Newbie- Can you tap on a machine WITHOUT rigid tap?

[svirfnebli]

Ok, totally noob question.

One of my 9 fadals (all VMC 4020's) is an older machine that does not have the rigid tap cycle and cannot be easily upgraded. Of course its that one machine that I need to do some basic taping on. I need to make 3/8" deep holes with 10/32 threads in steel. I have a compression holder at my disposal.

My fadal tech said there is a TAP cycle of some sort, but no rigid tap. Is he full of crap? Can I do SOME form of taping on the machine? Im not seeking high precision, but some basic threads. If so, can anyone tell me how to do it?

I currently use mastercam X3 for NC programing.

HEeeelllpp!!

Matt

[Geof]

You need a floating tap holder; this allows the tap to follow its own correct pitch even if the machine spindle and Z feed are not perfectly synchronized. The tap holder floats between opposing springs with a small amount of axial travel so the tap can go ahead of or lag behind the spindle travel.

[Bwana Don]

Use a tension/compression tap holder. The cycle you want to use is Right Hand tapping which is G84 (I think). Program the feed the same as rigid tapping except only use 90-95% feed in and out. This allows the tap to cut ahead of the push/pull tapper. You'll see the tap going faster than the feed on the machine, actually you'll see the tapper getting longer (pull on the end it has a spring in it).

I hope I explained this well enough. The principle is that the tap will cut the threads, not the feed of the machine. The tap is feeding down faster than the programmed down-feed of the machine. It's going at 100% the machine is going at 90-90%.

Example;
1/4-20 thread (20 pitch)
500 RPM
feed = (RPM/pitch)*.95 or (500/20)*.95 = 23.75 IPM for 90% = 22.5 IPM.
(Tap is actually going 500/20 = 25 IPM)

I hope I helped; my machine is a 98 Fadal 3016 with a 88HS controller.

[svirfnebli]

So my mastercam post processor will only due rigid taping.. Which I believe is G84.2 .. Do you think I can just remove the .2 so that it's EXACTLY the same as the rigid tap, just with a G84 code instead of the G84.2?

[denmar]

YOU CAN ALSO USE A TAPMATIC HEAD: G75F2000.(LOW RANGE)Q0.050 (20 THREADS PER INCH)

[Bwana Don]

Originally Posted by svirfnebli So my mastercam post processor will only due rigid taping.. Which I believe is G84.2 .. Do you think I can just remove the .2 so that it's EXACTLY the same as the rigid tap, just with a G84 code instead of the G84.2?

I think so, try it on a dry run first. Make sure it reverses at the bottom and looks like it feeds down and then back up. Might want to try the whole thing in a piece of scrap first to insure it all works. I think this is it though.

G75 with a tapping head works also, like denmar said. Tapping heads will cost you, but if you all ready have one go for it.

[Neal]

The G84.2 is a calibration cycle. The code for rigid tapping the G84.1. You can do compression/tension tapping using the G84 code. You line should read in the following style: Format 1 = G84 G99 R0+.2 F(RPM) Q(lead of the thread) Z-.xxxx
Format 2 = G84 G99 R0+.2 F(calculated feed rate) S(RPM) Z-.xxxx
You can also use the G75 code for Tapmatic sytle of tapping.
Neal