Can't get acceptable finish in 6061

ranchak · Feb 8, 2019

I've been battling a finish program for quite awhile now. I make some parts out of 3/8" x 2 3/4" bar stock. The back side and front side need to be faced in a single pass (no stepover). I'm using a 3" face mill that uses SEHT inserts. In the past i have had good luck with Korloy inserts that are aluminum specific. I bought a bunch on eBay and found out that they where counterfeit inserts. I ordered new inserts from a known reputable source. Still bad finish. played with feeds, speeds, D.O.C. still no good. Tried two different Tungaloy facemills, two facemills from MariTool, a facemill from Exkenna and still no luck. I have two Hass VF3s, a 2010 inline and a 2004 gearbox, both machine have 10K spindles, machines are in good condition. The coolant concentration in between 8 and 10%. I'm starting to think this is a material issue, I have been getting aluminum that is American made, comes from Service Centers (?). I have also tried some Kaiser aluminum that I have here, still can't get a good acceptable finish. Is anyone else having finishing issues? I thought that I have been thorough on trying to figure out this problem, but it's about time to ask the big boys for help.

Finegrain · Feb 8, 2019

ranchak said:
I'm starting to think this is a material issue, I have been getting aluminum that is American made, comes from Service Centers (?).

Don't know that this is the only cause, but I have had lots of issues with Service Center 6061. Accelerated tool wear (chipping), form taps that don't make proper threads, etc.

Regards.

Mike

Generic Default · Feb 8, 2019

What is the finish pattern on the faces? Is it a striped banded repeating pattern, or are the areas near the sides of the part showing a different finish than the center of the facemill path?

If you need the best possible surface finish in aluminum, you need to get a diamond insert in your facemill. One of the DLC coated inserts is second best, if you already have a Maritool facemill you can buy DLC coated inserts like this:
Milling Insert APET160508PDFRSN-DLC100 MariTool

Finegrain · Feb 8, 2019

What sort of "not OK" finish are you getting? Pics?

Have you indicated all of the inserts in your facemill? One insert sitting high will wear quickly, and end up cutting like s**t.

Have you tried facing the other way? A slight tram error will cause issues going one way but not the other.

Regards.

Mike

SND · Feb 8, 2019

Yeah, need pictures of that the finish issue is.

Try with just 1 insert like a fly cutter maybe.

ranchak · Feb 8, 2019

I've tried using all six inserts, three inserts, one insert. Still looks like shit. I've re-leveled the machines. I've tried facing in both directions. Generic Default, "What is the finish pattern on the faces? Is it a striped banded repeating pattern, or are the areas near the sides of the part showing a different finish than the center of the facemill path?" I have noticed that I will get a pattern where the edges do change direction, typically this is on the edge that the face mill enters the part.

EmGo · Feb 8, 2019

If it's *just* this material then this doesn't apply, but if it's everything, can be spindle bearings.

Otherwise, are you getting built-up edge on the inserts ? Tried a different coolant, like kerosene or wd-40 or westlube ? Tried an hss flycutter just for kicks ? Even on soft forging material you can get a reasonable finish if you absolutely have to. Which is why I would be nervous about spindle bearings ...

chip_maker · Feb 8, 2019

I'll bet my lunch money it's crap material.

ranchak · Feb 8, 2019

So if you guys have parts that need a machined finish, what brand of material are you using? Another supplier has Hydro, never used it. I can't believe two machines are giving a bad finish, my bet is crap material as well, but I can't believe I'm the only one with this problem.

allloutmx · Feb 8, 2019

The finish doesnt look terrible- but here are a couple things I see.

it looks like the edge of your facemill is almost exactly tangent to the back of your material. Shift your tool path Y positive .05" and see what that does for you.

Maybe I missed it but what are you taking for a finish pass?

Why are you clamping on the far left of the vice instead of in the center? May sound trivial but it does matter. the moveable jaw pivots from center.

Did you prep the stock? I almost always take a skim cut on all 5 faces especially on a relatively thin/wide ratio part like this. Taking the skin off will help you with the stress and will ensure you are getting a firm bite on op1. Getting a firm bite will help you with your finish.

The fine lines in your surface finish look to me like you may be feeding too fast or you have a very small radius on your facemill. Whats your feedrate and what size rad is on the insert?

The pattern you mentioned in your last post is likely due to accel/decel of the cutter as it enters and exits the material. could be material flexing under the cut as well especially if you are not clamped up on a prepped/uniform surface.

ranchak · Feb 8, 2019

allloutmx said:
The finish doesnt look terrible- but here are a couple things I see.

it looks like the edge of your facemill is almost exactly tangent to the back of your material. Shift your tool path Y positive .05" and see what that does for you.

Maybe I missed it but what are you taking for a finish pass?

Why are you clamping on the far left of the vice instead of in the center? May sound trivial but it does matter. the moveable jaw pivots from center.

Did you prep the stock? I almost always take a skim cut on all 5 faces especially on a relatively thin/wide ratio part like this. Taking the skin off will help you with the stress and will ensure you are getting a firm bite on op1. Getting a firm bite will help you with your finish.

The fine lines in your surface finish look to me like you may be feeding too fast or you have a very small radius on your facemill. Whats your feedrate and what size rad is on the insert?

The pattern you mentioned in your last post is likely due to accel/decel of the cutter as it enters and exits the material. could be material flexing under the cut as well especially if you are not clamped up on a prepped/uniform surface.

I'm taking a 0.020" finishing pass, thicker doesn't seem to make a difference. I am on centerline, I have tried shifting by 0.100", same results, but I can try your suggestion of 0.050".

I'm using aluminum specific inserts Korloy SEHT1204AFFN-X83 H01

These parts are clamped two at a time in Mitee Bitee Talon Grips

I've tried feedrates from 10 ipm to 120 ipm. This photo is 20 ipm, 3000 rpm

These parts definitely look worse in person than the picture shows.

Finegrain · Feb 8, 2019

I'm going to go with bad material as well, and maybe cutting some of the Service Center material compromised the fragile edges of the Korloy inserts. I run those same Korloy inserts, and get pretty nice finishes in Kaiser, Sapa and Hydro. 10,000 RPM, 180 IPM. I usually try for a .01" or even .005" finish pass, and get there with a roughing endmill instead of the facemill. Those Korloy inserts are great, but fragile and do not hold up long if taking 1/8" depth cuts.

Regards.

Mike

allloutmx · Feb 8, 2019

ranchak said:
I'm taking a 0.020" finishing pass, thicker doesn't seem to make a difference. I am on centerline, I have tried shifting by 0.100", same results, but I can try your suggestion of 0.050".

I'm using aluminum specific inserts Korloy SEHT1204AFFN-X83 H01

These parts are clamped two at a time in Mitee Bitee Talon Grips

I've tried feedrates from 10 ipm to 120 ipm. This photo is 20 ipm, 3000 rpm

These parts definitely look worse in person than the picture shows.

I would suggest .003-.005 for finish.

if you are on center then disreguard the .05 move.

is the spindle tram?

are the inserts all seated and at the same height?

have your spun it a 6k yet?

wheelieking71 · Feb 8, 2019

Hydro = Sappa

3000rpm seems slow.
Try aiming your coolant in a way that it keeps the top surface of the part wet. But, doesn't blow the chips back under the tool.
I had an issue similar to that in a HAAS with P-cool years ago.
Finally figured out that I had the P-cool aimed directly at cut height, and it was blowing the chips right back under the tool.
Moved the P-cool up so it was blasting the shank of the tool, which let the chips fly away, and problem solved.
Your issue looks to be on the leading edge though, so that may not help?

Otherwise, I agree with the notion to spin it up.
I generally face at 12k and 120ipm with a tool not known for great finishes, and get good results.

ranchak · Feb 8, 2019

Finegrain said:
I'm going to go with bad material as well, and maybe cutting some of the Service Center material compromised the fragile edges of the Korloy inserts. I run those same Korloy inserts, and get pretty nice finishes in Kaiser, Sapa and Hydro. 10,000 RPM, 180 IPM. I usually try for a .01" or even .005" finish pass, and get there with a roughing endmill instead of the facemill. Those Korloy inserts are great, but fragile and do not hold up long if taking 1/8" depth cuts.

Regards.

Mike

I use a different face mill for roughing, the Korloy inserts are only used for finishing. I'll try the 10,000 RPM and 180 ipm, 0.01 DOC. This material in the picture is Kaiser material.

ranchak · Feb 8, 2019

allloutmx said:
I would suggest .003-.005 for finish.

if you are on center then disreguard the .05 move.

is the spindle tram?

are the inserts all seated and at the same height?

have your spun it a 6k yet?

Only One insert.

I used to feed at 6000 rpm and 30 ipm, I noticed my finish wasn't as good and I dropped to 4000 rpm and 20 ipm

allloutmx · Feb 8, 2019

ranchak said:
Only One insert.

I used to feed at 6000 rpm and 30 ipm, I noticed my finish wasn't as good and I dropped to 4000 rpm and 20 ipm

one insert makes it act more like a fly cutter. you will have to go really slow to get a good surface finish with one insert. like 5-10ipm

DethloffMfg · Feb 8, 2019

I have a Maritool 2.5" 45-degree face mill running those Korloy inserts. I really, really dislike it. I have .0035" variation between cutters and I have to run it at 4000 rpm with flood at around 35ipm to get a finish that is better than that but still has visible lines like that and doesn't come close to the finish of a quality face mill, in Hydro 6061 with new Qualichem 250c at 8% at full blast. I genuinely dislike the facemill. I get better finishes from YG Alu-Power end mills. It is not at all a terrible face mill, and it's very affordable, but I want near-mirror finishes.

P.S. Maritool doesn't post their max RPM on those face mills so I don't go over 4k. It was made very clear when setting up the machine to watch face mill max RPM's, if the tool is made for a max of 5k and you turn it up to 10k you might have a very bad day.

precisionmetal · Feb 8, 2019

I might go with "chip_maker" on this. The finish almost looks a bit "Mic-6-ish".

Heck... I can hand-jog my face mill at .020" deep cut across flat bar and get a better finish than that.

You'll find it... something vibrating, rotten material, face mill loose on the adapter? Something else?

PM

CarbideBob · Feb 8, 2019

I agree the finish looks like shit.
Picture shows that you are not on centerline. Look at the imaginary tangent lines to the arc cuts top and bottom.
They should be the same. Entrance and exit should match.
If your math works out to on center something is way screwy.

In fact you are at a very bad location, the opposite would be better.
You are chip welding. Why can be many reasons but that shallow entrance is not helping things.
There is more here than a c/l problem but why is the basic stuff off?
Bob

Can't get acceptable finish in 6061

Cast Iron

Diamond

Aluminum

Diamond

Diamond

Cast Iron

Diamond

Stainless

Cast Iron

Titanium

Cast Iron

Diamond

Titanium

Diamond

Cast Iron

Cast Iron

Titanium

Cast Iron

Stainless

Diamond

Similar threads