Need Help! Diagonal Hobbing - Page 3

1. ## Re: Diagonal Hobbing

large end of hob is toward "top" of machine
hello corey cutting forces are :
... getting bigger ( or lower ) during the cutting, or
... are constant ( because depth decreases while cutting edge length increases )

in all these cases, i think that is better to have the hob with the smaller diameter near the M spindle, so to have increased rigidity when finishing

as i have seen from the program, the hob is under the part; if you wish to flip the hob on the arbor, than the hob must be above the part when cutting simply replace in your program YPOS=-1 with YPOS=+1 should work of course, real trials are required so to take a decision about hob orientation

it will take some time to get your requested info. This machine hasn't sit idle since we got it in april
15minutes should be more than enough time for measuring the hob inside the cnc i proposed this variant, because it provides data from the clamping position, thus measuring the tool where it will be used

of course, tool may be measured also externally the cnc

is good, from time to time, to run trials on the cnc / so to die smarter

I think the hob angle u want is on the cutter but it doesn't hurt to double check i suppose
i need the taper of the cutting edges; edges are disposed on a cone; the conicity of the tool

in image 1 i represented the segments for 2 rows of teeth; each row of teeth has the cutting edges colinear, among a generator; all these generators are intersecting right at the top of the cone ( image 2 )

i need the cone angle ( 2*alfa from image 3 )

you may measure it inside another cnc, or just ask for this value from the tool provider ( hoping that is not a resseler, but the manufacturer of the tool )

again : what i am doing with this hob story is not something that i have done before, so i hope it will work

2. ## Re: Diagonal Hobbing

please, what is the purpose of this comment : (INTERRUPT SUBROUTINE) + (ACTIVATED BY YELLOW BUTTON) ?
It's for the big yellow Emergency Return button right above the "e-stop" button.... it makes the tool escape out of the cut if the operator doesnt like how something looks or sounds. But the "feed hold" button does the same thing during the hobbing cycle.

Okuma made contact this morning so hopefully help is on the way.

BTW, How can i tell if i have the flat turning option?

3. ## Re: Diagonal Hobbing

hi, maybe your Okuma rep has a good application guy but diagonal hobbing is not common ...

flat turning allows only this ratios : 1:n, where n=1,2,3...6; this function realizes the sync between S&M axis, but you allready have the M556 that is designed for hobing so ...

however, if you are really interested to see if you have it, simply run a specific flat turning code, and, if you dont have it, an alarm about specs will occur / kindly

4. ## Re: Diagonal Hobbing

It's been almost a full revolution around the sun and i have another order of these bastard parts coming up real soon... okuma was no help on this at all so im back doing more research and getting mentally prepared for frustration, anxiety and finally a victory when i present a good part to my boss. Has everyone brushed up on diagonal hobbing in the past year??

5. ## Re: Diagonal Hobbing

ooo, happy birthday corey far as i remember, there was a missing piece in that puzzle, which involved the tool angle ( cone angle )

did you delivered those parts ? if so, simply run that program again ...

otherwise, pls share drawing and tool photo, and i will try to help best as i can / kindly

ps : 1year ? time is flying don't worry, i have never done diagonal hobbing; i imagine the required movements, try to calculate the ratios and code it ....

6. ## Re: Diagonal Hobbing

hello i have been thinking about this : is required to "sync the rpms" and to "find the ratio for Y&Z axis"

- syncing the rpms :
... n1 = live tool ( hob ) rpm
... n2 = part ( spindle ) rpm
...... n1 / n2 = hob_nr_of_teeth / part_nr_of_teeth ( should be something pretty close to this )

- finding the ratio between Y&Z :
... if y is not moved, you should end up with a straigth gear
... inside the machine, you may measure a few points :
...... among the blue line in image 1 ( maybe for 2-3 different C angles ); from those points you may check how close you are to the value from image 2
...... among the yellow line in image 1, thus to compare the simetry of the right & left flank

even if you measure the hob, in the end, you still have to measure the part, so maybe is better to measure only the part

to shorten the trials time, don't cut the full gear from 1st time, thus don't cut until z2.484 is reached, but a smaller distance : on this smaller distance, measure, adjust, and recut

one more thing : be sure that there is no play inside the live tool transmission, thus that the hob is cutting at constant rpm; if there is play, it may be possible to detect it by checking the rpm displayed inside "axis data menu - this menu has a higher display refresh rate" ( also a discontinuous sound may be there, etc ); if part does not has a nice surface rugosity, it may be because of the play : consider a light-finish final cut same for trials : light passes, so to end up with a nice smooth part, that should be easier to measure; if you go hard, and there is play and/or rigidity issues that are not taken into consideration, downtime & wtf moments will appear

i would start easy, smooth, and when measurements are ok, i would increase the specs, or maybe rough+finish increasing the specs should deliver a part with increased surface rugosity, but all should be ok if dimensions are inside given tolerances, or part functionality is acceptable

kindly

ps : i am still woking on my teleport tower-sledge, otherwise i would be santa-claus, helping you find a good-part on monday morning; i am also digging tunels deep underground, but i have no clue where they end up ...

7. ## Re: Diagonal Hobbing

Very interesting! Who manufactured the hob & what information came with it? Seems like you'd need to know exactly where the hob needs to be positioned (along its length) when it's centered over the beginning of the spline. You'd also need to know exactly how far the hob needs to shift over as it cuts the length of the spline. Once you have that information you should be able to figure out how much to adjust the RPM of the work piece to get straight teeth.

8. ## Re: Diagonal Hobbing

You'd also need to know exactly how far the hob needs to shift over as it cuts the length of the spline
hi technical ted measuring the cone among the blue line, in image 1 from my previous post, will show how close is the angle to the desired 3*16'44"

measuring the flanks ( yellow line ) will show how good the ZYsync is, because a wrong shift will destroy / damage the flanks

all these measurements can be done inside the machine, with the part in the spindle ( i guess light cuts are recomended, for a good surface finish )

i believe that finding the good ZYsync is a priority, and i would run trials to achieve the middle of all flanks among a straight line, or pretty close to this ( at this point the tapered root angle should be pretty close to hob taper )

Seems like you'd need to know exactly where the hob needs to be positioned (along its length) when it's centered over the beginning of the spline
if ZYsync is known, then simply lower / raise the start position of the hob, until the "circular tooth thickness=6.239-0.05( image 2 )" is achieved at "pitch_dia=56( image 2 )", at a position where root_dia=52.77(image 1a)=tool_base_diameter(image 3)

this can be measured inside the machine, with a 3d taster ( with minimal tir and a palpator with a ball_dia=2.5mm; at this size, there is still 0.362 clearance until the tapered root - image 1c )

well, so far so good, but the tool has a different taper then the required value from the drawing; tool has 3*11'55"=3.199* ( image 3 ) while the technical drawing shows 3*16'44"=3.279* ( image 2 previous post )

i would run some trials until i would obtain the taper from the tool 3.279*, and after that i would target the taper from the drawing 3.199*, and compare results : at this point i should be pretty close to something; ( well, close but no cigar )

kindly

9. ## Re: Diagonal Hobbing

Good morning guys and thanks for the response. It will be at least a week, maybe longer before i begin setup on these so i can't do any trials or testing until then. However, i am running a straight tooth spline now that i may be able to play with as the job winds down. Same principle would apply to traverse the tool diagonally, but also would take the taper out of the equation... but this job is running so well i hate to mess with it! Probably best just to solve original problem first, then apply it to other parts later as to get full use of the hob with least amount of wear..

Anyways to answer a few questions. Sync of z and y? Should be whatever its supposed to be i guess? Machine is 18 months old and luckily no hard crashes. A few bumps that required a turret alignment but nothing major. Nobody else ever runs this machine. I do not understand how the spindles are synced, the machine gear software does this for you when u plug in values for no. of teeth on cutter and no of teeth on part etc.

P.S. the tapered root spline part in question has an angular tolerance of -+ 2 degrees!!!
Gleason made the tool, it has alot of info on it and pictures are in some previous posts toward beginning of thread.
Last order of these parts that i did, well lets just say we had to bend over and take it from an outside source... 4-5k on a 44 pc. order and it took them 3-4 weeks

10. ## Re: Diagonal Hobbing

this job is running so well i hate to mess with it!
hey corey if you wanna mess with it, but still be safe, target small changes, thus to be sure that the tool won't fail

i guess there is no problem if the part is a failure, but tool has to be protected

Sync of z and y? Should be whatever its supposed to be i guess?
aha ... that's it

Machine is 18 months old and luckily no hard crashes. A few bumps that required a turret alignment but nothing major
i have custom load-monitor code, that is designed to increase safety, more precise to reduce the force that trigers motors-shutdown

it may save the day, may lower the turret deviation, or stop before turret goes missaligned, or stop before a tool is broken

[ protection during positioning ] : find the "torque value" parameter, and lower it as much as possible; should be inside "system parameters"
[ protection during cutting ] : use a general load monitor address, for all axis : for example, at the begining of the program, i load 80%limit into all axis : XZCYM; no limit in S

so far it saved me at least 4 times

I do not understand how the spindles are synced, the machine gear software does this for you when u plug in values for no. of teeth on cutter and no of teeth on part etc
i remember that you have that fancy software ... it outputs G-code, and it would be nice to understand that code, so to adjust it faster

maybe you can run some trials with a representative from Gleason he may tell you to input 0.2 somewhere, and like this, you will get the part in no-time

however, he may tell you to change a parameter that is not available as input directly into the software interface / kindly

11. ## Re: Diagonal Hobbing

Hi Corey – 1st thing I would do is try to contact the person who posted the video that Deadly linked in post #11.

Here’s what I think you will have to do:
1) Calculate how far the hob must shift to get the full depth root diameter and taper to zero depth.
2) Let’s say the above dimension is 2.473695. Divide that by .494739 (circular pitch). That equals 5.
3) So the workpiece would have to rotate 5/14 more (or will it be less) to compensate for the hob shift.
Does this make sense to anyone else? I’ll work on some of the math & we can compare results.

12. ## Re: Diagonal Hobbing

Calculate how far the hob must shift to get the full depth root diameter and taper to zero depth
hello technical ted, you are right ... there is an image at post #20, which shows the part/material and the tool/hob in contact; the taper on the part depends on the taper of the tool, and in that moment i suggested that is a good idea to measure the tool, so to calculate Z_travel & Y_shift with a precision of few tenths

after that, rpms has to be calculated; tool_rpm/part_rpm=tool_nr_of_teeth/part_nr_of_teeth ( i guess ) / kindly

#### Posting Permissions

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