universal mill has ball screws on all three axis as well as power feed on all three axis. I try to climb mill every chance I get as it seems to save my carbide tools. I am a novice but it seems to be working for me. I see a noticeable difference in finish when I climb mill.

becksmachine
12-10-2012, 06:06 PM
You don't say what size tooth/gear, what size machine or material.

If they are large tooth sizes, it may speed the overall process considerably if you gash the teeth (gullets) first with a stagger tooth cutter and then come back and finish with the appropriate form cutter.

An involute gear tooth milling cutter has about the worst chip flow characteristics that can be imagined, especially when cutting from solid. This is in contrast to the stagger tooth cutter which can easily operate at depths of cut and feed rates that would quickly destroy an involute cutter. This is accentuated when working in steel, not so much in the short chipping materials.

Dave

lane
12-10-2012, 07:28 PM
Well every one has had their say .So here is mine. If you have a big horizontal mill B&S ,Cincinnati are what ever you can climb mill . If you in a Bridgeport are small mill I would not .As far as depth of cut . I cut 32 pitch gears in one pass they only about .078 deep if I was cutting a 14 DP gear may be 1 pass if soft material something less than 4140 PH. A big gear 6 DP are larger 2-3 passes depending on what Dp. so go from their. Listen to the machine and just watch the cut . Don`t push it just pay attention to what the machine and the set up is telling you . If you need ear plugs something is not right.

Arthur.Marks
12-10-2012, 09:56 PM
Always try to cut to the correct depth with one cut; nibbling away with a succession of small cuts is not recommended. Commercial gear cutters are expensive items and naturally the amateur wants them to last as long as possible between re-grinds. It is a fallacy to think that you are being kind to the cutters by making numerous light passes. Set the cutter to the correct depth and regulate the feed to suit the machine, naturally a heavy robust machine will be capable of a faster feed rate than a small lighter one. When cutting large teeth such as those found on traction engine models, the equipment available may not be man enough to produce the tooth at one pass in which case it may be an advantage to 'gash' the teeth first with either a slitting saw or a side-and-face cutter. This will remove the bulk of the material and lighten the load on the machine when the form cutter is used. Gears and Gear Cutting, Ivan Law. pp. 66-67

If the gear teeth are of fairly coarse pitch, it may be desirable to take roughing and finishing cuts. This is often done in cutting gears coarser than 6 or 7 diametral pitch, although a definite dividing line cannot be drawn owing to variations both in regard to the cutting capacity of the machine itself and the cutting qualities of the stock. When roughing cuts are considered desirable, special stocking cutters are often used for the roughing operations, as they are more efficient for removing stock rapidly than the regular formed cutters. When a second cut is taken for finishing, it is important to have the roughed-out tooth spaces central with the cutter to avoid removing unequal amounts of metal on the sides, since this tends to wear the cutting edges unevenly and produce inaccurate teeth. If roughing cuts are taken, the "stocking" cutter should be set to mill the teeth the full depth, the allowance for finishing being on the sides. Machine Shop Training Course Vol. 2, Franklin D. Jones. pp.226-227

Depth of Cut. On most work no more than two cuts are required---a roughing cut and a finishing cut. If it happens that two or more cuts are necessary, the rule is to take, for the roughing cuts, a coarse feed and about all the depth of cut the machine, cutter, and work will stand...
Finishing Cut. Remember that attention to the slogan "keep cutters sharp" is one of the main factors in good milling; bear in mind that a surface that has been milled with a good sharp cutter is as accurate as a filed and polished surface. Also it is easier and quicker, and therefore cheaper, to mill to size than to finish by filing and polishing.
When it is advisable to make two cuts, a roughing cut and a finishing cut, leave at least 1/64 in. for the finishing cut. In any machine a cutting tool will do better work and last longer if the edge has a chance to get under the chip, where it has less tendency to rub.
There is always spring in every milling operation. If the feed is stopped while the cutter revolves on the work, the surface will be defaced by an undercut. Do not throw out the feed on a finishing cut.
For the same reason as above, if a cut just made is run back under a revolving cutter, the work will be marked each revolution of the cutter. Stop the cutter before running back or else lower the work a trifle. Machine Tool Operation Part II, Burghardt and Axelrod. pp.210-211

It is always tempting to reduce the feed rate if the cutter exhibits distress, but though a slight reduction does no harm this is, in general, a mistake. The depth of cut should be reduced and the feed rate maintained... Very slow feed rates cause the tooth to rub at the beginning of the cut, and this causes poor finish... DEPTHS OF CUT. The rule here is simple: the depth of cut should be as large as the available power will permit up to the limit prescribed for the type of cutter... it will be realised that the thickness of the chip is unaffected by the depth "D" -- it depends only on the feed rate. A full depth cut produces a long, but thin, chip.
...To sum up. The cutting speed is the main factor determining tool life. The figures suggested above are not critical, but when in doubt, use a lower speed. Feed rate is goverened by the tooth load. Too high a tooth load will result in poor finish and may cause "interference" on the primary clearance. Too low a feed rate will cause rubbing, especially if the cutter is a bit worn. Again, the rates derived from Fig. 43 are not critical. The depth and width of cut which can be used depends more on the rigidity of the machine and the power available than on anything else, and should be as high as can be managed with comfort. Very light cuts should be avoided, especially if the cutter is not dead sharp. Milling Operations in the Lathe, Tubal Cain. pp.27-28

Remember to bear the above quote in mind when reading the following comment later in the same book---especially his use of the term "moderate cut." It is obviously reflective of a set-up lacking rigidity when cutting gears on a small (3-1/2" English designation) lathe. A compromise between depth of cut and chatter must be realized while maintaining sufficient feed for the best result.

Even small wheels in brass will benefit from a finishing cut, and any wheel of any size should be given a series of moderate successive cuts. The setup is inherently "whippy" and there is always risk of chatter if too much is taken off at one cut. Once chatter develops it may be very difficult to get rid of it. Cain. pg.104

The size of the cut is made up of the feed per revolution (or per tooth on milling work) and the depth of cut... The amount of feed largely determines the point of initial chip contact and the unit pressure against each unit length of cutting edge. The depth of cut does not change the unit edge pressure but only varies the total pressure against the tool which in turn controls the amount of shank deflection. Design and Use of Cutting Tools, Leo St.Clair. pg.249

Analysis of Cutting-feed Conditions. First, it will be understood that in any operation of cutting metal a considerable force is exerted against the piece being cut and equally against the cutter itself; and that the amount of metal removed (feed and depth of cut) is in proportion to this force. Therefore, the proper depth of the cut and the proper amount of feed depend to a certain extent upon each other and, in addition, both depend on the power and rigidity of the machine itself.
Second, the correct depth of cut and feed depend on the strength of the cutter and the rigidity with which it is held, and the strength of the work and the manner in which it is held. For example, a slender end mill or a thin slitting cutter cannot be given heavy duty; neither should a frail piece of work or a piece held in such a manner that it may spring or bend be given a heavy cut or feed.
Third, the teeth of the coarse-tooth cutter are proportionately stronger than the finer teeth, the chips wash out more readily, and the cutting fluid keeps the cutting edge cooler. For these reasons a heavier chip may be taken with a coarse-tooth cutter.
Fourth, while the coarse feed removes metal faster, the appearance and accuracy of the surface are not as good as is desirable for finished work; therefore, a finer feed is used for finishing...
The general tendency is to overspeed and underfeed a milling cutter. The reason for most of the too quickly dulled cutters is too much speed, and rarely if ever too much feed. It will be well for the beginner to go fairly slowly at the start and avoid spoiling the cutter, the work, or possibly both, but to keep right on the job with the idea of advancing the speed or the feed as much as possible with due regard to the time it takes to sharpen the cutter. Machine Tool Operation Part II, Burghardt and Axelrod. pp.209-210

J Tiers
12-10-2012, 11:58 PM
Once you are "in" the cut, milling involves a gradual transition from "zero chip depth" to maximum, so I don't know that feed adjustment is any worse than setting depth of cut..... The less the depth of cut, the longer the shallow portion of the cut as a percentage of the total cutting distance, very much the same effect as for a slower feed.

Since they both have similar effects, I prefer to adjust feed and have a deeper depth of cut. That tends to have more "teeth in the cut" at once, making the load more even.


Rigid machine/setup. Climb milling saves your cutter and thus makes it live longer AND the surface finish is just much more better.

People tend to advice against climb milling just because they always think the maker has only a clapped out crappy mill but don't even bother to ask. Many manual machines have ballscrews and there can always be the unusual CNC user (especially when asking if you can cut something with multiple passes).

Not just about rigidity...... the real reason for NOT climb milling is if the machine has any slop at all in the feed.

Climb milling is "self feeding", in the sense that the cut is taken in the direction to make the cutter "draw the work in", so there must not be any slop in the feed that allows the table to pull towards the cutter. If it CAN, it WILL, and the "draw-in" will cause an uncontrolled increase in the chipload per tooth.

Ballscrews are about the only feed that won't do that, other than an adjustable double nut on the feed which can be tightened so as to have no slop. But wear on the screw can cause the double nut to lock up when the nut reaches a less-worn part. The screw must be 100% in control of the table movement.. ANY slop will result in the work being repeatedly "drawn in" by the amount of the slop.

Chances are that is enough to break something, or cause the cutter to "walk over" the work, maybe bending the arbor. If the machine is not rigid, it may "give" enough not to bend anything.

If the machine is non-rigid enough, I suppose it could have the same effect as slop, but most such machines will probably have a slop problem that is worse than the rigidity problem.

if your machine CAN take it, climb milling gives a very nice finish, though.

Sometimes, if you can set for a light depth of cut, and put drag on the table with the axis lock, you can make the feed friction more than the "pull-in" force, and then you can get away with it. You then have to "push" the table with the feedscrew. I think that is best left for rare instances of real necessity.... it involves a good deal of force on the feedscrew, and extra wear on the machine in general.

oldtiffie
12-11-2012, 01:55 AM
I am in the midst of cutting several spur gears. Because of the purpose I need them to be done "by the book". The book being Machinery's Handbook or similiar. In my career there have been many discussions of making spur gears. Some say that you must cut them in a single pass, giving no reason besides "thats how I was taught". Others state that you must cut them by climb milling also giiving the same reason or stating "thats how I always do it".

I would like any thoughts or facts that either substantiate or debunk those ideas. If you have other ideas to share that would be welcome also.

Thanks in advance

Pete

The gear outside diameter (OD) is not important within reason - most who consider it imporatant only do so to "scratch" (ie "witness") to set depth of cut to zero.

The Pitch Diameter is not too important either as it can be varied to suit the gear tooth width and "back-lash" ie "Clearance" which is set by increasing or (decreasing) the depth of cut to get the correct gear tooth width.

Gear tooth width/thichness can be measured with common shop vernier ir digital calipers. Gear calipers are not needed.

http://i200.photobucket.com/albums/aa294/oldtiffie/measuring/Gear-measure1.jpg

The centre/axis of the gear cutter and the centre axis of the job must be in the same vertical plane (assuming a horizontal mill is used). Rotate into the horizontal plane when using a vertical spindle/arbor.

Common tables while in accordance with "Machinery's Hand Book" are nominal only and if used would result in gears with no clearance.

http://i200.photobucket.com/albums/aa294/oldtiffie/Black_book/BB_50-51.jpg

http://i200.photobucket.com/albums/aa294/oldtiffie/Black_book/BB_52.jpg

I will enlarge on this later if I have time and if it is necessary.

Jaakko Fagerlund
12-11-2012, 03:51 AM
Not just about rigidity...... the real reason for NOT climb milling is if the machine has any slop at all in the feed.
That's what I said.

oldtiffie
12-11-2012, 05:40 AM
Not quite.

I was taught in at least one shop (many years ago) that climb milling is OK- if the cut it light - to "brake" the lead-screw hand-wheel with your (right) hand (light cuts only) which takes a bit of skill to aquire it - but it can work very well.

I use it on the lathe the "scrape" the trailing/rear thread face when screw-cutting - that works well too - but learn that skill first before you try it on something you might wish you hadn't if you get it wrong.

oldtiffie
12-11-2012, 05:42 AM
Here is the OP.


I am in the midst of cutting several spur gears. Because of the purpose I need them to be done "by the book". The book being Machinery's Handbook or similiar. In my career there have been many discussions of making spur gears. Some say that you must cut them in a single pass, giving no reason besides "thats how I was taught". Others state that you must cut them by climb milling also giiving the same reason or stating "thats how I always do it".

I would like any thoughts or facts that either substantiate or debunk those ideas. If you have other ideas to share that would be welcome also.

Thanks in advance

Pete

I am not sure that anyone has really addressed the OP's core requirements.

J Tiers
12-11-2012, 08:32 AM
That's what I said.

It IS?


Rigid machine/setup. Climb milling saves your cutter and thus makes it live longer AND the surface finish is just much more better.

People tend to advice against climb milling just because they always think the maker has only a clapped out crappy mill but don't even bother to ask. Many manual machines have ballscrews and there can always be the unusual CNC user (especially when asking if you can cut something with multiple passes).

Indirectly, if at all. That depends on what a "clapped-out crappy mill" is inside your mind. I expect that most everyone here has a "clapped-out crappy mill", as most don't have ballscrews with opposed angular contact bearings holding the screw. I "always think" that because of what I see people write.... Black Forest seems to have a different sort, but I don't think his equipment is typical of people here with Mill-drills, old Bridgeports, Clausings, Rockwells, etc.

Stepside
12-11-2012, 09:39 AM
There have been several good points raised by different members. The first being a lack of information provided. So in my case this time I am cutting 24DP gears on a ProLight CNC mill. The cutter is an Involute gear cutter that is brand new. I have found that cutting a gear to the handbook specifications seems to produce a gear with little if any clearance. I should have included this in my request for information.

I also use my Clausing horizontal mill to cut the larger gears. This particuliar machine has very little wear and is adjusted tight but I still would favor conventional as opposed to climb milling. My Bridgeport is beyond "clapped out" and is not used for this purpose.

What I have heard so far 1) Climb cutting is an option if you have ball screws in good condition. 2) Some like to multi-pass and some don't. 3) The handbook numbers are for a "zero clearance" gear set. 4) The answer depends upon the type of cutter, the machine being used, personal preference, and a few WAG's from those who failed to read the original questions.

Thanks to all who provided advice.

Pete

Gunsmithing
12-11-2012, 10:26 AM
The main reason for not Climb cutting is if some thing goes wrong it will cost you a $60.00 or more for a new cutter.

Dave


There have been several good points raised by different members. The first being a lack of information provided. So in my case this time I am cutting 24DP gears on a ProLight CNC mill. The cutter is an Involute gear cutter that is brand new. I have found that cutting a gear to the handbook specifications seems to produce a gear with little if any clearance. I should have included this in my request for information.

I also use my Clausing horizontal mill to cut the larger gears. This particuliar machine has very little wear and is adjusted tight but I still would favor conventional as opposed to climb milling. My Bridgeport is beyond "clapped out" and is not used for this purpose.

What I have heard so far 1) Climb cutting is an option if you have ball screws in good condition. 2) Some like to multi-pass and some don't. 3) The handbook numbers are for a "zero clearance" gear set. 4) The answer depends upon the type of cutter, the machine being used, personal preference, and a few WAG's from those who failed to read the original questions.

Thanks to all who provided advice.

Pete

Mcgyver
12-11-2012, 10:47 AM
The main reason for not Climb cutting is if some thing goes wrong it will cost you a $60.00 or more for a new cutter.


hehe, price arbors lately? you'll bend it as easily as breaking the cutter.

As I said early on the issue with climb milling is NOT whether the mill is clapped out, its wether its built for it OR whether the cut is so light the table's inertial & and table lock partially on (tough on the mill) is enough. Without an antibacklash mechanism (I think Harry posted some excellent pics of a classic one from a heavy mill) you will get many thou's of clearance in any acme thread - thats backlash. .005- .010 would be common and far from a clapped out machine. Plus what there is in the way of bearings taking the thrust. A brand new mill, not designed for climb milliing, will crash with a heavy cut on climb milling

Arthur.Marks
12-11-2012, 02:59 PM
I have found that cutting a gear to the handbook specifications seems to produce a gear with little if any clearance... The handbook numbers are for a "zero clearance" gear set.
Not exactly. You must always keep in mind that you are not milling the gear tooth but the space between the teeth. The "handbook specification" to work with is the Pitch Diameter, which is a measurement of the tooth itself. That is what accurately sizes a gear. The other relevant handbook figures should probably be qualified. The OD of the gear has a negative, unilateral tolerance. You can make it exactly to spec. but not oversize. By making the gear blank slightly undersize (remember to calculate your cutting depth accordingly less), you make the gear tooth less tall. The involute shape will still be the same; the pitch diameter will still be the same, but the overall height of the tooth will be slightly less. This increases the difference between the top of the gear tooth and the mating gear's root. That is one aspect of creating clearance. The other aspect of clearance is the root diameter achieved when you mill the teeth. All commercial spur gear milling cutters to my understanding of the standards will include an added clearance height to the gear cutter form. This results in a greater depth to the cut spaces which result in the gear teeth profile from the milling operation. "The [depth of cut] is also usually quoted on the actual cutter although it does not say depth of cut as such but is prefixed by the term D + f." (Gears and Gear Cutting, Ivan Law. pg.65) Where "D" equals the "Working Depth" and "f" equals "clearance." Clearance is furthermore defined as "the radial distance between the top of a tooth and the bottom of a mating tooth space, or the amount by which the dedendum in a given gear exceeds the addendum of its mating gear." (Machinery's Handbook Vol. 28, Large Print Edition. pg.2031)

In conclusion, if you are sizing your blanks no larger than specified and cutting to a depth which results in an accurate Pitch Diameter, clearance is provided for in both the "handbook specification" and the gear cutter form itself. Now, if you are talking about "backlash," that is a different matter entirely and is covered in the section "Backlash in Gears" in Machinery's Handbook starting on pg.2068 in my edition referenced above.

J Tiers
12-12-2012, 12:22 AM
hehe, price arbors lately? you'll bend it as easily as breaking the cutter.



Dontcha make yer own arbors? They are a lot cheaper that way, and you get any kind you want.

Mcgyver
12-12-2012, 06:46 AM
Dontcha make yer own arbors? They are a lot cheaper that way, and you get any kind you want.

I've built up the assortment I need one the used market included all the ground spacers. You might not buy the chrome moly for what the same dollars yield and it would be a lot of work making and grinding all the spacers.

If I had to shell out $700 each or needed non standard ones making them might be considered. The point of my crack off on the other post was when things go wrong on a horizontal more than just the cutter is at risk. Once was enough.

J Tiers
12-12-2012, 08:31 AM
I buy the spacers, that's too much like work..... Didn't have much choice, the main mill takes MT3 taper arbors. The other one (a Benchmaster) takes MT2, but that's a pretty light duty "hobby" taper for a horizontal mill, and it will be turned into a vertical soon with a new head.

mc_n_g
12-14-2012, 12:37 AM
I recently had to cut some gears and I made my own 'rack' style cutting 'hob' (for lack of a better term).
Ground a HSS toolbit to the proper 14.5 degree angles. Used O1 on my lathe and to get the proper depth I used a dial indicator.
Used plenty of cutting oil on the HSS bit. It was great to reach the proper speed and depth of cut and watch the chips come off all 3 sides at once.
The 'disks' of the 'hob' are cut with the gear formulas as if you are cutting a gear rack. This way the formulas are straight forward and dimensions are direct.
(use INVOLUTE GEAR DATA as search term in Google. Should be 1996 article from Model Engineers Workshop)
Roughed the flutes on my Sheldon/Vernon horizontal mill leaving about .005-.007 left to grind after hardening.
Flamed, quenched and then tempered in an old toaster oven.
The end results turned out well.
Cut the teeth on my dividing head mounted on my horizontal mill.
The first cut to get started was 5 or 6 passes. All subsequent teeth were cut in 3 passes with a 0.010" final pass.
The teeth are not as smooth as with an involute cutter but for the few metric threads I will be cutting the gears will work just fine.

http://i10.photobucket.com/albums/a140/mc_n_g/machinery/DSCN9757_zpsca606afd.jpg

http://i10.photobucket.com/albums/a140/mc_n_g/machinery/Making_hob_zpsd2c3dcbf.jpg

http://i10.photobucket.com/albums/a140/mc_n_g/machinery/Cutting_flutes_zps22b0e78b.jpg

http://i10.photobucket.com/albums/a140/mc_n_g/machinery/Cutting_flutes2_zps43446c03.jpg

http://i10.photobucket.com/albums/a140/mc_n_g/machinery/All_flutes_cut_zps16ff59f3.jpg

http://i10.photobucket.com/albums/a140/mc_n_g/machinery/Cutting_18DP_teeth_zps8d836b29.jpg

http://i10.photobucket.com/albums/a140/mc_n_g/machinery/Cutting_18DP_teeth_2_zpsfc5f0861.jpg

http://i10.photobucket.com/albums/a140/mc_n_g/machinery/Cutting_18DP_teeth_3_zps58ed79db.jpg

Abaker
12-14-2012, 09:56 AM
Nice work MC.

I see you are using a dividing head to hob. I'm thinking of doing something along those lines with my K&T universal DH. My only reservation is that the input gear train includes a very high angle helical gear made of brass or bronze - not sure if it's meant for that kind of duty.

Could you post a picture or two showing the drive train? - Thanks

Mcgyver
12-14-2012, 10:14 AM
Could you post a picture or two showing the drive train? - Thanks

I don't think there is a drive train as its not hobbing as per the correction definition of the term (no slight to the poster, he puts 'hob' in quotes as he knows its not a real hob), I call it faceted hobbing...again for lack of a better name. The 'hob' doesn't have a helix just V grooves at the pressure angle. The index head is used as it always is, ie index a tooth and take a cut. The result is a good approximation of an involute made of up of facets. It can work well but I've used this approach only for slow speed applications.

mc_n_g
12-14-2012, 12:29 PM
Mcgyver is correct, there is no gear train. It was cut one increment at a time but cutting different sections of teeth in the same pass.
That is why I identified the cutter as a 'hob'. It would open up another ball of wax here.
depending upon the diametric pitch and the number of teeth I can see nothing wrong with this method for simple home use.
I would not recommend this method for long term duty.
I cut my gears from 7075 aluminum and delrin and have not had any problems with them.
For an 18DP gear the tooth is very close to form but not a good smooth involute.
Also, my dividing head is just a simple dividing head and not the universal type with the additional gearing.

http://i10.photobucket.com/albums/a140/mc_n_g/machinery/cut_gears_view1_zpsc7510822.jpg
http://i10.photobucket.com/albums/a140/mc_n_g/machinery/cut_gears_view2_zps9c1024fe.jpg
http://i10.photobucket.com/albums/a140/mc_n_g/machinery/gear_after_cutting2_zpsb0184f68.jpg

Picture showing facets the best I could
http://i10.photobucket.com/albums/a140/mc_n_g/machinery/gear_zoom_facets_zps585ffafa.jpg

Arthur.Marks
12-14-2012, 12:38 PM
Excellent, practical example with clear documentation, mc_n_g. Thanks for sharing!

Wirecutter
12-14-2012, 01:32 PM
Listen to the machine and just watch the cut . Don`t push it just pay attention to what the machine and the set up is telling you . If you need ear plugs something is not right.

I couldn't have said it better, lane.

I have a Bridgy, and I sometimes climb mill for surface finish. Normally, it's in aluminum, and of course, not a heavy cut. Works great. The machine has acme, not ball screws.

Bill Pace
12-14-2012, 01:44 PM
While on the subject of "hobs", heres a link to my post on making up a worm and gear for my Sheldon lathe a while back. (please overlook the fact that I failed to put "hob" with the quotation marks, I am aware that it is not a 'real' hob) As mc_n_g noted this method is not for long term use, my "hob" cutter was pretty shot by the time we were through. Sure saved the Sheldon though, the apron was non-functioning otherwise.

http://bbs.homeshopmachinist.net/threads/54672-Making-a-worm-and-gear-for-a-Sheldon-lathe

Since that was done, I have had the lathe under operation for some time now and feeds and threading modes on the apron is working great.

lane
12-14-2012, 06:34 PM
For what you are doing you can easily cut 24 DP in one pass. As for as all said . They are right . But in machine work their is no have to do it this way method. What ever works for you. its your machines and your project .So I say get er Done what ever it takes right are wrong. One thing I have learned over the many years of doing this is what works for you may not work for some one else and vice adverser. To each his own way.

Mcgyver
12-14-2012, 09:02 PM
depending upon the diametric pitch and the number of teeth I can see nothing wrong with this method for simple home use.
[/URL]

absolutely, i hope my post wasn't taken as casting aspersions, just explaining the difference. I've used it and it works well.

mc_n_g
12-14-2012, 10:29 PM
Absolutely no harm Mcgyver. I did not take it that way. My wife is more angry at me than anyone on these boards.
If I was doing something long term I would recommend anyone buy a correct involute cutter (if available) and use better materials than I used.
I was happily surprised by the delrin. It cut cleaner than I thought it would.
I never used this method before and I think it is very handy for the homeshop.
I was worried about trying the Dean Williams method of making the cutter( he was not the first but has a fantastic website on the method) .
http://www.deansphotographica.com/machining/projects/multipoint/multipoint.html
I was worried the cutter was going to end up too thick and take out too much leaving the tooth too thin.
I think the excentric cutting to get relief is fantastic. The pictures are great and really shows how to do it.

vincemulhollon
12-16-2012, 08:54 AM
Some say that you must cut them in a single pass, giving no reason besides "thats how I was taught".

No one's mentioned it yet, but lets be honest here, if you're using a manual rotab, everyone screws up X percent of the time, doesn't matter if X is disturbingly large or impressively small, if you make 2 cuts you'll by definition make twice as much scrap as a one cut machinist, or if you make 3 cuts you'll make 3 times as much scrap... Also when you really screw up and destroy a cutter (sometimes arbor!) making 3 cuts per gear means you only make 1/3 as many gears, per destroyed cutter. Finally the labor cost of gear cutting is going to be directly proportional to the number of cuts.

Its a financial thing from a job shop, not an inherent technical issue. If you're mr super-machinist and never mess up, then technically one cut will cause less wear and less strange shaped profile wear, very much in theory, but the "destruction" and labor time effects swamp the wear argument unless your cutters are like 4 digits each and your labor is one digit/hr etc.

Stepside
12-17-2012, 01:16 PM
Here are the results: Basicly it depends upon the size of the project, the machines available, if it is for profit or enjoyment as well as the quality required.

So I used my "home built" dividing head/indexer, my ProLight CNC vertical mill and a new made in China" involute wheel cutter. I hand wrote the code to cut the teeth. The first time I conventional milled the gear in one cut. The results were usable but nothing special. The second time I climb milled the gear and used 3 cutter passes. he results were much better.
My next step was to use thread wires to check the gear for size. The gears were within .0005 of computed diameter.
Then I drilled and reamed two dowel pin holes in a plate the correct center distance for the two different gears. I pressed the pins in the plate and installed the gears and they ran great.
The gears had a reamed bore that fit the pins.
So my conclusion would be that the numbers work out and how you get there depends upon what you have in your shop and what the gears need to do.
Thanks for all the input.
Pete