Aluminium 6061/6082 on profiling surface finish

[usolutions]

I have a question regarding achievable surface finish in aluminium. I am currently running 3mm ball solid carbide endmill 2fl polished from haas shop, 0.075mm/fl, 0,075mm stepover, 15000rpm. Stock to leave from previous operation 0.25mm. I am getting quite smooth finish, but it is not, lets say bright or mirror-like. Am i missing somethin here? Part calls for R5mm internal fillets with sharp corners of R1.5mm.
Or getting smooth matte finish is to be expected? Or some kind of tool change/cutting mode is required for better finish. I dont have porfileometer at hand, can not give exact Ra value.

 

[Mtndew]

If you're just using it to finish profile, why not go for at least a 4 flute so you can feed it twice as fast?
Are you using coolant?
You probably won't get a bright mirror finish in 6061 so I wouldn't be too concerned as long as your finish meets the micor requirement.

 

[usolutions]

High pressure flood coolant, 10-12% concentration.
Haas does not have 4 flute aluminum. MSC/harvey are not serving our region. Guhring/kennametal are way too expensive for the job.

 

[Mtndew]

High pressure flood coolant, 10-12% concentration.
Haas does not have 4 flute aluminum. MSC/harvey are not serving our region. Guhring/kennametal are way too expensive for the job.

It doesn't need to be an aluminum specific end mill. Just uncoated, especially if you're just finishing.
Garr has them for the same price as you're paying for the Haas end mill but I don't think they ship to your country.
Oh well, it's the thought that counts lol.

 

[usolutions]

Being in Eastern Europe is next worst thing to be in Russia right now

 

[hi-fly-cnc]

Your step seems too high? I find that with a 12mm, my magic chipload for a mirror finish is about 0.08mm or less. H&V suggest about half of that...

So I might be expecting you to be under 0.03-0.04mm chipload for finishing...?

 

[usolutions]

Your step seems too high? I find that with a 12mm, my magic chipload for a mirror finish is about 0.08mm or less. H&V suggest about half of that...

So I might be expecting you to be under 0.03-0.04mm chipload for finishing..

Lowest i tried was 0.04, cycle time is dramatically increased, however surface finish did not improve, it feels it was worse, since chip does not form and surface gets smeared instead. Also such fines clog coolant filter like

 

[usolutions]

Your step seems too high? I find that with a 12mm, my magic chipload for a mirror finish is about 0.08mm or less. H&V suggest about half of that...

So I might be expecting you to be under 0.03-0.04mm chipload for finishing...?

tried 0.03mm chipload 0.03 stepover, still cloudy finish.I guess I can not get it with this material. oh well, does not matter.

 

[hi-fly-cnc]

The actual shininess of the result can be very hard to dial in. You will need to play with stock to leave and amount/concentration of coolant and surface speeds. You might need more RPMs to shear the material, or a sharper cutter, etc? I might think you want a slightly smaller stock to leave, you could try 0.12mm and below, perhaps around half that in fact.

Presumably you are just finishing some tight internal corners, so perhaps polish them with the dremel if that's all you need?

 

[jz79]

Lowest i tried was 0.04, cycle time is dramatically increased, however surface finish did not improve, it feels it was worse, since chip does not form and surface gets smeared instead. Also such fines clog coolant filter like

if you reduce chipload to such a low value and your finish gets worse, it could mean there is runout on the tip of the tool, explanation being that one of the flutes is still cutting, but the other one is just smearing due to offset induced by runout

2 micron indicator on the flutes or on the shaft as close to the tip as possible could tell what is going on, don't put it near the holder, need to measure at the tip

also - what kind of holder is used for this 3mm ball?

and 3mm ball might be cutting near the bottom where surface speed can be very low, there is a Hoffman group distributor, might try DLC coated ball endmill, might help with the smearing, but 60-70eur/pc... and presumably hours in cycle time, so perhaps better investment is, like suggested here - dremel and hand polishing while the other parts are running

p.s. there is also this - despite what the material certificate says, the aluminum we get sold here can be of very questionable quality

 

[usolutions]

The actual shininess of the result can be very hard to dial in. You will need to play with stock to leave and amount/concentration of coolant and surface speeds. You might need more RPMs to shear the material, or a sharper cutter, etc? I might think you want a slightly smaller stock to leave, you could try 0.12mm and below, perhaps around half that in fact.

Presumably you are just finishing some tight internal corners, so perhaps polish them with the dremel if that's all you need?

I dont have more RPMs, I have 15k spindle and using it to the max.
Corners look fine, however flat surfaces are garbage. 200x400mm flat hand polishing is out of the budget.

what kind of holder is used for this 3mm ball?

er 20 stubby collet. I'll check runout once again, but intially it was less that half dial tick.

if you reduce chipload to such a low value and your finish gets worse

I would not say it is worse per se, it is the same super fine lines, even finer, yet not even close to what i get from surface mill. From Ra standpoint it should be perfectly servicable, since material grain is significantly coarser than surface roughness. But it is dull on flat spots. I bet it would be a non-issue if ti was a 5axis mahcine to avoid tip cutting.

 

[empower]

I have a question regarding achievable surface finish in aluminium. I am currently running 3mm ball solid carbide endmill 2fl polished from haas shop, 0.075mm/fl, 0,075mm stepover, 15000rpm. Stock to leave from previous operation 0.25mm. I am getting quite smooth finish, but it is not, lets say bright or mirror-like. Am i missing somethin here? Part calls for R5mm internal fillets with sharp corners of R1.5mm.
Or getting smooth matte finish is to be expected? Or some kind of tool change/cutting mode is required for better finish. I dont have porfileometer at hand, can not give exact Ra value.

what toolpath strategy are you using? i just went through this myself, 'scallop' type toolpaths are pretty bad for finish because in some spots you'll be conventional cutting.
if you're looking for shiny finish, you HAVE to make sure the tool is ONLY climb milling.

 

[hi-fly-cnc]

I'm not clear why you are using a D3 tool to cut the majority of the D10 fillet?

 

[jz79]

I dont have more RPMs, I have 15k spindle and using it to the max.
Corners look fine, however flat surfaces are garbage. 200x400mm flat hand polishing is out of the budget.



er 20 stubby collet. I'll check runout once again, but intially it was less that half dial tick.


I would not say it is worse per se, it is the same super fine lines, even finer, yet not even close to what i get from surface mill. From Ra standpoint it should be perfectly servicable, since material grain is significantly coarser than surface roughness. But it is dull on flat spots. I bet it would be a non-issue if ti was a 5axis mahcine to avoid tip cutting.

I don't think ER20 is the right choice for a finishing tool, the precision for that size of tool just may not be there, you could "dial" it in by tapping the nut to zero out the runout though (if the stickout isn't excessive), that is - semi tighten, put 2um indicator on flutes and then tap with a piece of aluminum on the nut to zero the runout, then final tightening (and recheck after final tightening ofc), but still, for 3mm ball in an ER...
if I recall, high precision ER had 2um runout tolerance, but I don't recall at what distance from holder, I had one "high precision" ER25 collet, new one, for 10mm shaft with 0 runout near the collet, but needed 70mm stickout, and at 70mm it was 0.05mm, took another collet, and that one could be dialed in with the nut-tapping method

200x400mm with 3mm ball... machine time must be real cheap...

 

[usolutions]

what toolpath strategy are you using? i just went through this myself, 'scallop' type toolpaths are pretty bad for finish because in some spots you'll be conventional cutting.
if you're looking for shiny finish, you HAVE to make sure the tool is ONLY climb milling.

Only climb and only up, parallel currntly

 

[usolutions]

I'm not clear why you are using a D3 tool to cut the majority of the D10 fillet?

Because I have it on hand, proper tool ordered, doing preliminary testing.

 

[usolutions]

I don't think ER20 is the right choice for a finishing tool, the precision for that size of tool just may not be there, you could "dial" it in by tapping the nut to zero out the runout though (if the stickout isn't excessive), that is - semi tighten, put 2um indicator on flutes and then tap with a piece of aluminum on the nut to zero the runout, then final tightening (and recheck after final tightening ofc), but still, for 3mm ball in an ER...
if I recall, high precision ER had 2um runout tolerance, but I don't recall at what distance from holder, I had one "high precision" ER25 collet, new one, for 10mm shaft with 0 runout near the collet, but needed 70mm stickout, and at 70mm it was 0.05mm, took another collet, and that one could be dialed in with the nut-tapping method

200x400mm with 3mm ball... machine time must be real cheap...

I am doing it with 8mm, and finishing corners with 3mm. However I have small piece of same material, same geometry, but just 80x80mm. Just for testing. Have not done anything like this before. doing tests before I scrap big plate of alu

 

[empower]

Only climb and only up, parallel currntly

can you post pictures of this finish?

 

[usolutions]

lighting is a bit tricky


As you can see nothing is shiny, like bright shiny

 

[empower]

thats very weird, if its actually only climb milling as you say, it should be shiny. unless you have really bad quality material