Reaming Aluminum

[Namliek_J@TheeCircle™]

I have to ream a 22mm hole in a piece of 6061 Aluminum using a HSS cutter. What kinds of RPMs and Feed Rates should I be running? Never really did alot of reaming on CNC machine.

[Namliek_J@TheeCircle™]

Drill size for the ream is 27/32

[Jedi Mastercam X]

Have u Drilled the hole already? theory goes, well at least from what i learned, u want a reamer to follow a hole. so, double the feed rate of what u ran ur drill and divide the RPMs of what u ran that drill in half. works great for me. hope this helps.

 

-R.

[Slixmix]

I would run it at 150 rpm at 2.0 IPM. Pretty conservative. I know everyone has there own preference.

[Namliek_J@TheeCircle™]

thanks guys.

[JASON JACQUES]

We run at 150-300 rpm at 3 IPM

[horsepowered]

I would run 200 RPM at 10 - 12 IPM feed rate if you have a good solid machine. And lots of coolant.

[Tom Szelag]

I'd second horsepowered and a bit more aggressive feed. It's gotta bite.

 

Usually half the speed, twice the feed of the drill works pretty well.

[DavidB]

On the same topic REAMING does any one have a formula for stock to leave for reaming or a rule of thunb?

[Guest]

Under 1n 1/8" or so I'll leave .001 - .0025 per side

1/8" to 1/2" .004 to .006

over a 1/2" .008 to .012

 

Of course depth and hole bottom condition will have an determining effect on how much stock as well

[DavidB]

John whats that mean in Metric

[Guest]

3.175mm about .0254mm to .0635mm

3.175mm to 12.7mm .101mm to .152mm

 

over 12.7mm .2032mm to .3048mm

 

[Charlie Pierson]

Floating holder or solid ????

Opinions please !

 

cp

[CNCme]

Good evenin',

 

I would make sure to indicate the reamer if your not using a floating holder

 

Tony G

CNCme Engineering LLC

X Beta Site

SO Almost Employed Senior Programmer

N.E Massachusetts - Southern New Hampshire

_________________________________________

End mills and tooling are like The "AMMO"

And coolant and chips are like the enemy

Under your boots as you advance in the

Manufacturing Battle

-------------------------------------------------

[DavidB]

If you want an accurately positioned reamed hole I would drill, circular interpulate then ream. A reamer will only follow the hole its going into.

[Brad MacKinnon]

Ive done some production runs in this before (1 1/16" hole 1 3/8" deep.Drilled and Interpolated to leave .004" radial ,S175 F9.0 IPM ) and I found that the holes were more accurate when I used the feed in spindle stop rapid out cycle. Also it didnt drag the chips as much and scar the finish.

[DavidB]

If the machine is good enough like my Makino I wouldn't even ream just cut it.

[88Matt]

I agree with David, I avoid using reamers if possible. Only if the hole is to small and deep to helix bore do I use a reamer.

 

Matt

[CNCme]

Good Day,

 

+1

Many of the new design parts, I circlemill all reamer type holes.

Reaming is old world, but there are still people doing it for special applications. Or non-CNC machining parts.

 

Tony G

CNCme Engineering LLC

X Beta Site

SO Almost Employed Senior Programmer

N.E Massachusetts - Southern New Hampshire

_________________________________________

End mills and tooling are like The "AMMO"

And coolant and chips are like the enemy

Under your boots as you advance in the

Manufacturing Battle

-------------------------------------------------

[Andy]

We frequently short chuck the reamers so they will easily flex and follow the hole. Another trick is to circmill the start of the hole then ream so reamer is guided... at least for deep reams that you cant circmill finish.

[dprovost71]

Whats your depth of cut? This can play a part in the speed and feed also. For that size hole I would probably use a good boring head depending on depth...whats the tolerance on the hole?

[mcpgmr]

I've had good results in all grades of Aluminum using 100 sfm and .003 chip load using HSS reamers. So about 450 rpm at 8.1 ipm using a 6 flute reamer.

HTH !

[Psychomill]

I'm near MCPGMR here... I'm at 530 rpm and 10 ipm.