PDA

View Full Version : Face Mill?



pntrbl
05-23-2010, 08:14 PM
I've had a Seig X3 for a few months now and I think I need a face mill for it. I've been using end mills to get surfaces flat and what I've found is I'm wearing the corners off of the poor little things in an unreasonably short amount of time. Wrong tool for the job?

My manual says the machine is face mill capable up to 2" dia, but 95% of the time I'm working with mild steel and an X3 is not a behemoth of a mill by any means. Maybe I should tone that down to a 1.5" dia?

I've looked at the usual places. ENCO, Wholesale Tool, etc. But there's such a crazy amount of info on cutting angles, insert types, and so on that I quite frankly don't know what to pick.

Any help is greatly appreciated.

SP

oldtiffie
05-23-2010, 08:45 PM
I have both a Sieg X3 as well as a Super X3. Both are rated at/for a 2" face milling cutter. I have a "high-rake" 2 1/2" face milling cutter that I bought for my HF-45 square-column mill and it works quite well on the X3's.

Just take it easy - the X3's are a very good small bench-top mill - but they are not as "big" as my HF-45 which in turn is by no means a "production" mill either.

This is my 2 1/2" cutter:
https://www.machineryhouse.com.au/Products?stockCode=M516

I am thinking of getting a 2" for my X3's so that I don't "thrash" or over-load them:
https://www.machineryhouse.com.au/Products?stockCode=M515

J. R. Williams
05-23-2010, 08:46 PM
Build a simple Fly Cutter Tool and save your money.

JRW

tmc_31
05-23-2010, 09:07 PM
pntrbl,

I have a RF-31 mill that I use a 2" face mill on with very good results. You just have to adjust your DOC to suit your mill. Also if you face anything wider than your face mill you will wind up with a ridge you will have to fix with a file. I couldn't tell you if my machine is more or less rigid than yours.

That said, I must agree with J.R.. I bought a cheap set of fly cutters (3) from CDCO and have been using the cheap brazed carbide lathe bits from HF with excellent results. Again you have to set your DOC to suit the Mill and the material you are using (with a flycutter you will want to only take off a few thou at a time). Another advantage to the flycutter is you can adjust you width of cut.

I had purchased the 2" face mill, then the first project I did on the mill was 3.5" wide.

The way I have been running at these facing on wider material is to rough with the face mill and then go back and take a final cut with the flycutter.

Tim

beanbag
05-23-2010, 09:33 PM
45 degree face mill like old tiffe said. I think less inserts is better. Sharp inserts take less cutting force. Go with a very light DOC at first, and go heavier until you can hear the spindle being battered. Then back off. I prefer the cutter with an integrated shank, like 3/4", so you can just stick it right in your collet without worrying about getting an arbor. I have a sandvik RA-245 face mill which I like very much, but I know that it causes spindle battering in a Bridgeport knockoff with greater than .02 DOC. (I think that spindle is a little loose anyway, or rather, the interface between the spindle and pulley)

oldtiffie
05-23-2010, 09:39 PM
The OP's question was about face milling cutters and that is why I answered as I did.

But I'd always prefer to finish with a fly-cutter - either a TC or HSS tool - HSS preferred.

If using a HSS cutter I prefer to set it to just a bit wider than the cut and to have it climb milling - it enters with a wider chip instead of "rubbing" - but be careful.

See:

Conventional milling versus climb milling

A milling cutter can cut in two directions, sometimes known as conventional or up and climb or down.

Conventional milling (left): The chip thickness starts at zero thickness, and increases up to the maximum. The cut is so light at the beginning that the tool does not cut, but slides across the surface of the material, until sufficient pressure is built up and the tooth suddenly bites and begins to cut. This deforms the material (at point A on the diagram, left), work hardening it, and dulling the tool. The sliding and biting behaviour leaves a poor finish on the material.

http://upload.wikimedia.org/wikipedia/commons/thumb/4/41/Conventional_Milling_01.png/275px-Conventional_Milling_01.png

Climb milling (right):

Each tooth engages the material at a definite point, and the width of the cut starts at the maximum and decreases to zero. The chips are disposed behind the cutter, leading to easier swarf removal. The tooth does not rub on the material, and so tool life may be longer. However, climb milling can apply larger loads to the machine, and so is not recommended for older milling machines, or machines which are not in good condition. This type of milling is used predominantly on mills with a backlash eliminator.

http://upload.wikimedia.org/wikipedia/commons/thumb/8/83/Climb_Milling_01.png/300px-Climb_Milling_01.png

from:
http://en.wikipedia.org/wiki/Milling_cutter#Conventional_milling_versus_climb_m illing

at:
http://en.wikipedia.org/wiki/Milling_cutter

beanbag
05-23-2010, 09:59 PM
pntrbl,
Also if you face anything wider than your face mill you will wind up with a ridge you will have to fix with a file.

sounds like your mill is out of tram

tmc_31
05-23-2010, 10:10 PM
sounds like your mill is out of tram

Could be just a bit

pntrbl
05-23-2010, 11:20 PM
Thanx for all the replies guys. I thought a fly cutter had a drill bit in the center and a bit swinging around the outside. Shows how much I know!

I think I'll mosey on over to CDCO now ......

Thanx again.

SP

ptjw7uk
05-24-2010, 03:42 AM
In the diagram OldTiffe posted, I am a bit puzzled by the statement that in climb milling the 'cutcut starts at the maximum and decreases to zero'.
Surely as in the diagram the material will have moved approx half cut depth, and there will be no zero material cut!

Puzzled -- peter

oldtiffie
05-24-2010, 06:17 AM
Peter.

I have repeated the part of my post that you refer to here:


Conventional milling versus climb milling:

A milling cutter can cut in two directions, sometimes known as conventional or up and climb or down.

Conventional milling:
http://upload.wikimedia.org/wikipedia/commons/thumb/4/41/Conventional_Milling_01.png/275px-Conventional_Milling_01.png

The chip thickness starts at zero thickness, and increases up to the maximum. The cut is so light at the beginning that the tool does not cut, but slides across the surface of the material, until sufficient pressure is built up and the tooth suddenly bites and begins to cut. This deforms the material (at point A on the diagram, left), work hardening it, and dulling the tool. The sliding and biting behaviour leaves a poor finish on the material.
The description here is perhaps a bit over-simplified as the cutter seems to infer a straight tooth - ie no helix angle or "twist" - as on a router cutter. It also infers that the cutter engages the job along its full length - which it does not. The helix causes the cutter to first engage the job on the end of a clock-wise flute on a very small part of the job - almost like a sheet of paper in a stack - and as it further engages the job it increasingly shears the chip off at angle normal to the cutter helix. As the job advances into the cutter the depth of cut increases until the tooth reaches a maximum depth of cut as it reaches its exit point. All teeth follow successively. If the tooth is blunt it makes vary hard work for both the cutter and the mill. Same applies if the cutter edge misses the "pick-up" and has to rub the job to form a "bulge" that it can start cutting into.



Climb milling:
http://upload.wikimedia.org/wikipedia/commons/thumb/8/83/Climb_Milling_01.png/300px-Climb_Milling_01.png

Each tooth engages the material at a definite point, and the width of the cut starts at the maximum and decreases to zero. The chips are disposed behind the cutter, leading to easier swarf removal. The tooth does not rub on the material, and so tool life may be longer. However, climb milling can apply larger loads to the machine, and so is not recommended for older milling machines, or machines which are not in good condition. This type of milling is used predominantly on mills with a backlash eliminator.

In this case the cutter - still a spiral - engages the job at the maximum depth of cut and some have zero or very little "rub" and engages fully and cleanly. As the cutter rotates and the job is fed into the cutter the chip is still peeling but the depth of cut is reduced so that it is zero at the point of exit. The main problem with climb milling is that as the cutter passes the line of progression it moves from a "pushing" mode to a "pulling" mode and so pulls the job and table through the sum of any lead-screw back-lash and end-play. It can be quite violent - and potentially dangerous with regard to the operator, the machine, the holding medium and the job.

Climb milling tends to clear the swarf where-as the conventional milling is inclined to pull it (back) into cut and so fouling and interfering with the cutter starting and maintaining its cutting action.

Climb milling is more efficient as regards machine and cutter load and as regards unit material removal in unit time.

I normally mill "conventionally" for material bulk removal as my mills have "excessive" back-lash and end-play for climb-milling but I often take a light "spring cut" by climb-milling either at the previous depth of cut setting or with a slight additional depth of cut. This gives a better finish as well as relieving any "spring" in the cutter and/or the milling head due to conventional milling.

I hope this helps.

loose nut
05-24-2010, 10:05 AM
Wholesale Tool sell one that they advertise as "for smaller machines".

BobWarfield
05-24-2010, 11:22 AM
But I'd always prefer to finish with a fly-cutter - either a TC or HSS tool - HSS preferred.

I'll take a cheap flycutter over a cheap facemill any day--better finish.

I'll take a quality facemill over any flycutter any day--better finish and does it faster.

Quality doesn't have to cost the moon, but it likely won't be in the realm of cheap, at least as many people describe it. I like Glacern's cutters, for example. You need one with a modern insert geometry set up to do well with those inserts. You also need one that isn't too crazy big for your milling machine as they eat horsepower like candy.

I'm not sure I'd buy a facemill if I couldn't get a pretty nice one. I have 3, and the first one I got was barely better than a flycutter with a lot of fussing. The last two are excellent. One is a 90 degree taking APKT inserts, the other is a Glacern 45 degree.

BTW, if you still want a flycutter finish, go for it with the facemill. Just remove all but one insert and you're there. That might be the best yet.

Either the flycutter or the facemill will be sensitive to tram, and the bigger the diameter, the more sensitive. A ridge as mentioned is a clear indication of a tramming issue. However, a perfectly "flat" tram isn't necessarily going to give you the ultimate finish due to back cutting. These cutters can often produce a better looking finish if they're ever so slightly out of tram so that only the leading edge is cutting. We're talking 0.001" per foot or so on that.

For best finish, climb cut as OldT advises, but also don't take a full pass. Limit it to about 2/3's of the cutter's diameter. You want the forces on the cutter to settle out and predominate on one side. If you're doing a full pass, they will see saw back and forth a bit and the cutter wobbles.

The 45 degrees take less cutting force and leave a nicer finish, but you have to give up square shoulders with them.

Quite a bit more on milling surface finish here:

http://www.cnccookbook.com/MTMillSurfaceFinish.htm

Cheers,

BW

oldtiffie
05-24-2010, 10:27 PM
Bob,

I take your point.

If I am finishing I prefer to take a light cut - hence the HSS fly-cutter.

But my TC insert facing cutter does very well for heavier work - but I prefer not to use it on lighter cuts on anything that might work-harden.

https://www.machineryhouse.com.au/Products?stockCode=M516

It is a pretty good tool.

http://i200.photobucket.com/albums/aa294/oldtiffie/HF-45%20Mill%20misc/TC_end-cutter1.jpg

http://i200.photobucket.com/albums/aa294/oldtiffie/HF-45%20Mill%20misc/TC_End-cutter2.jpg

Here is a "used" vehicle brake hub that I faced with it. It went very well indeed - straight through the surface and I was running it at pretty well top speed on my HF-45 mill and winding my 90:1 rotary table as fast as I could go - I could not get it to its limit. I took some finer cuts as well and it came out as well as you suggested that it should.

I suspect that one insert may have been just a smidgen lower than the rest and acted as a "scraper tooth". The bottom face of the inserts are flat.

http://i200.photobucket.com/albums/aa294/oldtiffie/HF-45%20Mill%20misc/Brake-disc3-1.jpg

http://i200.photobucket.com/albums/aa294/oldtiffie/HF-45%20Mill%20misc/Brake-disc2-1.jpg

In this image the "rust" (I think) was the lanolin preservative I use - but the finish was as good as the others in the pics above.
http://i200.photobucket.com/albums/aa294/oldtiffie/HF-45%20Mill%20misc/Brake-disc1-1.jpg

I have thought seriously of leaving the inserts in the cutter and sharpening the bottom and side (45*) TC insert faces on my TC grinder so as to get an edge approaching that of a HSS cutter. I might do it later.

BobWarfield
05-24-2010, 10:56 PM
Tiffie, it'd be interesting to compare the performance of your face mill with all but one insert removed against your fly cutter.

I haven't yet tried the experiment directly as I'm pretty happy with the facemill's "diffraction grating" finish.

I will say that the fly cutter I picture on that web page from Widgitmaster gives pretty amazing results on aluminum.

Cheers,

BW

beanbag
05-25-2010, 01:52 AM
speaking of face milling, I recently helped somebody face a piece of steel on a bridgeport with my 45 deg face mill. I didn't have the ideal inserts, but only some medium roughing inserts (i.e. dull on purpose). Spindle battering was a real problem, and we were able to seemingly minimize it by using conventional milling and nearly full width cuts. I guess that stabilizes the cutter more, but is a little tougher on the inserts. (Ideally, you use 2/3 width pass and climb mill) The inserts managed to survive just fine, although the surface finish wasn't very good.

ptjw7uk
05-26-2010, 06:27 AM
Tiffie,
This thing is doing my head in, it just seems to be wrong, take the first picture - Conventional milling.
'The chip thickness starts at zero thickness, and increases up to the maximum.' Not right, as the second blade will at point A meet material that has advanced by the half the feed rate and the amount of material removed must be the same for both sides of the cut!
I realise they are trying to explain the difference in the way each method cuts but but to say the material cut starts at zero and increases to maximum just seems to be nonsense. Far easier to say that in climb milling the cutter will pull the work against all the slop in the system!

peter

beanbag
05-26-2010, 07:53 AM
conventional milling always has a chip that starts at zero thickness because the blade always enters the work at a glancing angle

BobWarfield
05-26-2010, 11:56 AM
Tiffie,
This thing is doing my head in, it just seems to be wrong, take the first picture - Conventional milling.
'The chip thickness starts at zero thickness, and increases up to the maximum.' Not right, as the second blade will at point A meet material that has advanced by the half the feed rate and the amount of material removed must be the same for both sides of the cut!
I realise they are trying to explain the difference in the way each method cuts but but to say the material cut starts at zero and increases to maximum just seems to be nonsense. Far easier to say that in climb milling the cutter will pull the work against all the slop in the system!

peter

Look at it slightly differently, Peter.

With conventional milling, the feed is pushing more material into the cutter since relatively speaking, the feed is increased because of the head-on collision. It isn't a lot, because the feed is much slower than the spindle rpm. Yet, it isn't inconsequential either, because the chips start out pretty thin.

With climb milling the feed is pulling the material away from the cutter, so the feed is slower. Instead of a head-on collision, we are rear ending the car ahead of us who is already moving, albeit slowly relative to us, LOL.

However you want to look at it, once we've gouged a chip up, it is easier to get it to let go, and creates less trauma, for a better surface finish, if it got a little thinner by the time we're ready for it to release.

This geometry of the interaction of rotating cutters versus objects moving in straight lines happens over and over:

- Climb vs Conventional Milling

- Chip thinning when cutting less than 1/2 the tool's diameter width of cut.

- Ballnose chip thinning

- Making an arc entry to a cut rather than straight lead-in for better finish (see my page for more: http://www.cnccookbook.com/MTMillSurfaceFinish.htm)

- The engagement of a cutter as it goes through an inside corner. Controlling this precisely is what modern high speed machining toolpaths do.

It is fascinating how all of this works, and more complex than you would think. For example, many CNC'ers are used to the idea that they should always climb mill, no matter what. Yet there is a point of engagement where climb milling will create a negative cutting geometry and it would've been better to use conventional milling for the cut.

Cheers,

BW

beanbag
05-27-2010, 04:44 AM
(see my page for more: http://www.cnccookbook.com/MTMillSurfaceFinish.htm)


excellent page with lots of useful info