High Helix Angle Crashing Hobbs - Is feed speed my issue?
Close
Login to Your Account
Page 1 of 3 123 LastLast
Results 1 to 20 of 45
  1. #1
    Join Date
    Mar 2020
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    15
    Post Thanks / Like
    Likes (Given)
    11
    Likes (Received)
    1

    Default High Helix Angle Crashing Hobbs - Is feed speed my issue?

    Hi everyone,

    I am currently cutting a 3 tooth helical gear with a high helix angle on a Barber Colman 6-10 gear hobber. So far, I have successfully cut several dozen of these gears, but I have shattered the teeth on two hobs in the process. I suspect feed speed is my issue, but I only have two hobs left, and I absolutely must cut these gears, so I'm reaching out for opinions before I try something else.

    My gear has the following specs:
    3 Teeth
    81.1° Helix Angle
    Left Handed Gear & Hob
    38 NDP
    .01” feed per revolution of work (is this too high?)
    Cut: Conventional
    Hob Rotation: CCW
    Direction of Feed: Left
    Work Rotation: Top Going
    Depth of Cut: .0592
    Outer Diameter: .5629
    Blank Size: .57
    Hob Spindle RPM: 412.5

    I have adjusted my worksheet to have a feed speed of .002" per revolution of work, but this is currently untested. Here is a link to the Excel workbook I have designed to make my gears: https://drive.google.com/open?id=121...PPHumwk5vwE5dX

    Does anyone have any ideas why my hob keeps chipping teeth off? Am I correct that my feed is too high? Is the hob spindle RPM off? I'm very open to any ideas or wisdom you might have as to why I'm having issues. I'm a novice at this, so I can't help but feel that I'm missing something obvious.

    Thanks again; I really appreciate any help!

  2. #2
    Join Date
    Jan 2005
    Location
    Victoria, Texas, USA
    Posts
    4,221
    Post Thanks / Like
    Likes (Given)
    2497
    Likes (Received)
    1091

    Default

    How about a picture of the part and the hob. Trying to understand a gear with 3-teeth on it. I'm no expert at gear hobbing but I would say that .010 feed is too high for sure, even .002" may be still be high feed rate for such a small part. I don't know. Interested. Where in Texas are you located?

  3. #3
    Join Date
    Dec 2008
    Location
    minnesota
    Posts
    177
    Post Thanks / Like
    Likes (Given)
    34
    Likes (Received)
    171

    Default

    3 tooth gear ???

    Do you mean a triple-start worm ?

  4. Likes 4GSR liked this post
  5. #4
    Join Date
    Apr 2018
    Country
    UNITED STATES MINOR OUTLYING ISLANDS
    Posts
    3,973
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1794

    Default

    Quote Originally Posted by petersen View Post
    3 tooth gear ???

    Do you mean a triple-start worm ?
    Basically, yes. OP, you are going to break lots of hobs and cry a lot. I did a bunch of 67* left-handers and hated every second of it. There is no good answer. If you told Barber-Colman what you were doing, their answer would be "DON'T !"

    Are you using a right-angle head ? Don't think you can even do it without, mostly just curious...

    Better way to do that is in a thread mill. Hobbers are not designed for that, if you look in the book you will see they go to 45* not 81*, it's possible but awful and will destroy a lot of cutters. Also workpieces when the hob shatters in the middle of the cut. Don't even think of trying climb.

    I had slightly better luck with a 1 mod taking it in three cuts with an opposite-hand hob. Yeah, triple-cut a 1 mod

    Sucks, there's no way around it

    Your setup better be rigid as hell and the machine tight to even have a tiny chance. The slightest quiver in the part and it's bye-bye hob, bye-bye part. Time to shift to a new set of teeth and scrap that blank ....

    Pure conjecture here but if you are trying to one-cut it, I'd go to two cuts and leave the feed alone. It's not the feedrate breaking teeth, it's that you have a whole bunch of teeth in the cut at once and the load is sideways instead of fore-and-aft and hobbing isn't supposed to work that way. Even the tiniest little vibration means suddenly the cutter is taking a big bite (big, for a tiny cutter.) Snap.

  6. Likes Milland, Panza liked this post
  7. #5
    Join Date
    Mar 2020
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    15
    Post Thanks / Like
    Likes (Given)
    11
    Likes (Received)
    1

    Default

    Quote Originally Posted by EmanuelGoldstein View Post
    Basically, yes. OP, you are going to break lots of hobs and cry a lot. I did a bunch of 67* left-handers and hated every second of it. There is no good answer. If you told Barber-Colman what you were doing, their answer would be "DON'T !"

    Are you using a right-angle head ? Don't think you can even do it without, mostly just curious...

    Better way to do that is in a thread mill. Hobbers are not designed for that, if you look in the book you will see they go to 45* not 81*, it's possible but awful and will destroy a lot of cutters. Also workpieces when the hob shatters in the middle of the cut. Don't even think of trying climb.

    I had slightly better luck with a 1 mod taking it in three cuts with an opposite-hand hob. Yeah, triple-cut a 1 mod

    Sucks, there's no way around it

    Your setup better be rigid as hell and the machine tight to even have a tiny fighting chance. The slightest quiver in the part and it's bye-bye hob, bye-bye part. Time to shift to a new set of teeth and scrap that blank ....
    I'll post some pictures tomorrow when I get back into the office. What's killing me is that we have, for many years, successfully cut some 3 tooth helical with a 74 degree helix without any issues. After looking at their setup sheets, they have a very low feed rate (.00375" per rev of work). I'll post those tomorrow too.

    Part of our problem is that we inherited these hobbers and their accompanying product line without a mechanical engineer or machinist to go with them, so a lot of our learning has been trial and error.

    Regarding the head, both it and the gear are left handed. The Barber Colman manual suggested that you use the same handed hob as the gear for high angle jobs.

    Thanks for all the comments so far; I'll add more info tomorrow like I said.

  8. #6
    Join Date
    Apr 2018
    Country
    UNITED STATES MINOR OUTLYING ISLANDS
    Posts
    3,973
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1794

    Default

    Quote Originally Posted by JasonGGI View Post
    After looking at their setup sheets, ...
    'scuse me ? If you have setup sheets and they were doing this for years, is there some reason you don't just do what was working ?

    Inquiring minds and all that ...

  9. #7
    Join Date
    Mar 2020
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    15
    Post Thanks / Like
    Likes (Given)
    11
    Likes (Received)
    1

    Default

    For some reason mobile keeps deleting my replies. Sorry if I'm spamming.

    I currently do not have a working set up sheet for the gear I am attempting to cut which is a 3 tooth 81.1 degree Helix angle. I have a working set up sheet for a 74 degree Gear with similar aspects that we have successfully cut for many years. I was simply listing the successful build as an example that I think it's possible to do what I am trying to do.

    For the gear I am trying to cut with an 81° helix, there is a Google Drive Link in my original post that takes you to the setup sheet that I have designed that, so far, isnt quite working. I suspect my feed rate is the issue.

  10. #8
    Join Date
    Sep 2014
    Country
    UNITED STATES
    State/Province
    Georgia
    Posts
    381
    Post Thanks / Like
    Likes (Given)
    286
    Likes (Received)
    147

    Default

    I think I would make these in a cnc lathe, but...

    The below is copied from a first edition B-C Hob handbook copyrighted in 1954.

    The set-up for machining worms is the same as for hobbing helical gears. The ratio of the work spindle rotation to the hob spindle rotation depends on the number of threads in the worm and the lead angle. A definite relationship must be held between the index and feed. The worm hob must be swivelled to the lead angle of the worm, with compensation for the lead angle of the hob. Normally, the swivel is turned to such a large angle that interference may be encountered using a standard swivel. A special 90 degree hob swivel is available for these applications.


    Although worm milling cutters are normally applied to thread milling machines, they can also be used very satisfactorily on hobbing machines. The thread form on the worm is the same as would be produced on a thread milling machine. Worm milling on a hobbing machine is usually restricted to single or double-thread worms, with hobbing being recommended for three or more threads. Cutting double-thread worms with a single cutter requires an indexing device and is best accomplished on a thread milling machine. With a duplex cutter, however, a hobbing machine is applicable since indexing is not necessary.


    When worms are milled on a hobbing machine, the feed change gears are arranged to move the cutter one worm lead per revolution of the worm. The index change gears produce the feed, and they are determined to give the desired chip-load per tooth. To obtain the desired cutter setting angle, a 90 degree hob swivel is usually required.


    For both hobbing and milling, if the worm does not extend to either end of the shaft, the work is fed radially to full depth and then axially for the required length. The axial feed must be engaged before feeding the work radially, and the feed should not be disengaged until the machine is stopped or the part is raised out of the cut. For production runs, a cam vertical feed unit can be designed to feed the work automatically to depth.

    Shown below is the right-angle attachment:

  11. Likes Milland liked this post
  12. #9
    Join Date
    Apr 2018
    Country
    UNITED STATES MINOR OUTLYING ISLANDS
    Posts
    3,973
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1794

    Default

    David, have you ever actually done this ? It's a little different reading about it in a book, you know.

    Normally, cutting forces are directed into the table and they are generally along the axis of the part. Setups are stiff in this direction.

    When you swivel the cutter to where it is almost parallel to the blanks, the cutting action is now trying to make the arbor vibrate, instead of just pushing down onto the table. Also, rather than one tooth totally in the cut and one tooth on each side partially in the cut, you end up with an entire hobs' worth of teeth in the cut. This is tremendously different.

    A worm cutter has ONE tooth in the cut, not six or seven.

    Hobbers are generally designed to do up to a 45* helix angle on gears. Worms are slightly different. Hobbing a high-helix like this can be done, it's common on camshafts, but they use special hobs and frequently have a steady rest / support right behind the hobbed area..

    In short, it is a BITCH, not the simple process you think by reading about it in the operator's manual.

  13. #10
    Join Date
    Sep 2014
    Country
    UNITED STATES
    State/Province
    Georgia
    Posts
    381
    Post Thanks / Like
    Likes (Given)
    286
    Likes (Received)
    147

    Default

    Emanuel Goldstein,

    Are you saying that the home-study course on becoming a foreign diplomat may not work out as well as I expect? J/K

    I was editing as you typed. I added that it is a quote from the Barber-Colman Hob handbook (just being a lowly messenger). I, also, added that it looks like a cnc lathe job to me.

  14. Likes daredo222 liked this post
  15. #11
    Join Date
    Apr 2018
    Country
    UNITED STATES MINOR OUTLYING ISLANDS
    Posts
    3,973
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1794

    Default

    Quote Originally Posted by David_M View Post
    Are you saying that the home-study course on becoming a foreign diplomat may not work out as well as I expect? J/K
    Like me learning to become a card shark ? Umm, yeah

    I, also, added that it looks like a cnc lathe job to me.
    Might be easier .... but it can be done, the underlying problem is vibration and the arbor is so small, there's no rigidity. A tiny little bit of vibration and there goes the teeth on yor hob It's like getting a little chatter on an end mill and you lose the endmill, except hobs cost a few hundred bucks each.

    Of course materials and all that enter ito it too ... would have been nice if OP had mentioned they already made these before and he had some indications of what worked for them ... I mean, if three thou feed worked why try ten ?

    Sigh.

    Every situation is different when you do these weird-ass things ... every single part of the setup counts and you have to try different stuff until you get a method that works. Then you WRITE IT DOWN because there are so many variables. What worked (sort of) for me doing a similar thing was probably different than him ... I did several lighter cuts and feared the vibration like the devil. My parts were 4140, don't know what his are. I gave that job back to the customer, found him a machine, taught him how to use it, and got the hell out of the way. That machine had a differential which is not supposed to do high helixes but we got it working. (Thats the one zahnrad was skeptical about, he'd never seen one in the flesh. The 6-10 diff is a mystical device, seldom seen by mortals

    That's how nasty this job can be .... but if his shop was doing it for years, they developed a method that works, yay. All he has to do is re-find it. 400 rpm sounds kinda fast to me but who knows ... what matters in this case is getting away from vibration, not the surface speed of the cutting tool. That's why teeth are chipping, the part quivers a little then boom goes london, boom paree, might as well drop the big one, those teeth are gone.

    It won't come out of the book tho. That's for sure.

  16. Likes David_M liked this post
  17. #12
    Join Date
    Mar 2020
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    15
    Post Thanks / Like
    Likes (Given)
    11
    Likes (Received)
    1

    Default

    Quote Originally Posted by EmanuelGoldstein View Post
    would have been nice if OP had mentioned they already made these before and he had some indications of what worked for them ... I mean, if three thou feed worked why try ten ?

    Sigh.
    I haven't made THIS particular gear before, my company has cut a similar one. As to why I choose a .01" feed rate, well, I am a desk jockey with ZERO machinist/engineering experience. As I mentioned before, my company inherited this product line and pretty much just followed the 30+ year old laminated setup sheets for the EXISTING designs. A customer asked us to revive an older gear ratio, so I decided to take a stab at it.

    I am entirely self-taught. I spent around 4 hours each morning for about 5 straight work weeks studying our 50+ year old Barber Colman manual, reading college textbooks, and trolling the internet trying to understand how and why these hobbers work. After brushing back up on all my old collegiate math, I managed to create an excel workbook that auto calculates all of the trigonometric functions for me, but I was at a standstill. I was missing a single variable: the feed rate.

    You can see my excel workbook for my CURRENT TARGET here: https://drive.google.com/open?id=121...PPHumwk5vwE5dX

    After a few weeks of beating my head against the wall someone told me that the feed rate was a variable that was selected by the operator and not a function of the gear itself. He told me that .02" was a good starting point for the types of gears we generally cut. Of course, now I realize that .02" is far too fast for my current operation, so I choose to cut it in half. It is clear now that that is still way too fast. I went digging through our old archive of setup sheets and found a 74° helix angled 3 tooth gear that we have cut many times when I looked up our inventory records and its feed rate was .00375".

    Of course, none of the shop employees know why or how the feed rate is determined, so no one here knew better to tell me that my selected feed for my current project was stupidly fast. They simply follow what the old setup sheets tell them to do (which is partly WHY I started this project because I wanted to build some institutional knowledge about our product line).

    Quote Originally Posted by EmanuelGoldstein View Post
    400 rpm sounds kinda fast to me but who knows ... what matters in this case is getting away from vibration, not the surface speed of the cutting tool.
    What would you recommend for a proper hob spindle speed? I think the lowest I can drop it to 18/36 for a hob spindle speed of 300 RPM.

    Quote Originally Posted by 4GSR
    How about a picture of the part and the hob.
    I've cut a few dozen of my desired gear between hob crashes, so here's a freshly cut sample that hasn't been heat treated: 81.1deg Successful Cut - Album on Imgur

    Here is a setup sheet for an OLD high angle gear that I just pulled out of the archives: OLD Working Setup with 80deg Helix - Album on Imgur This part was last cut successfully about a decade ago. Note the .00375" feed rate (which I did NOT until now when I discovered this part's existence recently).

    Finally, here's a picture of my current setup complete with hob with broken teeth: Hobber Setup - Album on Imgur

    So, from what I've written here, is the consensus that I'm just feeding way too fast? In addition to cutting an already idiotically high/risky angle?

  18. Likes 4GSR liked this post
  19. #13
    Join Date
    Sep 2014
    Country
    UNITED STATES
    State/Province
    Georgia
    Posts
    381
    Post Thanks / Like
    Likes (Given)
    286
    Likes (Received)
    147

    Default

    You can't arbitrarily change the feed rate. It is tied in with the index.

    This is what I have come up with for your change gears as best I understand your situation.

    Index constant: 6
    Feed constant: 0.0375
    Helix angle: 81.1 (dms: 81°06'00.0000")
    Diametral pitch: 38 (Module: 0.668421)
    Number of teeth: 3
    Transverse pitch dia.: 0.510291327618 (12.961mm)
    Outside dia.: 0.562922906565 (14.298mm)
    Lead: 0.25104333868378812199 (error: 0.00000027383350092844)
    Act. feed rate: 0.0026150319255 (0.07mm)
    Using: Left-handed hob to cut: Left-handed gear
    Type of cut: Conventional
    Constant-one sign: Minus
    Direction of cut: Top going

    Intermediate studs: Index: 2; Feed: 2
    Hob threads: 1

    This uses a C constant of 32 (it is scaled up from 32(/1) to 192/6 for this problem)

    Index error: none

    6 x 1 x 192 = 1152 = 16 x 72
    (3 x 192) - 6 = 570 = 30 x 19

    After doubling the 16(driver) and 19(driven):

    32 x 72
    ---------- Index change-gears:
    30 x 38


    0.08267349088394 / ((192 x 0.03750000 x 0.98795986576939) / 6) = 0.069734184680635331541012

    0.0697342607454967005528 = (17 x 23) / (89 x 63)

    Feed error: 0.0000000760648613690118687


    17 x 23
    ----------- Feed change-gears:
    89 x 63

  20. Likes JasonGGI liked this post
  21. #14
    Join Date
    Mar 2020
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    15
    Post Thanks / Like
    Likes (Given)
    11
    Likes (Received)
    1

    Default

    Quote Originally Posted by David_M View Post
    You can't arbitrarily change the feed rate. It is tied in with the index.
    David,

    Thank you for the detailed reply. I want to make sure I fully understand your comment, so forgive me if I'm asking the obvious. I know that the feed rate is tied into the index and many other variables, but I've set up my spreadsheet to take this into account and change the index gear ratios and so on. Isn't the feed rate determined by the difficulty of the cut and the material being cut? I can cut the same gear at different rates. I've sped up slower cuts without issue and slowed down more difficult ones. Is the rate you've given me the "ideal" feed rate for my 3 tooth 81.1° helical?

    For example, if I plug in .00375" for my feed, I get an Index gear ratio of 2.002992006.

    If I use your feed rate of 0.0026150319255" my workbook comes up with an index gear ratio of 2.021052638.

    No matter what IGR I come up with based on my feed rate, I simply use a ratio calculator to find my setup gears (while keeping the total difference under .000015 between the actual and desired ratio according to the Barber Colman 6-10's instruction manual).

    Let me know if you want a copy of my excel calculator I've built if you just to see what I'm talking about.

  22. #15
    Join Date
    Sep 2014
    Country
    UNITED STATES
    State/Province
    Georgia
    Posts
    381
    Post Thanks / Like
    Likes (Given)
    286
    Likes (Received)
    147

    Default

    Quote Originally Posted by JasonGGI View Post
    David,

    Thank you for the detailed reply. I want to make sure I fully understand your comment, so forgive me if I'm asking the obvious. I know that the feed rate is tied into the index and many other variables, but I've set up my spreadsheet to take this into account and change the index gear ratios and so on. Isn't the feed rate determined by the difficulty of the cut and the material being cut?
    Yes, that is extremely important to do.
    Using the desired feed rate, you calculate the C constant that determines how much the part is rotated out of sync. The intentional rotating of the part "out of sync" combined with the feed rate determine the helix angle (feeding faster or slower while keeping the same index gears changes the lead angle and helix angle).

    Quote Originally Posted by JasonGGI View Post
    I can cut the same gear at different rates. I've sped up slower cuts without issue and slowed down more difficult ones. Is the rate you've given me the "ideal" feed rate for my 3 tooth 81.1° helical?
    I think is is a lot better (safer) than 0.010". Feed rates for this are faster than the numbers sound because the part is rotating into the cutter as the cutter is fed into the part.

    Quote Originally Posted by JasonGGI View Post
    For example, if I plug in .00375" for my feed, I get an Index gear ratio of 2.002992006.

    If I use your feed rate of 0.0026150319255" my workbook comes up with an index gear ratio of 2.021052638.

    No matter what IGR I come up with based on my feed rate, I simply use a ratio calculator to find my setup gears (while keeping the total difference under .000015 between the actual and desired ratio according to the Barber Colman 6-10's instruction manual).

    Let me know if you want a copy of my excel calculator I've built if you just to see what I'm talking about.
    Here are some other index and feed gears for ~ 0.002 feed:

    Index change-gears: 43 x 98 / 41 x 51 driver x driver / driven x driven

    Feed change-gears: 16 x 19 / 92 x 65 driver x driver / driven x driven

    no index error and a feed error of: -0.00000000094

    Act. feed rate: 0.001906

    Lead: 0.25104306020066889632 (error: -0.00000000464961829723)

    I'll add to my answer a little later.
    Last edited by David_M; 03-24-2020 at 07:27 PM.

  23. Likes JasonGGI liked this post
  24. #16
    Join Date
    Jul 2006
    Location
    Hillsboro, New Hampshire
    Posts
    8,913
    Post Thanks / Like
    Likes (Given)
    2140
    Likes (Received)
    6161

    Default

    While I'm not a gear expert at all, I do think that the failure of the hob teeth is from a sideward loading, not an "over feed" condition. That would "mesh" (sorry) with the idea that you've not matched the relative gear/hob rotation ratio correctly.

    [Edit: Or have some other condition that's leading to side loads]

    Interested to hear what the more knowledgeable gear guys have to say.

  25. #17
    Join Date
    Sep 2014
    Country
    UNITED STATES
    State/Province
    Georgia
    Posts
    381
    Post Thanks / Like
    Likes (Given)
    286
    Likes (Received)
    147

    Default

    I looked at your spread sheet and I see that the circular pitch is off by a small amount, but what is off more is the C constant. You have 41.84049744. The actual C constant for 53 * 90 / 26 * 91 is 41.8421052631578947368421052631578...

    If you use your C constant to calculate the feed gears it will cause an error you are not seeing in your double check.

    I know that your C const is calculated from the feed you want, but your index change gears don't match up with that.

  26. #18
    Join Date
    Jul 2006
    Location
    Hillsboro, New Hampshire
    Posts
    8,913
    Post Thanks / Like
    Likes (Given)
    2140
    Likes (Received)
    6161

    Default

    I heard from an anonymous source that there's always some sidewards forces on the Hob teeth during this sort of cutting, but:

    A) If that's the case, could the hob teeth be ground for clearance?

    B) Going back to #16, does anyone else think the tooth failure in the #12 pic is from side load, or am I all alone in the wilderness?

  27. #19
    Join Date
    Mar 2020
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    15
    Post Thanks / Like
    Likes (Given)
    11
    Likes (Received)
    1

    Default

    Quote Originally Posted by David_M View Post
    I looked at your spread sheet and I see that the circular pitch is off by a small amount, but what is off more is the C constant. You have 41.84049744. The actual C constant for 53 * 90 / 26 * 91 is 41.8421052631578947368421052631578...

    If you use your C constant to calculate the feed gears it will cause an error you are not seeing in your double check.

    I know that your C const is calculated from the feed you want, but your index change gears don't match up with that.
    Fascinating.

    Regarding my NCP Error

    Looking at my spreadsheet I had an error in Pi. I had 3.14159165 and NOT 3.14159265. I have now corrected it to 3.14159265358979. My new NCP measures at 0.0826734908839418, is that what you get?



    Regarding my C Constant Error

    Can you tell me where I'm going wrong? Was my "only" using 9 digits of Pi the problem? My C constant is NCP / (SIN 81.1° X Feed Rate) or now 0.0826734908839418 / (0.987959866 X .002) = 41.84051081 which does not match your C of 41.8421052631578947368421052631578

    Am I using the wrong formula?

    Thank you again, David. I really feel like I'm closing in on the issue.

  28. #20
    Join Date
    Sep 2014
    Country
    UNITED STATES
    State/Province
    Georgia
    Posts
    381
    Post Thanks / Like
    Likes (Given)
    286
    Likes (Received)
    147

    Default

    You aren't doing anything wrong. I think you are missing a couple of important steps.

    Most people who do this simplify the C constant to a whole number, then look for an exact match. If the first whole number doesn't work they go to the next larger whole number and try again until they get an exact match.

    My method is somewhat unorthodox because, like you, I choose the gear set closest to the calculated C constant. At that point I figure out what the chosen gear set's exact C constant is (in the form of a fraction. Only fractions are always exact) and substitute it for the calculated one.

    This shows how I use the fraction in the formula using your example shown here


    The C constant for it is 21 1/3 (exact) (~21.333333333333333333...)

    21 1/3 = 64/3

    Working in fractional only math for the index (the denominators cancel. Though you do use it in place of the normally used '1' because C is scaled up by the denominator's value) :

    64 * 6 = 384 * 15 = 5760 = 90 * 64

    (64 * 3) - 3 = 189 * 15 = 2835 = 63 * 45


    feed:

    0.07853981633974483096156608458199 / ((64 * 0.0375 * 0.98713626507298792100490470465575) / 3) =

    0.09945412188602157080119885902369 =

    0.00372952957072580890504495721339 (feed for most accurate tooth form)
    0.0037295330503335 (closest choosing from 16-100 with no dups)
    0.0000000034796076910949550427866 (error)

    16 * 41
    97 * 68

    feed from the example:

    0.00372952957072580890504495721339 (feed for most accurate tooth form)
    0.00375 (actual feed in the example)
    -0.000020470 (error, not bad, but could be a little better)

    24 * 22
    66 * 80

  29. Likes JasonGGI liked this post

Tags for this Thread

Bookmarks

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •