What's new
What's new

looking to speed up this frame pocket.

troy fab

Aluminum
Joined
Dec 17, 2008
Location
Greene RI
Just making a .343 pocket .900 deep. If I go faster or take bigger cuts I snap bits.

Material is 6160 aluminum. Using a 3 flute .250 x 1 1/4" long endmill. ( no coatings). 1400 rpm
Bridgeport has a Anilam 3300 mk retrofit.
Start height .100
Island length 1.5
Island width 1.5
Z depth .900 ccw
Inside radius .750
Outside radius 1.093
Frame width .343
Step over .080
Depth cut .100
Fin stock .013
Ramp feed 2.0
Rough feed 4.5
Finish feed 5.0
speedospacerhub001-1.jpg
 
maybe a coolant mister and carbide that will get your RPM up with out melting the stock.
say, 500 SFM is 8k.

even at 200SFM your @3200 RPM. Crank that hog up.

Or drill the hole out, and final ream or bore..
 
I have found that snapping endmills in aluminium is 99% caused from chips clogging up and eventually welding to them. Every time it has happened do yourself a favor and try to get it off the bit and it is most probably still really sharp on the flutes.

As others have suggested pretty much your max RPM that you want to run is where you want to be. Having said that you need to make sure that you are blasting those chips away from the endmill as soon as it is cutting them. Ramping and plunging obviously make it a bit tougher but you should be fine with the ramp as long as you are ejecting all the chips. If you are helical ramping maybe try to ramp by following the boundary so that there is more space to get those nasty chips out. If you are not already using an aluminium specific endmill, but by your description you might be, invest in some! You will be amazed what those suckers can do, even the really cheap ones.

Loads of customers have said to me "yeah it's aluminium its waaay easier to machine than normal steel" :toetap: But in reality any material that needs to get hogged out has it's own sweet spot that is not always that easy to hit. I have recently finished an aluminium mould that I majorly under quoted on because I thought that I had hit the sweet spot up until I went 2xD in the pockets. The small little 5mm endmills,which had to be used to get through the ribs, tried their best but the coolant just could not get to where it needed to be. I resorted to hogging out the first 2/3rds of it at deep cuts and then babying the last few depths. That could also help you out a bit with your situation.
 
maybe a coolant mister and carbide that will get your RPM up with out melting the stock.
say, 500 SFM is 8k.

even at 200SFM your @3200 RPM. Crank that hog up.

Or drill the hole out, and final ream or bore..

Its not the hole, it is the groove around the hole.
 
I have found that snapping endmills in aluminium is 99% caused from chips clogging up and eventually welding to them. Every time it has happened do yourself a favor and try to get it off the bit and it is most probably still really sharp on the flutes.

As others have suggested pretty much your max RPM that you want to run is where you want to be. Having said that you need to make sure that you are blasting those chips away from the endmill as soon as it is cutting them. Ramping and plunging obviously make it a bit tougher but you should be fine with the ramp as long as you are ejecting all the chips. If you are helical ramping maybe try to ramp by following the boundary so that there is more space to get those nasty chips out. If you are not already using an aluminium specific endmill, but by your description you might be, invest in some! You will be amazed what those suckers can do, even the really cheap ones.

Loads of customers have said to me "yeah it's aluminium its waaay easier to machine than normal steel" :toetap: But in reality any material that needs to get hogged out has it's own sweet spot that is not always that easy to hit. I have recently finished an aluminium mould that I majorly under quoted on because I thought that I had hit the sweet spot up until I went 2xD in the pockets. The small little 5mm endmills,which had to be used to get through the ribs, tried their best but the coolant just could not get to where it needed to be. I resorted to hogging out the first 2/3rds of it at deep cuts and then babying the last few depths. That could also help you out a bit with your situation.
Thanks, I will fire up a couple test pieces and see what happens. (Right after I buy a spare endmill.)
 
Wow. You are wasting a lot of time and/or money on that part. A face grooving tool on a lathe would have that done in 1/5th of the time it takes you to mill it.

Or less.
 
Material is 6160 aluminum. Using a 3 flute .250 x 1 1/4" long endmill. ( no coatings). 1400 rpm
Bridgeport has a Anilam 3300 mk retrofit.

Max it out ..hmm.. I will try that. Not sure what max is, I have never been above 1500. I do know it goes higher.
Is this a joke? :confused:
 
Wow. You are wasting a lot of time and/or money on that part. A face grooving tool on a lathe would have that done in 1/5th of the time it takes you to mill it.

Or less.

I made a tool to do this in my lathe and it works fine. I only have one lathe so while I use the lathe for jobs that make more money I have the CNC run these at the same time. I can also have my wife run these and all she has to do is feed the part and push a button. She is not a machinist.
 
The endmill that you're using.. .is it just a standard 3 flute?
If so, you need to get something like a Blizzard from OSG where the helix is faster to make the chips come out of the hole.
You either want a ZrN coating or a bright polish finish.
And you need to (if you can) go 15k rpm or higher, if you can't go that high, run at max rpm.
You could also use a .312 drill and drill a bunch of holes around the center of the groove to remove a bulk of the material, then you could possibly feed the endmill faster.
 
I did a huge thread on this recently.

USE A 2 FLUTE on any diameter under 10mm.
Buy Carbide!
Spin it as fast as you can!
Cut fast.
Trochoidal machining is your friend.
Fast and deep... yeah :D
+1 misting, I didn't really get to read through everyones posts, loads of air with a mist is great.
 
Last edited:
What post 4 said. If no mister available get some air on it for chip removal. You are friction welding the chips to each other. That is what is breaking the tool.
i_r_
 
high helix end mill

buy a high helix end mill made for alluminum.
you dont have to buy expensive carbide if your rpms cant go above 4,000.
you can buy cheap hss end mills from latheinserts.com at about 16.00 for a 1/2" 2 flute run them at 3500 rpm and
20 ipm. depth of cut can be .25" if you have a fairly ridged set-up if machine cant handle that the maybe .125 depth. make sure you got plenty of cool mist or coolant hitting the tool.
 
Thanks for all the input guys, I will be messing around with high rpm speeds to see how it reacts. My machine goes up to 3000 rpm,s. Chips are not a problem I blow a high pressure mist in there. I have some 2 flute bits on the way.
Once again thanks for helping out a rookie.
Steve
 








 
Back
Top