Tips and Tricks for running a Drill Tap machine more efficiently

[Chips Everywhere]

We just received our new Haas DT2 and I hope to start cutting by the end of the week. The machine is dedicated for only cutting 6061-T6 Aluminium.

I would like to run these parts as efficient as possible within my programming abilities. These are the following areas I think I can improve on:

I have to tap 64 holes per cycle, 32 - M3x0.5 blind (13mm deep) and 32 - M5x0.8 thru (3mm). Haas claims the DT can, allegedly, tap at 5k rpm. How can I determine what is the maximum speed I can cut with my taps, to take advantage of this feature? Do I cut the threads at the tap manufacture's recommended SFM and reverse the tap out at 5k rpm?

In a drilling operation, my Feed and Retract heights are the same by default, they sit at 0.20" above the Top height. I feel like I can improve on this by lowering that height, what is a safe distance I can use? All the holes are on the same plane and no obstacles are in the way.

Any feed back is greatly appreciated.

 

[Mtndew]

We just received our new Haas DT2 and I hope to start cutting by the end of the week. The machine is dedicated for only cutting 6061-T6 Aluminium.

I would like to run these parts as efficient as possible within my programming abilities. These are the following areas I think I can improve on:

I have to tap 64 holes per cycle, 32 - M3x0.5 blind (13mm deep) and 32 - M5x0.8 thru (3mm).

Haas claims the DT can, allegedly, tap at 5k rpm. How can I determine what is the maximum speed I can cut with my taps, to take advantage of this feature? Do I cut the threads at the tap manufacture's recommended SFM and reverse the tap out at 5k rpm?

In a drilling operation, my Feed and Retract heights are the same by default, they sit at 0.20" above the Top height. I feel like I can improve on this by lowering that height, what is a safe distance I can use? All the holes are on the same plane and no obstacles are in the way.

Any feed back is greatly appreciated.

On those smaller taps, tap at 5k rpm in and out. I tap at 6k rpm on my Brother.

Feed and retract heights .02" or even at .01" is about the best you can do when peck drilling and increase peck depths. If you really want to cut cycle time, get carbide drills with thru spindle coolant so you don't have to peck. Your machine does have thru spindle coolant....right?

 

[Shawnrs]

Are you using 1 tool for each type of hole(drill/tap) or are drilling and then tapping holes?

 

[Chips Everywhere]

On those smaller taps, tap at 5k rpm in and out. I tap at 6k rpm on my Brother.

Feed and retract heights .02" or even at .01" is about the best you can do when peck drilling and increase peck depths. If you really want to cut cycle time, get carbide drills with thru spindle coolant so you don't have to peck. Your machine does have thru spindle coolant....right?

I have carbide bits, but no spindle thru coolant. Since most of the holes depths are 2XD, except the M3

 

[Chips Everywhere]

Are you using 1 tool for each type of hole(drill/tap) or are drilling and then tapping holes?

I am drilling, then tapping.

 

[Shawnrs]

I am drilling, then tapping.

I would set all your R-Planes for the drills to R.05 or closer like Mtndew said and the taps to R.1 or R.2. I think you can drill thru without pecking but you may need to reverse the spindle to remove the ball of chips on the tool.

 

[Chips Everywhere]

I would set all your R-Planes for the drills to R.05 or closer like Mtndew said and the taps to R.1 or R.2. I think you can drill thru without pecking but you may need to reverse the spindle to remove the ball of chips on the tool.

There is a feature that allows me to chip break, without retracting the drill, at a determined distance and it has worked great for me so far. I'm using Guhring parabolic drills for the M3 tap and so far I've been very happy with them.

Thank you for the feed back.

 

[Mtndew]

I have carbide bits, but no spindle thru coolant. Since most of the holes depths are 2XD, except the M3

In that case, eliminate pecking where you can. Unless you're making tens of thousands of these parts, a second or two here and there isn't going to hurt the cycle time.

Oh, and carbide bits are for routers.

 

[beege]

Roll tap or Cut tap? Roll Tap will be better for blind holes.

 

[Shawnrs]

What is your max RPM for this machine? I am willing to bet you max it out on the parabolic drills.

 

[Chips Everywhere]

What is your max RPM for this machine? I am willing to bet you max it out on the parabolic drills.

15,000 rpm

 

[Chips Everywhere]

Roll tap or Cut tap? Roll Tap will be better for blind holes.

Cut tap. I had a lot of issues with those M3 taps in the beginning. Broke a about 7. Now have it dialed in and it’s been one tap for 400+ holes and still going

 

[gkoenig]

Cut tap. I had a lot of issues with those M3 taps in the beginning. Broke a about 7. Now have it dialed in and it’s been one tap for 400+ holes and still going

Did you get to the bottom of why this was happening? An M3 form tap in 6061 should be fine, even at 5x depth.

 

[BugRobotics]

Did you get to the bottom of why this was happening? An M3 form tap in 6061 should be fine, even at 5x depth.

Agreed. Form tap is the way to go here and properly set up can run thousands of holes in 6061.

 

[Chips Everywhere]

Thanks for the feedback, will order a form tap.

For roughing,

Using a 3/8 chip breaker EM, for pockets and outside contours, is it preferable to 50% radial engagement and slower feed or 10-15% engagement and high feed? Axial engagement is about 1/2”.

 

[DouglasJRizzo]

We just received our new Haas DT2 and I hope to start cutting by the end of the week. The machine is dedicated for only cutting 6061-T6 Aluminium.

I would like to run these parts as efficient as possible within my programming abilities. These are the following areas I think I can improve on:

I have to tap 64 holes per cycle, 32 - M3x0.5 blind (13mm deep) and 32 - M5x0.8 thru (3mm). Haas claims the DT can, allegedly, tap at 5k rpm. How can I determine what is the maximum speed I can cut with my taps, to take advantage of this feature? Do I cut the threads at the tap manufacture's recommended SFM and reverse the tap out at 5k rpm?

In a drilling operation, my Feed and Retract heights are the same by default, they sit at 0.20" above the Top height. I feel like I can improve on this by lowering that height, what is a safe distance I can use? All the holes are on the same plane and no obstacles are in the way.

Any feed back is greatly appreciated.

When tapping at high speeds, keep in mind that the spindle almost never reaches the target RPM before stopping to reverse. None of these holes are terribly deep so the machine isn't really going to reach the intended speed.
What WILL happen is that your motor loads are going to be sky high and the wear and tear on your spindle will be enormous.

I highly recommend a Tap-Matic NC head or similar. MUCH faster for doing lots of tapped holes and the machine never physically reverses direction. Easier on the spindle, motors, drives, etc. I had one and I could even cycle through the ATC with no issue. A time saver.

 

[GiroDyno]

I highly recommend a Tap-Matic NC head or similar. MUCH faster for doing lots of tapped holes

 

[2outof3]

When tapping at high speeds, keep in mind that the spindle almost never reaches the target RPM before stopping to reverse. None of these holes are terribly deep so the machine isn't really going to reach the intended speed.
What WILL happen is that your motor loads are going to be sky high and the wear and tear on your spindle will be enormous.

I highly recommend a Tap-Matic NC head or similar. MUCH faster for doing lots of tapped holes and the machine never physically reverses direction. Easier on the spindle, motors, drives, etc. I had one and I could even cycle through the ATC with no issue. A time saver.

I am sorry but that is just not true. 0-6,000 RPM is milliseconds on a good machine tool of this type. I will let the customers tell their stories but that is archaic.

 

[david n]

Doug............you don't need a tapmatic head on a drill tap..............well, at least not on a Brother.................a Haas DT.......who knows?

 

[DouglasJRizzo]

I am sorry but that is just not true. 0-6,000 RPM is milliseconds on a good machine tool of this type. I will let the customers tell their stories but that is archaic.

When I worked for Doosan (Now DN-Solutions), the tapping cycles could NEVER get to that level before the threads were completed. Ever. You can program an M29 S6000, but it never sees 6k in the cycle. It might ramp to 2k or 3 on a deep hole, MAYBE. But 6k? I'd have to see some real good proof of that.
Even if you could do this - and I don't think it's physically possible, look at the load meter. You're slamming into the red for the nearly the entire FWD/REV cycle. Sure it's only for a few seconds, but with lots of holes, over a 20-30 year machine life? Nope. I wouldn't.