[JWB_Machining]

Hey,

I'm trying to face a Piece of Aluminum about an inch thick and around 6" x 6". I need to get a beautiful finish on this thing but what I'm getting you can see in the pictures below. I'm Running a 2" Indexable Carbide Shell mill and using flood coolant. i'm Running at 4000 RPM and 32 ipm. I'm sure there's an easy fix for this but i can't wrap my head around it for some reason.

[PinMan]

Is it 6061? I have a similiar tool that I use to face 6061, 2.5" 8 insert face mill.
Here are the S&F's that I use to obtain a 5.1U" finish:

1200 SFPM
.003 IPR

These work exceptionally well on 6061, hope this can help you out some.

[Geof]

Very likely you are using standard inserts not the highly polished positive rake micrograin inserts made for aluminum. Iscar has these inserts for some of their turning tools but I do not know about face mills.

Because the size is modest go to an endmill and for best appearance use one with a small corner radius.

[tstom]

What inserts? We face a lot of aluminum and we use a Sumitomo insert in a
4 " face mill that leaves a near polished finish The insert number is SEET13TAFGN-L I believe they are radiused and polished usually run around 3500rpm and 35-40 ipm with a 4" cutter 5 inserts

[JWB_Machining]

I do not know the material, just that it is forged Aluminium, my boss is out for the week so I can't get a hold of the drawing with the spec till monday.

I'm using SECO XOMX120408TR M12 T350M. I have a few over inserts here all XOMX120408TR with slightly different geometries and grades but the SECO catalog doesn't clarify all to well what grades and geometries are intended for what purpose so I emailed them earlier and am waiting for a response. I didn't work here when these inserts were purchased but I believe they're intended for Square Shoulder and Slot milling, not facing but sometimes you gotta use what you got. I'm assuming I may have to try different inserts but Geof are you recommending I just use a solid carbide endmill instead because that's entirely doable it's just my boss bought up so much stuff before I was hired that I try and take full advantage of all the toys he's bought me.

It seems like cutter starts to squeell as it gets to the end of it's pass and this is where the finish gets to be the worst, also I can feel a slight ridge at the edge of each pass. Could I have a support issue? I'm only use step jaws and it is 6 inches unsupported, I was thinking of tapping in some wood wedges underneath the part but don't wanna lift it out of the jaws.

Could My depth of cut also not be deep enough?

[Geof]

I had not looked closely at the picture. Yes with a big insert cutter and a piece of mateial relatively thin compared to its width you can get chatter.

Do you have any largish end mills? 5/8" or larger? Just cut your losses and whip up a quick facing program.

Don't waste time, this should do it; run it in Graphics first.

O00000 (FACING)
(Place G54 just clear of workpiece ar right back corner)
(Set tool offset to where you want the final surface to be)
(Program written for 5/8" cutter)
N1 G90 G40 G49 G20 G80
N2 G53 G00 Z0.
N2 (---)
N28 T01 M06
N29 G43 H01
N30 M03 S6000
N31 G54 G00 X0. Y0. Z1. M08 (MOVE TO START POSITION)
N32 Z0.0
N32 G91 G01 Y-0.6 F30. M97 P1000 L5
N32 G90 G00 Z1.
N77 G53 G49 G00 Z0.
N78 G53 G00 X-10. Y0. M30
N79 (---)
N1000 G90 X-7.0
N1001 G91 Y-0.6
N1002 G90 X0.
N1003 M99
N1004 (----)

[JWB_Machining]

Yeah i used the Facing program in IPS because that's pretty darn easy. As for my Endmill selection I have solid carbide up to 1/2 inch and then i have an indexable 1" endmill and I've got 3/4" and 5/8" roughing end mills.

And so if I have thin workpeices compared to their length the smallet cutters are better?

[HuFlungDung]

If you have a ridge between parallel passes, you might need to tweak out the levelling of the machine, if you are lucky, you might be able to fix this by tramming the spindle. Worst case, you might have to shim the spindle cartridge if you cannot get the spindle perpendicular to the table by levelling.

[JWB_Machining]

You Know I Just ran a 1/2" roughing end mill and the finish is good but I do have those ridges. Now my Machine is a Haas TM-1 and I know that even if My Vise is put in unlevel or my work piece that if the entire surface is faced it should be smooth, I wqas getting ridges on the old manual bridgeport so I just tilted the spindle a half of a degree to fix it but how can I go about this on my Haas? Should I post in the Haas Mill Forum? i'm only 22 and only so much experience, I'd love to fix the machine myself because whenever I do fix the machines around here my Boss praises me but i'm a lil apprehensive to dive into fixing a CNC machine that's relatively new. Any info on this "Tramming the Spindle" you speak of? How likely am I to make the machine worse then it was before I touched it?

Any Chance Haas can send a guy out to fix this for free because the machine is so new it shouldn't have this problem so I'm trying to think of any other reasons for the ridge but the tool is new, my spindle is clean and so is my tool holder. Now that I think about it this TM-1 and the probes we got with it have given more trouble then I thought they would, granted I might just be a poor operator.

[JDenyer232]

We do this type of facing all the time. We use a 2" diameter single point flycutter at 3000rpm and 10ipm, .010" depth of cut, flood coolant is on. This is on a finish pass where I want a mirror like finish. I can actually see my reflection quite clearly on the surface when using this method. Are those steel jaws? I would make myself a set of aluminum softjaws, the aluminum softjaws deform enough to hold the piece rigid if you have any variances on the gripping surface due to irregularities in the workpiece, in fact we only use aluminum softjaws around here, they are cheap and easy to make as well as great at holding parts fairly rigid. We often face 6"X6" plates at .500" thick with a very nice looking finish. I noticed that on you parts the marks are more pronounced away from the center, most likely from lack of rigidity and endmill selection. Hope this helps.

[JWB_Machining]

JDenyer,

Thanks for the recommendation, i'm out tomorrow but i'll give that a try first thing Friday n see how that goes. Mirror-like finish is what I'm going for.

[DareBee]

Seco makes an Octomill face cutter and has superb positive geometry with no possibility of dragging (for chatter).
Low horsepower or weak setups typically don't phase it.
Highly recomended.

[dertsap]

take a couple machine bolts that will just slide under the part and add nuts to them and use them as jack stands for the center edges , put a dial on the center of the part so you can be sure your not bowing the part as you jack , this will probably give you the rigidity that you need , sometimes a wad of packing foam will do the trick

[HuFlungDung]

RE: tramming the spindle to the table: mount a sensitive dial indicator in a holder in the spindle. You want this indicator to sweep through a circle almost as large as the table is wide. You sweep slowly and try to observe any trend for the needle to move up and down in a regular pattern (repeatable each sweep revolution).

If you notice a 'low corner' you can try adjusting the levelling screw closest to the low spot. If you make it worse, adjust the screw the opposite rotation If you think this works, be sure to go around and test all the levelling screws to make sure they all bear some of the machine's weight.

If you still get ridges on parallel passes, I would suggest that you get a Haas technician to come in and see what can be done. I shimmed my VF3 spindle cartridge a little bit because I could not bring the table into tram now matter how I adjusted the levelling screws. I did this by loosening off the big bolts that hold the cartridge into the head housing. You only need to loosen them a little bit, enough so that you can slide some shimstock between the flange and the head casting. It does not take a lot of thickness of shim, remember that the effect on the flange at an 8" diameter is going to be exaggerated if your sweep arm is longer and sweeping a larger diameter circle.

I like to ensure that I shim and get 3 point support of the spindle flange. That means at minimum, 2 shims about 120° apart while 120° from there, the flange bears directly on the head casting. If you only use a single shim, then the spindle cartridge cannot be stable and you may bend the flange over top the single shim when you tighten the bolts and this may transfer into an out of round condition of the spindle housing and cause bearing heat problems.

[JDenyer232]

Seco makes an Octomill face cutter and has superb positive geometry with no possibility of dragging (for chatter).
Low horsepower or weak setups typically don't phase it.
Highly recomended.

We use the Octomill for roughing passes and it leaves a decent finish even when used on it's own, we usually follow up with a single point flycutter for thin parts that require a mirror like finish.