1911Forum banner
1 - 20 of 26 Posts

·
Registered
Joined
·
37 Posts
Discussion Starter · #1 ·
Is there a noticeable difference in chatter between HSS and carbide tools on a mill, specially on the smaller tools given everything else being the same?

Reason I ask, will be ordering tools for my mill soon, most of which will be carbide but intend to order some in HSS as 'rough hoggers' and as a cost saving
measure.

Or is this something that the difference is so minuscule as to not worry about
in general and can easily be mitigated by varying spindle/feed rate?

Thanks
 

·
Premium Member
Joined
·
3,371 Posts
Tool chatter is an artifact of loose bearings and/or lack of rigidity in the tool (for the specific cut). Carbides are more rigid and more tolerant of heat (can be run faster).

Many people order roughing mills TiN Coated. Less expensive than carbide and tougher so they can run them faster.

Properly lubricated, at the proper feeds/speeds, with good bearings you should not get chatter with either. Finish might be a little better with carbide.

Cheers!
 

·
Registered
Joined
·
197 Posts
Carbide is more rigid than HSS, and in some instances carbide will deflect enough less to be a factor in reducing chatter or poor surface finishes. Cases where the tool is long compared to diameter are an example. Usually, the tool relief and rake angles have more effect on whether a tool is prone to chatter or not. Chatter can usually be reduced usually by increasing the chip load, either reduce the rpm or increase feed rate, or both. Normally a good HSS cutter will cut as well as carbide if the material is not too hard and proper speeds and feeds are used, but will wear faster. Some tools are ground for certain applications, and may not work well outside those applications, but some are junk and tend to chatter no matter what. Some brands are inconsistent from tool to tool.

On CNC equipment, we use almost all carbide tooling except most drills because it is more economical by far. If we were using HSS steel we would be doing nothing but replacing tools all day long. Carbide tools usually get taken out of service because of chipped edges, while HSS wears away until too dull for use. Most CNC machines are rigid and don't have backlash plus they run at higher rpm, but Bridgeport type manual mills are not as rigid and have backlash, and that will break carbide if you don't know how to work with it. Carbide doesn't flex or take shock very well. Think of carbide as being like glass, and HSS as being like plexi-glass.

HSS steel can be more cost effective on manual machines, especially while learning the ropes. If you are killing HSS tools, you are either trying to cut material that is too hard, the surface speed is too high, or the tool is overheating.
 

·
Premium Member
Joined
·
3,371 Posts
By the way, that is one VERY nicely finished WC frame you have there.

Excellent!

Cheers
 

·
Registered
Joined
·
3,236 Posts
If you tool around the Internet you will find a speed and feed chart which is a good guide. Also look at the Practical Machinist forum for some guidance . I also think MSC and Travers have the speed and feed charts along with a guide for the tool coatings which seems to get more complex every year.
 

·
Registered
Joined
·
37 Posts
Discussion Starter · #8 ·
It was kindly pointed out to me that I neglected to mention
what I intend on cutting. (thanks Pete!)

Ordered a Grizzly G0704 and plan on cutting aluminum, carbon steel
and stainless steel for 1911's and possibly AR style weapons.

Thanks again all, very valuable information and it IS appreciated!

-Ray
 

·
Registered
Joined
·
197 Posts
For steel, in general, you will want to use a 4 flute end mill. For aluminum, a 2 or 3 flute usually works best, I prefer the 3 flute medium to high helix flutes, like the ones in the link below. We use a lot of Niagra end mills, but haven't had the best luck with Accupro, though I suspect they would work fine with the rpm your mill will turn, and they are less expensive.

Niagra :http://metalworking.mscdirect.com/CGI/NNSRIT?PARTPG=IMLMPLW&PMPXNO=5882296

Accupro: http://metalworking.mscdirect.com/CGI/NNSRIT?PARTPG=IMLMPLW&PMPXNO=7912544

I think you would best off with 3 flute tools for aluminum cutting on your mill, they should cut smooth if the mill and setup is rigid enough, and the speeds and feeds are in the ballpark. I doubt you will be removing metal at a rate where 2 flutes are of benefit. The 3 flutes will give a finer finish than 2 flutes with a low rpm spindle. You can get 2and 3 flute end mills in HSS as well as carbide. Uncoated tools should be fine, and are some cheaper.

Four flute end mills can be used on aluminum for certain types of milling, but usually have more issues with chattering and aren't generally ground properly for aluminum anyway. Aluminum is more forgiving than steel, so you might get away with using carbide although at first HSS might be good to learn with. The cutting forces of high helix end mills will pull up hard on the parts, so keep that in mind if you use them, as the part needs to be extra secure to prevent uplift, pulling the tool out of the collet is possible if not tight enough.

MSC (in the links above) sends out sales fliers and catalogs regularly. We get discounts almost weekly, some weeks only good for xx% off certain products, some weeks good for xx% off most products, sometimes the discount is 25-35%. If you aren't in a hurry, place a small order or set up an account to get on the mailing list (they send emails, faxes, and catalogs through regular mail), and buy when the items are on sale. They also have the sales catalogs online under special offers.
 

·
Registered
Joined
·
344 Posts
Get your hands on an Onsrud catalog and read the appendices over and over untill you have a firm grasp on chip load.

Sometimes this is counter intuitive, and you'll find yourself wanting to slow down the feed rate, when just the opposite is what is really required.

We bumbled around at work for some time on a particular job and finally achieved the desired results (chatter free, clean cutting, improved tool life, etc...) by increasing the feed speed x4. The decreased cycle time was a nice dividend as well ;)
 

·
Registered
Joined
·
45 Posts
i am reading this post and i must speak up ,i spent my day standing at a bridgeport maching mostly stainless,17-4 most of the time,75 % heat treated.
if you are going to machine ss ,get your self some endmills with a .015 radius on the end . they will last much longer and give a better finish. and USE COOLANT. and keep your aluminum end mills seperate from your ss steel ones.
tighten up the nuts on your way screws,and if you have to, the gibbs. coated endmills are fine for ss,there is realy no sense in using carbide for soft steel,they WILL wear out if you run them too high! a half inch em. in soft ss at 700 rpm will cut fine,2000 for brass or alum, but in heat treated ss, keep the depth of cut low and wet. this isnt something i can put on paper,i just know when i am standing at the machine,i know what seems right . many times right in the midle of a cut ,i stop and change.i have been doing this for 35 years. just my 2 cents,and yes i do all my own and my friends gunsmithing,tis so e-z when you have all the toys.
 

·
Registered
Joined
·
197 Posts
i am reading this post and i must speak up ,i spent my day standing at a bridgeport maching mostly stainless,17-4 most of the time,75 % heat treated.
if you are going to machine ss ,get your self some endmills with a .015 radius on the end . they will last much longer and give a better finish. and USE COOLANT. and keep your aluminum end mills seperate from your ss steel ones.
tighten up the nuts on your way screws,and if you have to, the gibbs. coated endmills are fine for ss,there is realy no sense in using carbide for soft steel,they WILL wear out if you run them too high! a half inch em. in soft ss at 700 rpm will cut fine,2000 for brass or alum, but in heat treated ss, keep the depth of cut low and wet. this isnt something i can put on paper,i just know when i am standing at the machine,i know what seems right . many times right in the midle of a cut ,i stop and change.i have been doing this for 35 years. just my 2 cents,and yes i do all my own and my friends gunsmithing,tis so e-z when you have all the toys.


Just to expand on this, the tooth corners are the weakest part of the tool, and a radius or a 45 degree bevel is stronger than a sharp point. For end mills that have small chips on the corners but are otherwise serviceable, one can use a diamond wheel or hone to dress the corners up and make the end mill good again.

I tend to run a little more rpm, but that's with CNC's and production work, for soft steel/stainless and some tool steels 2-3,000 rpm with a 1/2" end mill (carbide), and 10-15,000 rpm in aluminum and brass (1/2" carbide also). Some 2" to 3" face mills up to 15,000 rpm in aluminum, depends on the particular tool and if it is balanced for high rpm.

The low rpm machines will give a finer surface finish in a lot of cases by using the smallest diameter tool that is rigid enough, because the tooth/flute pitch is less. The surface speed will be even that much lower than what it could run at, but the results will still be good. A side benefit to using smaller tools, assuming they are rigid enough like I mentioned and otherwise fill the bill, is they are less expensive.
 

·
Registered
Joined
·
2 Posts
Carbide vs HSS for small mills is an interesting question, and chatter may not be the limiting factor.

There is a trade off in material removal rates and rigidity within the envelope your mill is capable of. For example, chiploads are generally higher for HSS than for Carbide, all other things being equal. So, for a given rpm, you can remove more with HSS. However, carbide will tolerate a much higher rpm that will offset this and overcome it if you can go to a high enough rpm.

Where rigidity is concerned, I would think about two rigidity issues. First is tool deflection, especially for smaller tools. Many machinists are surprised at just how much small tools can deflect. I have software called G-Wizard that does tool deflection calculations, and I can say that if you're running less than a 1/2" diameter tool, it may be a lot more than you expect. You should keep the tool deflection below 0.001" when roughing to minimize the likelihood of chatter.

Chatter is a resonant phenomenon. Think of a tuning fork. Something is struck and it oscillates. You can either try to make a more rigid tuning fork, or reduce the "striking" that pumps the energy to keep the chatter going. When the tool flexes, it "pumps" the chatter, so reducing the flex reduces the energy available to cause chatter. Carbide is 3x more rigid than HSS, so it is harder to get it to chatter, all things being equal.

Keep tool stickout to a minimum, and you reduce the length of the tuning fork's tines. Less chatter. Increase your tool diameter, even just a little bit, and you have a much more rigid tool. A 1/2" HSS EM sticking out 1" is 9.5x more rigid than a 3/8" HSS EM sticking out 1".

Second issue is machine rigidity, always a scarce commodity for smaller machines. Deal with this via horsepower. For every action, there is an equal and opposite reaction. The horsepower from your spindle pushes the cutter which pushes the workpiece which pushes the workholding which pushes the machine, and back around to the spindle. Do see another tuning fork coming up?

So if you have a 2 HP spindle, consider that if you run a 2 HP cut, you're pumping the max into the tuning fork. You can back it off if chatter is a problem, or at least be aware that the closer to the limits you come, the more likely the chatter. Leave plenty when roughing for a light finish pass that pumps very little chatter. Calculate the cut's HP vs your machine's HP to estimate how much margin you have available.

Lastly, chatter is a resonant phenomenon (tuning forks again). Your machine and tooling has natural frequencies where it likes to resonate. Your job is to avoid exciting those frequencies. You may be able to do that not just by going slower, but also by going faster, oddly enough. Always try increasing feedrate, then increasing spindle rpm, before slowing down, to see if that gets you out of the chatter zone.

What should a small shop with a lightweight mill do RE carbide vs HSS?

Buy carbide below some size. I like carbide in 1/2" diameter or less. The small tools suffer most from lack of rigidity. Buy HSS in larger sizes where the bigger diameter vs the relatively low HP of a small mill means you have enough rigidity. Big carbide is the most expensive anyway.

The limiting factor on small carbide is that it is brittle. Particularly for very small endmills, if you have much runout in your spindle or toolholder, you're going to break more cutters. I prefer ER collet chucks for small tools. Be sure to measure the runout if you use import tooling. I had a bad collet one time in an otherwise good set that broke 3 cutters before I finally tracked it donw.

Cheers,

Bob Warfield
www.cnccookbook.com
 

·
Registered
Joined
·
45 Posts
do you need a square bottom if you are cutting a slot? if you dont then the .015 radius will suit you fine.its not esay trying to hone or grind a corner radius on an endmill,i can do it better than most, but when push comes to shove, i use a factory ground endmill.our main customer is very picky when it comes to corner radius's,if the print says .025 plus or minus .005 it better be that, or its reject time. just to put it all into perspective ,i made surgical intruments,just think of that next time your in an operating room on the table.
 

·
Registered
Joined
·
344 Posts
Welcome aboard the 1911 Forum Bob. Glad to see you here... your contributions will be very welcome...

Reprinting from another source is a copyright violation
All those who hang out on CNCZone are well aquainted with Bob's many excellent machine shop articles and his CNCcookbook web site is crammed with all kinds of great how-to information... He also publishes the G-wizzard program if I'm not mistaken.

I'll have to swing by and see what new inventions you've bolted on your CNC RF-45. Wish I had downloaded G-wizzard when you had the free beta version up.

Any cool gunsmithing projects in the works?
 

·
Registered
Joined
·
5,745 Posts
Yeah it took me a while to see that Bob was the blogger and actually reprinted his answer to our original question here on the blog. I have been poking around a few of the machining web presences to try to understand some of the gunsmith picture threads. Man I wish I had some room... I crammed in a drill press and I'm about to have to throw out the washer & dryer. Yeah that'll happen.:biglaugh::biglaugh:
Joe
 
1 - 20 of 26 Posts
This is an older thread, you may not receive a response, and could be reviving an old thread. Please consider creating a new thread.
Top