What's new
What's new
By:
Advanced search…

Carbide Hob Grinding - Feeds and Speeds Questions

R

rhadfield

Plastic
Joined
Jun 28, 2021
The shop I work at recently picked up an Anca FX3 to grind our HSS and carbide hobs. I am new to grinding and looking for information on grinding carbide.

I have read that carbide hobs are sharpened in one pass at full depth with a slow feed rate. However, this information is out of a shop book that is older than I am and much of the information is outdated.

I have had semi-good finishes using the same program I use for HSS hobs, but with a diamond wheel. The tolerances for AA ground hobs are tight, so I am seeking any information to improve my process.

Thanks in advance.
 
Hopefully Carbide Bob will chime in here, but I would call your grinding wheel manufacturer and speak with them. Everything I have read about carbide hob sharpening is that's its better to sharpen more often and remove less material than to wait for the hob to wear excessively and then have to remove a lot of material. Interested in what you find out. Welcome to PM!
 
Was going to say the biggest biggest MOST IMPORTANT thing when sharpening hobs is to make sure the face of the teeth is exactly radial (unless the hob is marked as having a hook, so always check.) ITW had charts showing what happens to the involute when you get the cutter face off radially, and it ain't pretty. That's even more important than finish or index spacing.
 
The programs used with these hobs has hob shift after every part and sharpened after one full pass across. The wear is minimal for carbide.
I have been experimenting with the amount of removal, removing less and less. The finish and grind quality is noticeably better with a lower material removal

Thanks for the advice.
 
EmanuelGoldstein said:
Was going to say the biggest biggest MOST IMPORTANT thing when sharpening hobs is to make sure the face of the teeth is exactly radial (unless the hob is marked as having a hook, so always check.) ITW had charts showing what happens to the involute when you get the cutter face off radially, and it ain't pretty. That's even more important than finish or index spacing.
Click to expand...

Thanks for the advice. The Anca I use does a pretty good job of probing the flute face. Flute rake is < 5 microns.
 
Just curious- how much are you hob shifting after each part in relation to the circular pitch? Have you seen any difference shifting after, say 10 parts? thanks in advance.
 
rhadfield said:
The programs used with these hobs has hob shift after every part and sharpened after one full pass across. The wear is minimal for carbide.
I have been experimenting with the amount of removal, removing less and less. The finish and grind quality is noticeably better with a lower material removal

Thanks for the advice.
Click to expand...

I've only minor experience sharpening carbide Hobs, but a bit more sharpening Carbide Shaper Cutters since we started making them ourselves. My experience agrees with this completely. I've found that sharpening more often, and removing surprisingly little translates directly to greatly improved life and quality of cut. We now only take a few tenths off to retain performance. This also has the benefit of preventing some of the more spectacular failures. You might find that your coolant medium will have more impact now that you've gotten to this point. Carbide Bob will have much good information in that area, too. Good luck.
 
Update

After some trial and error, I have found parameters that yield very good results.

Rough - 0.002" stock removal, 6 in/min at 4000 RPM
Semi-Finish - .0006" stock removal, 10 in/min at 5000 RPM
Finish - .0002" stock removal, 20 in/min at 5500 RPM with a spring pass

I am also grinding wet.

The resulting hob rake, lead, and flute spacing are all well within AA standards. Often, rake and flute spacing are < 1 micron.

I believe the semi-finish is not required, but the best results are with the extra pass. We only grind a hand full of hobs per week, so the extra 5 minutes is not a problem.
 
EmanuelGoldstein said:
Kinda intersting that hob sharpening is generally dry, while shaper sharpening is generally wet. Never wondered about why before ... you gotta answer ?
Click to expand...

No, I've never really thought about it to be honest. LOL. I think it is likely something to do with the fact that so many of the Hob Grinders I've encountered are remnants from 50 years ago, or more. When I have rigged up a tool grinder or more modern grinder to accommodate grinding Hobs, I've always used the coolant available for doing so. Admittedly, I've not done it for some time now. These days ( with our own shop ) it is just SO much easier to pay someone else to do it. When I was younger, I did it because it was part of that thirst and quest for knowledge. Nowadays, it's a tooling maintenance that gets planned...

The only reason we sharpen our Shaper cutters is because we make them and have purpose build fixturing that makes it simpler. I would not have any problem sending out the HSS ones though.
 
I understand the logic of sending the tools out for sharpening. The company I work for is owned by a Japanese company that requires us to send our hobs to them for sharpening, which is a 3-4 week process. This is the reason we began doing it ourselves.
 
Everybody is different.
Rough pass at only .002 seems very light but the 6 per minute good for me at say .010-.040 per pass.
How much are you removing?
Skip the semi, not worth the time to setup right.
Finish at 20 ipm is way faster than I would go but I do not do 2 tenths passes on any carbide wet.
I ass-u-me different wheels in use for these ops. If not one is stuck with a finish wheel for everything.
If you walk into ten carbide shops you will get ten different answers.
If it works good for you it works and that is what matters.
I would rough with 120-180 and finish with a 400-600 or even finer.
Surface finish on that tooth matters a lot for tool life as it reduces chip sliding friction and heat. This is a bigger deal in hobs where SFM is not that high.
Bob
 
Bob,

Thank you for the information.

I am currently using only a 320 grit wheel.
Typically removing .003-.004 is enough to remove wear on the teeth. The hobs are, mostly, 50mm diameter and a DP of 50-200. The teeth are very small on the majority of the hobs.
Seems like you would recommend removing all of that in one pass?

I understand that every shop will give different answers. I was thrown into this project with no experience with grinding and limited resources for gaining knowledge so I appreciate any guidance.


Thanks again,
Ryan
 
You must log in or register to reply here.

Similar threads

S
Drilling speeds and feeds for tool steels D2, H13, O1, S7, W2
Replies
9
Views
336
Dan from Oakland
D
avivz
Spindle design for low speed carbide grinder
Replies
13
Views
1K
neanderthal mach
N
rons
The nature of a carbide edge and what care it likes the best?
Replies
10
Views
1K
dian
D
TokeloSello
The correlation between speeds, feeds and depth of cuts for a better finish ??
Replies
6
Views
576
Marc 1982
Marc 1982
P
Unusual Grinding Spindle, Friction Drive Perhaps?
Replies
4
Views
624
Peter S
P








 

ABOUT PRACTICAL MACHINIST

With more than 10.6 million unique visitors over the last year, Practical Machinist is the most visited site for metalworking professionals. Practical Machinist is the easiest way to learn new techniques, get answers quickly and discuss common challenges with your peers. Register for the world’s largest manufacturing technology forum for free today to stay in the know.

Learn more about us.

STAY CONNECTED

Facebook Instagram YouTube LinkedIn Pinterest Twitter Tiktok

Register Become a forum member. Register today.

Sign Up Sign up for our e-newsletter.

© 2024 Copyright Practicalmachinist.com. All Rights reserved.

Back
Top