[patveth]

I'm building a Bracket to hold a High Speed spindle. I plan to make the bracket similar to the one Tormach sells. I'll use 1.5" 6061, (because I allready have it). My quandry is, how to best cut the 3.375" hole that fits over the Tormach spindle.

Here's some of the options that I'm considering:

1. Plunge cut a 3.375 dia. circle using a .5" end mill, (cut approx .020 undersize and then finish profile or bore to size.

2. Cut a 3.375 pocket thru the 1.5 material.

3. Trepan with a hole saw and finish profile or Bore to size.

I suppose that all three methods would work but I'd like to hear your opinions and or other options.

Maybe option 4 would be, buy bracket from Tormach.

[Don Clement]

I regularly trepan large diameter through holes (3"-4.25" diameter) in 1/2" thick aluminum plate using a 1/2" 2-flute high helix endmill programmed using G2 and depth of cut increments of 0.1" and plenty of flood coolant. The finish cut is done with a boring head and CCGT carbide inserts. See: http://i72.photobucket.com/albums/i1...blankFlynn.jpg I suppose that if the endmill was not long enough to trepan 1.5" thick aluminum then one could trepan half way through and flip the part to trepan the other half through. On my manual mill and manual lathe I use an SPI Val-Cut 8mm "dragcut" trepanning tool but since getting the Tormach it is way easier to program an end mill to do the trepanning. Here is a picture of the Val-Cut trepanning tool in use on my manual lathe http://i72.photobucket.com/albums/i1...repanning2.jpg BTW I don't use flood cooling on the manual lathe or mill but a Vortec model 610 cold air gun when trepanning. The flood coolant on the Tormach is much better than the Vortec cold air gun but flood cooling on a manual machine makes quite a mess.

Don

[patveth]

Thanks Don,

That's pretty close to my option #1. I'll have to check and see if I have an end mill long enough.

Pat

I regularly trepan large diameter through holes (3"-4.25" diameter) in 1/2" thick aluminum plate using a 1/2" 2-flute high helix endmill programmed using G2 and depth of cut increments of 0.1" and plenty of flood coolant. The finish cut is done with a boring head and CCGT carbide inserts. See: http://i72.photobucket.com/albums/i1...blankFlynn.jpg I suppose that if the endmill was not long enough to trepan 1.5" thick aluminum then one could trepan half way through and flip the part to trepan the other half through. On my manual mill and manual lathe I use an SPI Val-Cut 8mm "dragcut" trepanning tool but since getting the Tormach it is way easier to program an end mill to do the trepanning. Here is a picture of the Val-Cut trepanning tool in use on my manual lathe http://i72.photobucket.com/albums/i1...repanning2.jpg BTW I don't use flood cooling on the manual lathe or mill but a Vortec model 610 cold air gun when trepanning. The flood coolant on the Tormach is much better than the Vortec cold air gun but flood cooling on a manual machine makes quite a mess.

Don

[Scott_M]

Hi Pat
I will be doing the exact same job in a couple of days.
I am going to try the hole saw. I bought a new Milwakee deep bi-metal 3" hole saw for the ocassion. I will use lots of flood coolant and a very slow feed to keep chip size down to a "flushable" size.
I will post back in a few days to let you know how it went.

Scott

[300sniper]

if i were just making a one-off for myself and time wasn't a huge concern, i'd probably machine a pocket with my favorite 3 flute ma ford endmill leaving .010" for a full axial depth finish pass. that only uses one tool and the pocket makes lots of room for chip evacuation. i can't imagine it taking more than 10-15 minutes.

[M250cnc]

Chain Drill

For those not in the know a series of holes close together, say 8mm dia 8mm centres.

Easy

[Scott_M]

I tried the hole saw this morning.
In order to keep the chips fine enough I had to run the feed slow enough that it created chatter. Kind of noisy but it cut good. I ran at S 250 F.5 it took about 10 min. with several starts and stops trying to figure the right speeds and feeds. Hole measures 3.025". I figure it is just about as fast as pocketing with a lot less chips. And I have the slug for another project.
I will call it a success.

Scott

[patveth]

Thanks to everyone who responded. I'll probably Trepan with a .5 End Mill. Looks like the other options I mentioned in the original posts are similar those proposed by responders. So...o I guess my options are validated at least.

Pat