Grinding chip breakers on HSS toolbits

This is where bits of wisdom will be stored, a frequently asked question section with answers.

Moderators: Harold_V, WJH

spro
Posts: 7541
Joined: Mon Feb 20, 2006 11:04 pm
Location: mid atlantic

chip relief

Post by spro » Fri Jan 12, 2007 12:44 pm

The quality of your writing delivers a clear picture. It makes perfect sense. There will be more questions no doubt. Take any absence of them as an indication you have helped more than you..aw crap i just wanna say Thx GUYS! oh btw you too, harold :)

User avatar
BadDog
Posts: 4744
Joined: Wed May 17, 2006 8:21 pm
Location: Phoenix, AZ

Post by BadDog » Fri Jan 12, 2007 3:12 pm

Still, my poor guidance is probably better than no guidance.
As a rank newbie, I very much appreciate you and others who take the time to pass along your knowledge. And I would say that, at least for me, your guidance has been far from “poor”. In fact, I would say that your guidance is “great” rather than “poor”.

Thank you...
Russ
Master Floor Sweeper

spro
Posts: 7541
Joined: Mon Feb 20, 2006 11:04 pm
Location: mid atlantic

chip relief

Post by spro » Fri Jan 12, 2007 4:41 pm

The chip relief info is then going to how to generate that without a straight wheel to start that cut and what happens after as radius increases on the wheel edge. This does not mean to distract but a thought about your grinder. Many as you know have on the right side a thread which fits a Jacobs chuck. This secured chuck can hold what you need for individual reliefs by means of expendable grinding or cutoff wheels. This would not be promoted but is done.

Harold_V
Posts: 17630
Joined: Fri Dec 20, 2002 11:02 pm
Location: Onalaska, WA USA

Re: chip relief

Post by Harold_V » Fri Jan 12, 2007 7:02 pm

spro wrote:The chip relief info is then going to how to generate that without a straight wheel to start that cut and what happens after as radius increases on the wheel edge. This does not mean to distract but a thought about your grinder.
Spro,

If I follow your point, which is a good one, you're suggesting that a grinding wheel would gradually evolve with a radius that is greater than may be desired for a chip breaker to be ground to desired specifications. If so, that isn't usually a problem. When you use a wheel that is suited to grinding HSS, it gets dressed on a fairly regular basis. While I didn't count, I dressed the wheel no less than five times when I ground the tool pictured. As a result of the fairly constant dressing, the wheel tends to keep a relatively sharp corner. Fact is, if you can grind such a tool without dressing the wheel, the wheel is magnitudes too hard, and grinding will a slow, laborious process. You'll come to understand that HSS grind quite well if you use the proper wheel, which I'll address in a future post.
Many as you know have on the right side a thread which fits a Jacobs chuck. This secured chuck can hold what you need for individual reliefs by means of expendable grinding or cutoff wheels. This would not be promoted but is done.
How one achieves a chip breaker isn't important. I grind almost all of them with the corner of a wheel, or by installing an old, worn out wheel that has been dressed with a desirable radius, which was the case with the tool in the original post. The negative in these instances is that wheels are formulated to run @ given surface speeds, and start losing hardness (not really---but they behave as if they do) as surface speed diminishes. That's not all bad in that you can often grind a chip breaker without overheating the edge. You experience rapid degradation of the wheel, but that's a small price to pay for the successful grinding of what is usually an excellent cutting tool.

There are times when the side of a wheel is not capable of grinding a desired breaker. I've included a picture of such a case, below. Sorry for such a lousy looking tool, but it has sat for years in less than ideal conditions, and it shows. The change in angle of the tool eliminated the possibility of grinding it as I normally would. It was ground many years ago, so I can't say with certainty how I achieved the breaker, but I am inclined to think I used an air grinder with a mounted point. Any port in a storm, so to speak. How you get there isn't important, not so long as you achieve success, without rounding the cutting edge.

The Jacobs chuck mounting you speak of would be particularly bad, although functional, if one uses mounted wheels for grinding chip breakers. Small wheels of that nature require speeds well in excess of 10,000 rpm in order to perform properly, but, again, that's of little significance if they serve the purpose.

Harold
Attachments
CHIPBREAKER.jpg
CHIPBREAKER.jpg (5.11 KiB) Viewed 8228 times

spro
Posts: 7541
Joined: Mon Feb 20, 2006 11:04 pm
Location: mid atlantic

chip breaker

Post by spro » Sat Jan 13, 2007 10:56 pm

Origionally saw that tool as not too bad but upon relooking at the pic see where the front edge is now nearly below center and since not using lamppost holder it is pretty much off the mark for shim even with face ground. I'm not trying to hold you up or anything. This has been some of the best advise but I can't really offer anything. I do remember a tool ground like that and it worked very well for awhile. It was probably right old and didn't fit into textbook portrayal of what that tool should look like.I know now why it worked and why it failed.

torker
Posts: 195
Joined: Wed Jan 14, 2004 12:59 am
Location: Southern BC, Canada

Post by torker » Sun Jan 14, 2007 1:31 am

Harold_V wrote:
torker wrote: I've been battling with a couple of thinwall 3 1/2" deep bores all week in my spare time. It hasn't gone well.
Material? Thickness of wall? Diameter of bore? Tolerance? Fighting chatter? Through bore, or to a shoulder?
I normally use brazed carbide boring bars and when sharpened right they aren't bad but they require a lot of pressure and high rpm.
That's because they generally lack proper geometry for free machining. If readers come away with nothing more than the understanding that a proper chip breaker changes the way a tool performs, almost always for the better, each will have learned a valuable lesson. Relief angles on tools play a far less important role than some may have you believe. What really matters is how the tool sees the work-----rake. It also often dictates tool life----so there are times when one must compromise.
I've got one of the bars for HSS that uses a short piece of 1/4" toolbit sticking out at 90*. I've tried a lot of different profiles but haven't had the success I should. I think I know what you will say...I should grind a narrow chipbreaker groove along the length of the short bit...correct?
I'm inclined to say yes, but without knowing more, I hesitate. Thin wall work can be exceedingly tricky---whether you're turning or boring. I'd want to know a lot more about your setup, including the nature of the bar, diameter (of the bar) , if you're running on center, speeds and feeds, and, of course, what material, what tolerance, and what kind of surface finish you're trying to achieve. Sort of a repeat of the above things I mentioned. It's all important if you're trying to solve the mystery. Some things can be unreasonable and make the task border on the impossible without addressing the job from a different perspective.
That's what you told me for a facing tool for alu and it worked well. I never thought of doing this with a bit for steel.
That's the beauty of chip breakers. They work on almost everything----although hard materials shorten their lives considerably. Tough materials can yield surprising results, however. It's important that you understand the difference between hard and tough. They're not the same thing.

The nature of chip breakers for steel as opposed to aluminum would be a slight reduction of rake angle----and if the machine is light duty, width and depth may have to be adjusted accordingly. A shallow cut with fine feed would require a narrow breaker, and shallow, in order for the chip to curl. By contrast, a deep cut with heavy feed would require a wider and deeper breaker. Rake angle may have to be altered to prevent edge failure----which can be accomplished by using a larger radius for the breaker. As the radius increases, the angle diminishes, and it isn't nearly as deep. These features are best determined by trial and error, so the tool suits the exact conditions in which it's being employed.
I'm getting a very rough finish....my point is too sharp. I keep getting the nose a bit rounder but it's still not nice. I theenk I'm going about it all wrong. I've been using a typical 60(ish) deg profile with the point sticking out the side. Have a decent chip breaker ground in it but it's looking wrong now that I see your.
Thanks again!
Russ
If you try something that resembles a tool in my post and are still having trouble, post a picture of your tool and lets see if we can figure out what the problem is. I agree----you're probably going about it wrong, but that's how we learn. You should build a strong, lasting impression of what doesn't work from this experience. It's all part of arriving as a machinist.

Harold
Harold...Sorry for the time lapse...been very busy.
The pieces I'm trying to bore aren't a "deep" bore as you would imagine...they are just deep to me....cuz of my noobness...lol!
It is 2" sch40 pipe(2.20 od if I remember right). The bore is 4 1/2" deep.The final wall thickness is .090.
I have about 3" sticking out of the chuck. I turned the od first....maybe not right but I wanted to see if it would distort before going any further.
I'm a bit handicapped with my lathe(14X40 Asian junk). The fine feed is .008 per rev but I am getting decent finishes with properley shaped cutters on the OD.
The finish inside these is very rough. Hoping to get a tool ground up like yours tomorrow. I've built a cutter/endmill grinder gadget and want to try freehanding on it. The thin edge cup wheel should work well. I'd like to make an adapter for Zip cut discs that I use on my angle grinder. They might work well for that chip breaker.
I'm sure if I follow your direction it'll be much better than what I have now.
I'll let you know.
Russ

Harold_V
Posts: 17630
Joined: Fri Dec 20, 2002 11:02 pm
Location: Onalaska, WA USA

Post by Harold_V » Sun Jan 14, 2007 2:01 am

Pipe is inclined to machine quite poorly, so you may be experiencing some of what goes with machining material that isn't really intended to be machined.

Finish turning the outside before roughing the inside is always a mistake. Parts, regardless of their nature, are best fully roughed before any finish cuts are taken. That allows any stresses that cause movement in material to be relieved as much as possible, then the error created by the movement is removed in final machining. That's pretty much industry standard, at least prior to CNC operations. I worked light production work for years, and that was pretty much the accepted practice. The added benefit is that you remove scale prior to applying your finishing tools. It's hard on edge life.

A tool in keeping with the design I showed will improve your performance, particularly for finish cuts. Again, it's important that you get all the scale out of the pipe before attempting finish----it's terribly hard on tools, especially HSS, which is far softer than carbide. The positive rake helps shear the material------instead of tear it.

You might consider following Kap's advice in this instance, at least for roughing. His modified flat chip breaker increases edge life considerably under harsh conditions, although you lose the benefit of shearing action from positive rake. The chip breaker would allow for chip control, and the narrow flat area will provide a much more resilient cutting edge, albeit at the cost of higher machining pressures. Go to the high rake for finish, after the scale is removed.

By the way, this is a great place for using soft jaws. You're going to have fits with a wall that thin, holding the part adequately without crushing it. Soft jaws (wide ones) prevent crushing, with the added benefit of minimizing chatter. Give it some thought.

Harold

torker
Posts: 195
Joined: Wed Jan 14, 2004 12:59 am
Location: Southern BC, Canada

Post by torker » Sun Jan 14, 2007 11:24 am

Thanks again Harold! I wasn't sure about the sequence for "roughing/finishing" What you say makes sense.
I found the worse part of machining the "hi tech" sch40 was roughing out the first pass with the welded seam on the inside...lots of interupted cutting til the seam was gone. That's where I first got into trouble after I'd thinned down the OD. The interupted cut caused some shifting and makes me believe that I should rough out the inside first when working with this stuff.
You have me thinking about the soft jaws now. I guess the idea there is to mount them then bore them to a close profile of the tubing/pipe that you want to grab...correct?
Thanks!
Russ

Harold_V
Posts: 17630
Joined: Fri Dec 20, 2002 11:02 pm
Location: Onalaska, WA USA

Post by Harold_V » Sun Jan 14, 2007 3:50 pm

torker wrote: You have me thinking about the soft jaws now. I guess the idea there is to mount them then bore them to a close profile of the tubing/pipe that you want to grab...correct?
Thanks!
Russ
That's the approach I'd use.

I'd like to point you to a post I provided long ago, in which I discuss the use of soft jaws. They are, in my opinion, the magic bullet of lathe work, and would be the perfect solution to holding your project. If you're inclined, please check this link:

http://www.chaski.org/homemachinist/vie ... php?t=4266

I had posted some pics originally, but I don't think they'll display now due to changes in the software the board has used. If there's any interest, could be I can re-post them. I still have them available, but I don't know if I can add them to such an old post. If not, I'd be pleased to send them to you on the side if you feel they'd be useful.

In the case of pipe, I'd make wide and long jaws that support it almost 100%--and use the "spider" I spoke of for fine adjustment. With the soft jaws bored to accept the rough OD of the pipe, I'd bore the pieces within .03" of finish size, then make a setup to rough turn the OD, again, within .03" of finish size. At this point you should have relaxed the majority of stress pent up in the material, and can go for finish sizes, starting with sharp tools. I'd turn the OD to size first, then re-bore the soft jaws to fit. Finish cuts would be virtually perfectly concentric (should be within .0005" if you've done your work well), and chatter would be a non-issue, due to the full support of the tube. Because you would desire full contact of the jaws to material, it's important to hold all the pieces identical in size, say within ± .001". That way the radius of the jaw will match the radius of the pipe and not distort it. I talk about jaw to part fits in the referenced post, so that will give you proper guidance on fitting the parts to the jaws.

Hope some of this helps, Russ. How about a report on the final product?

Harold

torker
Posts: 195
Joined: Wed Jan 14, 2004 12:59 am
Location: Southern BC, Canada

Post by torker » Sun Jan 14, 2007 8:32 pm

Yes it helped...cept I have 1 piece jaws :cry:
I'll post a few of my projects when they are close to done. I have my endmill grinder nearly completed but the tubing I'm making right now is a bit of R+D so I can mount a stepper motor and cnc controls to my rotary table. I have a bunch of gears to cut in the future and this'll make it easier.
Thanks again....have a lot of reading to do now...all the writing you did will take a bit to soak into the ol' noodle!
Russ

User avatar
SteveM
Posts: 6859
Joined: Mon Jun 27, 2005 6:18 pm
Location: Connecticut

Post by SteveM » Sun Jan 14, 2007 10:11 pm

Russ,

Also check out:
http://www.chaski.org/homemachinist/vie ... hp?t=75448
and you'll see some additional discussion and some shots of the "soft jaws" I made for my "hard jaws".

You'll also see an example of Harold's "spider" in use.

Steve

torker
Posts: 195
Joined: Wed Jan 14, 2004 12:59 am
Location: Southern BC, Canada

Post by torker » Mon Jan 15, 2007 12:09 am

Steve...Thanks for the link! Now I'm sold on soft jaws for sure. I just need to replace my three jaw with a real chuck now. Ow...they are pricey though. The Buck chuck in the KBC catalogue is worth as much as my lathe :cry:
Good to see a pic of a "spider" also. Cool looking gadget!
Russ

Post Reply