[wdp67]

Hi again everyone!

I have been doing pretty well with my cnc mill conversion you may have seen me post about before. I have x,y and z all done and have had it working pretty darned good for a while now.

I am now building a toolplate for it and have a question about tapping all them holes. Is there a way to use the machine to tap the holes without having to buy an expensive tapping head? Any help would be greatly appreciated.

Thanks in advance!

Walt

[Vern Smith]

I have not followed your previous posts so I do not know what type of machine you converted but I can give you a little information on tapping with the old Bridgeport style mills without a tapping head. This only works if you can release the spindle and feed it by hand. You will probably find a tapping head to be a good investment however.

Spot and drill the holes with the CNC capabilities. Now you can manually return to the exact position of each hole or write a code for each spot/drill operation and the machine will be there. Put the tapered tap in the chuck and manually crank the spindle down to the point where the tap contacts the hole. While maintaining moderate downward pressure on the spindle/quill rotate the chuck by hand to start the tap into the hole. You only need a couple of revolutions to get it started straight. Loosen the chuck key and pull the spindle/quill up and away from the hole leaving the tap protruding from the hole. Now put a regular hand taping handle on the tap and finish the job by hand. The secret to tapping has always been starting the tap straight and this will accomplish that. You will probably want to finish the bottom of the holes with a bottoming tap.

This process also works with the tail stock on a manual lathe. If your lathe will turn slow enough, less than 100 rpm, you can set the tail stock to slide but not move around and turn on the lathe which will draw the tap into the work. Remember, there will be some lag from where you turn off the motor and when the chuck stops rotating I doubt if either of these procedures are OSHA approved so proceed at your own risk.

Vern

[TonyAllen]

Hello
Cnc Tapping where the Machine does all the process Requires Syncronous Tap Cycles ...Not sure if a home made Machine would be able to accomplish this and would require software to drive the cycle ...if your Z axis feed and Spindle speed can be controlled Accurate enough : for example 1/2 13 Tpi
( 13 being threads per inch ) divide 1 inch divided by 13 = .0769 Thousands
so when your spindle turnes 1 turn the Z axis must move down .0769 thou.
the Trick is when you have gone the depth U want the Spindle has to stop and reverse to counter clock wise rotation AND the feed of the Z axis Must not have any backlash or the Timing of the feed .0769 and spindle will be off
This is when the tap will break... I suggest u Buy a spring loaded head that holds taps ..the spring inside the head allows the Spindle and feed to be off
a little ...with out breaking the tap ...
if U would like to try cnc tapping without the head here are some tips.
(1) Spindle as slow as U can
(2) if you have a different Size Tap or if it is Metric I can help U with Z Feed

I am assuming Your Z axis is controlled by cnc !
Good Luck
Tony

[kling8]

I have tapped parts before using a regular collet tool holder, there isn't any give so machine and spindle have to be rigid, and slow spindle speed as was allready said. It worked well for me that was a 1/2-13 modified bottoming tap. But I did break some taps now and again. Prefer a tapping head, but not always required.

[samco]

I don't know what you have for a machine or control. If you are using mach - you either have to use a floating tap holder or have a positionable spindle (stepper or servo) like...
[nomedia="http://www.youtube.com/watch?v=SNTSkN69r4M"]YouTube- Tapping Attachment 2[/nomedia]



If you are using emc2 - you could mount an encoder on the spindle and do real rigid tapping. (this was done with printer port hardware)
[nomedia="http://www.youtube.com/watch?v=C740zS9R9kk"]YouTube- Rigid Tapping M3X 5 750rpm[/nomedia]

Otherwise - floating tap head should work. (either way - the cnc would have to be able to control the spindle direction)

(or you buy a tapping head )

sam

[wdp67]

Thanks for all the replies, I am going to go ahead and get a tapping head!!

Thanks again!

Walt

[BobWarfield]

Walt, note that you can use a floating tap holder, as opposed to a true tapping head (which is more money). Maritool has some nice ones.

You just need to have some flex in the Z-axis since you spindle won't be precisely synchronized. Plus, you need a good handle on your VFD if you don't use a tapping head with a reversing clutch. If it doesn't reverse fast enough in a blind hole you're going to break the tap. Make sure you go slow enough to give it a chance.

Last thought: a butterfly impact wrench from Harbor Freight costs about $20 and will tap all day long with an Irwin tap adapter. Enco sells the latter to let you put a tapping chuck on any socket tool. It's not as nice as letting your CNC do the job, but it beats the heck out of a pure manual job.

A little more on the butterfly tapping here:

http://www.cnccookbook.com/CCTappingArm.htm

Make sure to use new high quality taps!

Cheers,

BW

[diamondyarn]

Hi, I have a Kira Drill Tap centre and wants to do Tapping with G84 , my Tap is 5mm , what should be the Exact spindle speed and feed rate .and also give the Peck tapping command
Please guide and Help

[Alaska Bob]

Hi Walt,
You probably already finished your jo, but...
I have recently started cutting threads with a single point thread mill from Scientific Cutting Tools. I helically interpolate a hole ~minor diameter and then thread tool starts at bottom and spirals up cutting threads.

One tool can cut 1/4-20, 1/4-28, metric and custom even. It's pretty cool.

Might be something to think about.

--bob

[ctate2000]

Thread mill it. I see you have x,y and z. If you have simultaneous control it will be no problem.