[Gundawg]

I have a product I make for myself to sell in my small Marine Products business that I need to tap 4 1/4-20 holes in 6061 T-6 Al each part the fixture holds 10 parts so 40 holes per batch.

My machine has a Proto Trak AGE3 control for those that don't know the machine or control it is a 3 axis CNC bed mill with manual quill and the column moves in the Z direction through CNC control. The control does not turn the spindle on or reverse directions. The control will turn off the spindle but that is all the control it has for the spindle. The machine travels are 31" x 17" x 23". The spindle is 2 HP. (3HP on static phase converter)

The holes I need to tap are in 1" 6061 I have purchased a 2E Procunier tapping head is this the best way to do this? I read the directions on the tapping head and it says it must be withdrawn at 2 times the speed that it is plunged. My control does not have this option I could go in and edit the code or write code to do that.

The other thing I could do is locate the spindle over the hole and program a pause then tap with the manual quill (not preferred). What have some of you done with this type machine? Thread mill? Can a 1/4-20 be thread milled? I have some spiral taps to use with this Procunier head I would like to have the fastest cycle time possible given my equipment.

I don't mind spending some money on tooling so if I need different taps or tooling I can do that. I plan to make many of these parts in the future so tooling will pay for itself.

I will add the holes are semi blind in that 2 of the 4 holes are covered on the bottom of the part by the fixture that holds the parts for machining. I will drill clearance holes in the fixture so the tap does not bottom out. I also do not really need to tap all the way through the part so I may just make them blind holes and go 1/2" deep that is an option.

Thanks for any help you can give.

Mike

[txcncman]

Are you sure it says "must be withdrawn at 2 times the speed"? Or is that just recommended?

I would still drill holes through but only tap slightly more than minimum needed.

Yes, you can thread mill. It will take up to 100 times longer than tapping.

[Gundawg]

Here is a link to the manual page 2 number 5. I did not know this when I bought the tapping head.

http://www.rockford-ettco.com/Portal...1000-13000.pdf

[txcncman]

If feeding by hand with the quill, this will not be an issue for you. If feeding with Z axis, you will need to match infeed to the RPM and double the retract feed. In your situation, I doubt you can manually regulate the spindle speed enough to allow for this. You will be stuck with using the quill for the actual tapping and use the CNC for positioning only.

[Gundawg]

Thanks txcncman I wonder if the Tapmatic heads work this way? I bought the Procunier used on ebay so I could move it on and change brands if the Tapmatic head is different. I don't really want to stand in front of the machine to tap holes manually.

Mike

[txcncman]

I do not recall that old Tapmatic models doubled retracting speed. Easiest thing would be look up Tapmatic on the internet and if needed contact them directly.

[Gundawg]

I do not recall that old Tapmatic models doubled retracting speed. Easiest thing would be look up Tapmatic on the internet and if needed contact them directly.

I looked up the manual and it did not specify that it doubled speed on retract so I will call them next week.

Thanks again Mike

[lstool]

A couple years later.... but i find this post and if you or anyone still interested.... I tap on a Proto Trak bed mill all the time using a CNCTapmatic tapping head.... automatically.... I will tell you the exact proceedure and give the exact model tapping head I use.... I do not recomend using a tapping hear that doubles the rotational speed when retracting but it will still work with this proceedure..... and yes you use a boring cycle to do this.... you need to calculate the speed and feed for your thread pitch (back off the feed rate by 2-3%)

[Burdyburdy]

A couple years later.... but i find this post and if you or anyone still interested.... I tap on a Proto Trak bed mill all the time using a CNCTapmatic tapping head.... automatically.... I will tell you the exact proceedure and give the exact model tapping head I use.... I do not recomend using a tapping hear that doubles the rotational speed when retracting but it will still work with this proceedure..... and yes you use a boring cycle to do this.... you need to calculate the speed and feed for your thread pitch (back off the feed rate by 2-3%)

hi isotool, i have a prototrak 4000 bedmill, please advise your methods.

[lstool]

Hey Burdyburdy, The tapping head I use is the same as this...
Tapmatic #10 - 1/2 Reversing Tapping Head 1" Shank NCR-1A (LOC2716B)

The method is simple, think RPM (Rotations Per Minute) first how fast you want to spin the spindle to tap. Then to get your IPM (Inches Per Minute) number to input into the control you need to take your tap pitch and multiply it by your RPM's to get you IPM's For example (1/2-13 tap at 200 RPM's) Tap pitch = 1" divided by 13 threads per inch=.0769 Now multiply your pitch X RPM (.0769 x 200 = 23.07 IPM) less 2-3% enter in control 22.5 IPM

So using a boring cycle on your ProtoTrak set your Z rapid for that tool higher than normal I use like 1/2" this allows the tap to fully retract before rapiding to the next hole so the formula is... RPM x Tap pitch = IPM (Inches Per Minute) back off feed slightly like 2-3% Use boring cycle and set Z tool rapid plane to .5.
Set your depth as you normally would tap to than check and adjust depth to suit.