Mini Mill can it repeat rigid tap?

[Loading]

Hello All,

I'm going to a local college here to use their Mini Mill. I've got to make around 100 pieces with 2 3/8-16 tapped holes about ~1" deep, in a through hole. The material is 6061.

Normally this wouldn't be a problem, however, I'm fairly certain the school does not have any tap holders, nor do they have collet holders.

Anyone know what the shank size on a 3/8-16 tap would be? If it's 3/8 I could just mount it in a 3/8 end mill holder. If it isn't, I'll most likely have to put it in a drill chuck.

I'm worried a drill chuck might not be able to hold it quite tight enough to drive it hard, so I'm thinking I may have to tap it in a couple steps.

Any advice anyone can offer would be great.

Also, could someone recommend what speed/feed would be good on a mini mill. All I've got is some cheap spiral point 3/8 taps. Thanks in advance!

[JROM]

To get the feed rate for any tap devide the number of threads per inch (16) into 1 then multiply buy the RPMs you are running it at.
1 devided by 16 = .0625 times 300 RPMs = 18.75 IPM Got it?
If you have to use a drill chuck, use one with a chuck key and tighten at all three holes. Tap the holes all in one shot with lots of cutting fluid. You cannot retap the holes on the machine it will not repeat the starting point and you will cross thread the holes if you try. If they are thru holes you should have no problems. Oh try to use a good sharp tap for the best result.
Good luck

[Loading]

Thanks for the reply.

I know how to calculate speed and feed for a tap, just not sure what a good starting place for a mini mill would be. On one hand I'd like to run it at low revs, as the taps I have access to are all rather bad. On the other hand, I'm not sure if the mini mill will have enough torque at low revs. The mini is rated at 33 ft-lb at 1200 rpm. If you slice that down to 400 rpm, are you then only playing with ~10 ft-lb?

I've used VF models of Haas before, and on them you can repeat tapped holes. The tap will enter in at the same location allowing you to take several steps at a hole. Great for long blind holes!

[Geof]

To answer the question in your title the MiniMill can repeat rigid tap if the option is turned on.

Go to Parameter 57 and in the left column you will see RIGID TAP and REPT RIGID TAP; both should have a 1. If they are zero there should be a T by the RIGID TAP and this means you can turn it on for a 200 hour trial.

If you cannot find the REPT RIGID TAP in the Parameters have a look in the Settings; I seem to remember them being in different places on older machines.

Regarding holding the tap a 3/8" ER32 collet will do fine, we use them all the time in both 6061, leaded steel and 1018. Most times we repeat rigid tap to clear chips.

We run at 1000 rpm and have found if you go slower such as around 300 to 400 hundred the machine may have diffculty synchronizing. I think the torque drops off too much at the lower speed.

[axis]

if you want to run faster just double the speed and feed to get them were you want them if you want 1200rpm then run 75 imp i think .if you can calculate speed feeds put it were you want it .
if you are running cheap taps you get cheap threads, go buy a new tap they arnt that much money.you are getting the machine for free it sounds like so spend 25-30 $. run it in one pass with lots of coolant.

[PBMW]

If you are making blind holes, a spirol tip tap will push the chip ahead and into the bottom of the hole. You want a spirol flute tap to get the chip out of the top of the hole. But....I would use a form tap myself.
I tap 3/8 16 holes all the time on my mini at 1500 rpm in alum.
Oh...a tap in a drill chuck will get ugly. Using a EM holder will result in broken taps as they are not a standard holder size. You are going to need either a tap holder or a collet and I'd go for an ER32. Otherwise, you'll be either making oversized holes or breaking taps.

[dougtyler]

It's alot easier to figure the feed for a tap if you use G95 (feed per revolution)
This way, you can play with the spindle speed without having to refigure to feed rate.

[1ctoolfool]

don't use a drill chuck with a tap, asking for trouble,

the minimill will re-start taps as many times as you want, just make sure the option is turned on as mentioned. Use 1000-1500 rpm as mentioned.

my opinion, i only own one keyless chuck and use it only when I'm being lazy or don't have a correct size collet available, chucks are just not reliable or accurate.

Seen many jobs ruined with drills slipping and/or pulling out of chucks.

Joe V.