Rigid Tapping 3/4"-16

[sklemp]

Hi all,

I'm just getting comfortable with our Fadal VMC 15XT and just when I think I can do something, Fadal throws me for a loop.

I have a file that needs 100 3/4"-16 holes tapped. I have already drilled them, they just need to be tapped.

Can anyone suggest an optimal spindle speed and Q value for the machine?

Currently in MasterCam it is setting the spindle speed at 2448. I know that can't be right. I'm only tapping at 1.03" deep.

Can someone suggest a way to calculate all the necessary values for the tapping function? Feedrate, spindle speed, Q value, etc?

Thanks in advance,

[Joe S.]

You'll find everything you need in section 4 of the user manual.
http://www.compumachine.com/Support/...xed_Cycles.pdf

[carbidecraters]

G84.1 G99 Z-(put in your final Z here) S320 F20.

This is what works great for us on thsoe taps.

[sklemp]

carbidecraters,

Thanks for the reply, I will try these settings for our tool. Do you not run a Q value at all? From what I've read the code needs to be something like this:

G84.1 G99 R0+.1Z-1.2 F20.1 S320 Q.05

Is this what you are doing?

I forgot to mention that I'm running Format 1 on the machin.

Joe S.,

I've read the manual inside and out regarding this issue, but have never seen that section. I'll give it a more in-depth read. I'm also just trying to find out what other people are running for their spindle speed and feedrate with positive results. The first one I tried stripped out the hole so I wanted to get an idea of what optimal speeds are for this machine.

[carbidecraters]

Get rid of the .1 after F20. Mastercam has an issue with Rigid tapping for the Fadal 4 axis post. In 22 years we have never used a Q designation HOWEVER it may be needed for either RETURN PLANE in FORMAT 1 or something else I am not aware of.

[Edster]

if youre running format 1 you need the q value. q is the lead of the thread. to figure it out divide 1 by the threads per inch of the tap, in youre case 16. you don't need a feedrate just the rpm and q.

[sklemp]

Thanks for all the information.

I'm going to try two things tomorrow.

G84.1 G99 R0+.1Z-1.2 S320 Q.0625

G84.1 G99 R0+.1Z-1.2 F20 S320

I'll let you know what works for us.

By the way, this is aluminum that we are drilling and tapping.

Thanks for all the help.

[Techman]

I run our machine in format 1 and use MasterCam.
It would post-

G84.1 Z-1.2 R0.1 F320. Q.0625 M45

If I want the machine to tap in high range you would use F320.2
That would force the machine to stay in high range but I doubt that would be desirable with a 3/4 tap.
Techman

[DareBee]

100X 3/4-16 holes - wow
I recommend thread milling instead.
I hope your luck with large dia tapping is better than mine.

[Edster]

I tap some 3/4-10 holes in C110 copper on my VMC3016L. The load meter is maxed out. I would say that it's the max tap size for the machine

Aluminum should be easier, good luck.

Oh, you should have a G84.2 in the line before the G84.1, it readys the spindle for rigid tap.

Also I usually use R0+0.4 for the rapid plane when tapping, it gives the spindle time to sync up to the feed. I'm pretty sure it says something like that in the manual.

[DareBee]

Ya - the manual suggests .4 clearance for sync.
Once in rigid tap mode you do not need to initiate it again.
just use XY moves and control automatically taps once it gets there using the parameters set in your initial G84.1 (well - in format 2 anyway). Continues on until you do a G80.
HTH

[carbidecraters]

Good catch on the Q. We rigid tap with only .2 sync distance sometimes .1