Roughing Help

[mike silvia]

Hey Guys
I have a bunch of aluminum motorcycle trees I need to make on my Bridgeport. I have a Acurite 3500i control on it and I'm trying to rough in out in a timely matter. I'm looking for ides that will help me decrease the time it takes for roughing without knocking my mill head all out of wack.
Thanks for any input
Mike

 

[carlquib]

Use a roughing end mill, they move more metal with less cutting pressure. I don't know if the fine or course cut is best for aluminum, I'll let someone else chime in on that.

Hello, my name is Brian and I'm a toolaholic

 

[Christian Poulsen]

....Well, you know your machine so when ruffing all I can say is: Plan your layout/set up and order of ops. to be the most efficient...Bigger cuts, faster speeds (speeds and feeds) that won't knock your head out and bounce your table around...and "regular" HSS or Carbide endmills will do for the profile work but the HSS endmills made for aluminum (they have a real fast "helical" (spiral) and more aggressive angles)...I have a couple of 3/4, 1/2 and 3/8 each)...And ifn' your plate isn't to size, play with your flycutter angles to take the most stock (steeper cutting angles too)...
...I've made a few sets of trees including converting a Honda Gold Wing front end to my HD FXWG (I came out the door one morning and my scoot had been stripped including the front end!...all during sometime in the night, all right under my bdrm window!

....oops and what Ulma Doctor said below...Operation 1= band saw! (Actually when I made my "trees" the roughing was mostly done from the band saw and drill press by the time I got to the mill

 

[Ulma Doctor]

if any of the parts can be saw cut, that would save lots of time
like Brian said, a roughing end mill is more efficient in stock removal.
use wd40 or kerosene to keep the aluminum from sticking to the tooling

 

[TakeDeadAim]

Id give Lakeshore Carbide a call, I got a couple small roughing cutters from them, for steel. Not sure if they have anything specific for aluminum but they work off chip load per tooth when they recommend and that formula, vs; the standard CSx4/dia seems to be more accurate when trying to get everything you can out of a cutter/machine combo

 

[Bill Gruby]

While I somewhat agree the HSS and carbide cutters will work, the Roughing End mill has no equal when it comes to hogging material. It's nick name is "Hog Mill" for good reason -- Max material with less strain on the cutter. Just my opinion.

"Billy G"

 

[Christian Poulsen]

...here's a Milling formula I worked out decades ago ago I dug up (I machine most everything on everything by sight and sound) as a starting point from those plastic slide calculators the vendors give out, my old version Machinists Handbook, and experience (Keeping in mind the following is for a Bridgeport or similar knee mill using up to the full diameter of a cutter. no climb milling. with the quill up and locked, table (y) locked with x snugged and an x power feed with inches per minute graduations:

.050 to .100 depth of cut

Spindle RPM= SFM (Surface Feet Per Minute) x 12...divided by the diameter of cutter x Pi

IPM (Feed Inches Per Minute) = Feed per tooth (tooth load of .003 for "hard", .005 for "soft") x the # of teeth...x RPM

SFM: (with Carbide cutters)
"Ledloy" and aluminum: 350-450
CRS: 250-350
Unhardened toolsteel (such as D2): 150-200
Prehard (up to around rc20 such as Maxell): 100-150
Prehard (up to around rc30 such as Maxell 3 1/2): 100

SFM: (with a HSS cutters)
Ledloy and Aluminum: 125
CRS: 100
Unhardened tool steel: 50
Prehard (up to around rc 20): 50

Example: (Using a 3/4 dia., 3 flute, carbide endmill)
D2 (175 SFM) x 12 =1800...divided by: .750 x Pi (= 2.356)... = 891 RPM spindle speed
.003 (unhardened tool steel tooth load) x 3 (teeth) = .009...x 891... = 8" per minute feed rate

Example: (Same work piece using a 2'' dia. "shell" cutter w/4 carbide inserts (3/4" shank in that same R8 collet)
D2 (lets go to the high 200 SFM) x 12 = 2400...divided by: 2.00 x Pi = 6.283...= 382 RPM spindle speed
.003 x 4 = .012...x 382 = 4.6" per minute feed rate

...Apprentices, trainees etc.: Generally: See how, depending on the stock, cutter etc. yada yada: Milling is like drilling (drill dia.), grinding (wheel dia.), honing (mandrel dia.), (and lathe work but think work dia. od's and id's) ...Smaller = faster rpm (and feed except tiny! Snap crackle pop lol) (but less surface area) and bigger = slower (but more surface area)

...Machine Tool feeds and speeds are related in that sense (including EDM)

 

[mike silvia]

thanks