Machining Alcoa mic 6

cmccull166 · Mar 23, 2018

What miserable material to machine this is 2018... WTH !!!.I remember what we called jig plate in the 90's it was crap material to machine but Blanchard ground somewhat flat until you ran a slot thru it..and not flat any longer.

Mic 6 same crap with a bigger price tag and a fancier brochure.
That being said, I started this plate today there is an oval spiraling inward toward the center of the plate 1 mm wide .047 deep
approximately 30 Feet worth...

Using Harvey tool feeds .016 deep at 90 sf (10,000 rpm machine)made 3 inches before it broke.
It's obvious it doesn't cut it just burns thru (seeing the burrs)until the tool fails.

Tool 2 .01 deep 5 ipr 14 inches.
SO...

I put a 45 degree included 2 flute endmill in .019 deep 9900 rpm 6 ipr pressed go and Left
..I dont expect this to have a happy ending!

I'm sure Monday I will be calling the customer 6061 T6 or this part wont happen.

If any body has a suggestion Im all ears.. :bowdown:

but the bottom line this material is crap and if I can save one person from banging their head on a bench ...i have been successful...

Finegrain · Mar 23, 2018

Which Harvey tool? One of the material-specific ones, or a "regular" endmill? Might try one of their Al-specific EM's if not already doing so.

IME MIC6 is gummier than 6061, but not night-and-day worse.

Good blast of coolant going right into the cut, not just in the general area?

Regards.

Mike

cmccull166 · Mar 23, 2018

Finegrain said:
Which Harvey tool? One of the material-specific ones, or a "regular" endmill? Might try one of their Al-specific EM's if not already doing so.

IME MIC6 is gummier than 6061, but not night-and-day worse.

Good blast of coolant going right into the cut, not just in the general area?

Regards.

Mike

Hello Mike
Material specific
24131-C8
I increased my coolant concentrate after tool 1
Thanks

CPM2014 · Mar 23, 2018

I agree with above. Easy as pie as long as you’ve got coolant and sharp tools

swarf_rat · Mar 24, 2018

If you are cutting at 5 ipr (inches per revolution) with a 1mm tool, the only surprise is that it took 3" to break.

litlerob1 · Mar 24, 2018

cmccull166 said:
If any body has a suggestion Im all ears..

swarf_rat said:
If you are cutting at 5 ipr (inches per revolution) with a 1mm tool, the only surprise is that it took 3" to break.

This isn't a great "suggestion" but I agree^^ with it

I "suggest" you run at least 50 IPM at .02 depth and 10,000 RPM. Assuming you are using Carbide 2 flute Endmill. It's all about chip load.

R

DMF_TomB · Mar 25, 2018

if you cant figure out how to machine aluminum thats your real problem

cmccull166 · Mar 25, 2018

litlerob1 said:
This isn't a great "suggestion" but I agree^^ with it

I "suggest" you run at least 50 IPM at .02 depth and 10,000 RPM. Assuming you are using Carbide 2 flute Endmill. It's all about chip load.

R

I went with the 45 degree 2 flute .018 deep it cut perfect didn't even create a burr.
next a Harvey 1 mm ball em .006 to a total depth of .047 ..5 ipm and yeah it took 15 hrs but it's done ...

I'm sure I can run a higher ipm but only had 2 ball mills and a delivery of Tuesday...

I have very limited experience with small tooling but 35 years and I am still learning...

And I still have 3 more to make due next month and would like to cut the time so ?

Also..

And my apologies to Alcoa the material is not terrible.... but my old coolant is..Valcool..I switched to Oemeta in my other machines ..great product! I was just burning my last pail of Val crap before I switched this machine over..and maybe the problem was the Valcool.as I ran Oemeta
after the mega fail .032 em ..

But litlerob1 50 IPM?... help.... :willy_nilly:

cmccull166 · Mar 25, 2018

swarf_rat said:
If you are cutting at 5 ipr (inches per revolution) with a 1mm tool, the only surprise is that it took 3" to break.

Oops.maybe that was the problem :dunce:

.

DavidScott · Mar 25, 2018

I was going to sugest it may be the coolant. Form tapping Mic6 is my way of testing a coolant to see how good it is with aluminum, good coolant makes a big difference with Mic6. With your first parameters .0007" chip load per tooth would be my starting point, and then I would see how much faster I could go. Mic6 is a bit gummy but with good coolant, good flushing, and good chip evacuation you can really feed fast. My only suggestion for next time would be a 3 flute mill. Get at least 3, 1 to find out how fast you can go before you break it, 1 to make the parts, and 1 for backup.

litlerob1 · Mar 25, 2018

cmccull166 said:
But litlerob1 50 IPM?... help....

Okay, a 1/32" is different than a 1mm (my assumption sorry). With a .0312" Endmill I would start at 1/3 the Tools diameter for the Depth (.01") and all the RPM you have (10,000) and maintain a chipload of .002" per flute, so that would be 40 IPM. BUT you will be able to go faster.

It's all about chip load when figuring out how hard to Feed the Tools, less about size.

So the cut parameters you had were 1/32" Endmill running Mic6 at 10,000 RPM and 5 IPM all = .00025" chipload. So you are fighting 2 things in that scenario 1. At that RPM you are getting the Aluminum warm, and because of the low feed (tiny chipload) it will just bond/meld to the Tool and make it impossible to cut. 2. 15 hours!!!!!

If anything, like if you are going to run 5 IPM and you don;t care what I say, at least turn the spindle down to 1250 so you get a real chip out of there, that is why Swarfrat said what he did about being surprised it lasted that long.

R

cmccull166 · Mar 25, 2018

litlerob1 said:
Okay, a 1/32" is different than a 1mm (my assumption sorry). With a .0312" Endmill I would start at 1/3 the Tools diameter for the Depth (.01") and all the RPM you have (10,000) and maintain a chipload of .002" per flute, so that would be 40 IPM. BUT you will be able to go faster.

It's all about chip load when figuring out how hard to Feed the Tools, less about size.

Thanks litlerob1
Since I have time on the next delivery I will sacrifice some tools and increase feeds...But 40 ipm?
I'll get back to you......

DavidScott · Mar 25, 2018

Get your coolant nozles focused right on the cut 2" away from the tool and 40 ipm may be conservative.

cmccull166 · Mar 25, 2018

DavidScott said:
Get your coolant nozles focused right on the cut 2" away from the tool and 40 ipm may be conservative.

Ok..I will give it a try..Thanks

Search

Largest Manufacturing Technology Community on the Web

Search

Machining Alcoa mic 6

cmccull166

Hot Rolled

Finegrain

Diamond

cmccull166

Hot Rolled

CPM2014

Cast Iron

swarf_rat

Titanium

litlerob1

Diamond

DMF_TomB

Diamond

cmccull166

Hot Rolled

cmccull166

Hot Rolled

Attachments

DavidScott

Diamond

litlerob1

Diamond

cmccull166

Hot Rolled

DavidScott

Diamond

cmccull166

Hot Rolled

Similar threads