Hello Everyone!

I'm in the process of learning about taping holes on a VMC. I have never used rigid taping. We just bought a VMC that will accommodate this and would like to find some information on feed and speed as well as dwell time.

For example we do a lot of 6-32 & 4-40 machine screw holes and some 2-56 and 0-80 as well. All of what we do is in 6061-T6.

Here are a few questions I have to begin with.

1.) What type of tool holder should I use for best results?
I have a "Floating Tap Holder" which accepts ER-20 collets. This holder has .300 compression and .500 extension. Am I on the right track with this holder?

2.) What taps would be best suited for rigid taping in Aluminum?
Should I consider roll taps (thread forming)

3.) What should I be using for cutting / tapping fluid?


These are just a few questions I have to get started. I am going to practice by tapping in machinable wax. I will also be searching the internet for some speed and feed info and in the machinery's hand book.

If anyone with experience doing this would like to comment, I would appreciate it!!

Thank You,

Kevin

For rigid tapping of course you use a rigid holder not a floating holder.

Have you done a search here on cnczone for both rigid tapping and form taps; these have been discussed a lot and you should find plenty of information. You will have to dig a littler bit.

the folating holder is nice for absorbing some of the machine acceleration inaccuracies, hopefully you will only need a few tenths of that stroke and not .300...

roll taps are very nice for small holes (read as "the way to go" for most applications), they last much longer, they are however are a bit more tricky on the hole diameter prior to forming (larger diameter needed than a cut tap and a tighter tolerance as well) it has been my experience that changing the preformed hole by .001" makes about a .002 change in the post forming minor diameter size (assuming you are close to the proper size to begin with).

if you have never rigid tapped be warned that the cycle turns off any manual override except E-stop.. so once it starts your feedrate override is useless till the cycle finishes.. to reduce underwear loss it is advised for first time setups to do your tapping up high above your part and with a low rpm/feedrate..

now that I have opened the can of worms on feedrate, depending on your machine type/control altering speed means you have to recalculate the feedrate(IPM) to keep the IPR the same,some newer VMC's feed in IPR so that is not needed, and most lathes use IPR almost all the time.


http://www.emuge.com/taps/gfu_druck.html

the folating holder is nice for absorbing some of the machine acceleration inaccuracies......


.... it is advised for first time setups to do your tapping up high above your part and with a low rpm/feedrate..


When a machine is capable of rigid tapping the feedrate is tightly synchronized with the spindle rpm throughout decceleration and acceleration; that is the whole point of rigid tapping. Think about it for a few seconds, the machine drives the tap in, slows to a halt and then backs the tap out; it has to maintain perfect synchronization, perfect being within .0002" or so.

Regarding speed be careful about going too slow because some machines have difficulty maintaining the necessary synchronization at low rpm. I use Haas direct drive machines and at any speed below about 300 rpm they do not perform well when rigid tapping, other members have also found this. At 1000 rpm they are perfect. For small diameter taps such as those mentioned this would be the slowest speed to use.

yes most machines rigid tap cycle are very accurate when they are new,good to the tenths, but you add your worst case couple of tenths to the worst case couple of tenths that the tap manufacturer has, and a couple of tenths of wind up on the tap shank and you almost have a thou... I've tapped many many hundreds of thousands of holes, in many different types of machines, and in my numble opinion the tap always lasts longer in a floating holder, even if the float is a little , there are holders on the market for just that, a thou or 2 of float..

http://www.mmsonline.com/articles/0703rt1.html

Thank you to all who have responded!

I am still waiting on the user manuals for this machine, ordered them last week. Without the manual I can't be certain that the G84 tapping cycle on this machine (Hyundai SPT-V30 - 1998) is actually able to preform rigid tapping in so much as synchronizing the spindle rpm and feed rate. It does a tapping cycle with G84 to be certain.

I have have executed many G84 cycles in the air to establish if the feed rate and spindle RPM seem to be at all synchronized. It would appear not on this machine or at least I am not able to do so.

The control on this machine is a Yasnac MX3 - anyone used one of these??? Ever even heard of it?? :) Circa 1998 vintage? I have a post processor and a Yasnac controller manual (not specific to my machine) so until I get the machine manuals from Hyundai Kia I am kind of at a loss in some areas.

With the post and the controller manual I have been able to implement the G84 cycle but have not attempted to tap a hole, just observed the cycle in air.

The command I used was something like:

G84 G99 Z-0.500 R0.010 P0.100 D1 F5.0;

The L word can also be used to repeat the cycle L times (L3 - 3 times)

Not sure if the dwell is in seconds, tenths of a second, ms or what. It would seem the D setting has no effect at all. Set D1. or D9000., no diff.

I start the spindle prior to the G84 command and set the speed M3 S500 for example.

What I am having a difficult time with getting my head around is determining the feed rate and RPM.

I read somewhere that a using the formula of RPM x THREAD PITCH = FEED RATE. In that post the example listed was for a 1/4-20 tap. The person that posted this example came up with 500rpm x 0.05 = 25 ipm.

Looking at thread pitch charts I see the basic pitch for 1/4-20 listed as .2175 and what they list as "section at minor dia." in sq. inch as .0269. Was this person using the sq. inch value x 2 as the basis to arrive at 0.05 for the thread pitch or maybe I just don't understand!

Is any of this valid to serve as a starting point for calculating RPM and feed rate?

Any thoughts on any of this???

In my opinion, I would take out the dwell. Seems like that would cause tap to break. Especially small ones you are working with. If you are tapping blind holes that small, I definitely would go with a thread forming tap. Also figuring out speeds and feeds for standard taps is very simple. FEED RATE x THREADS PER INCH = RPM. So for a 1/4-20 tap, for example 5 IPM x 20 = 100 RPM. Also on some machines you can use a G95 which uses feed per revolution. Basically you would just set your feed the same as your PITCH. 1/4-20 TAP has a pitch of .050" (1/20) Then no matter what RPM you use the machine will adjust accordingly. Good Luck!

Looking at thread pitch charts I see the basic pitch for 1/4-20 listed as .2175 and what they list as "section at minor dia." in sq. inch as .0269. Was this person using the sq. inch value x 2 as the basis to arrive at 0.05 for the thread pitch or maybe I just don't understand!
Any thoughts on any of this???


there is pitch Diameter and Pitch lead.

.2175 is the pitch diameter of 1/4-20, it's a gage diameter measured 1/4 lead from centerline, a way to measure the threads with a number and not go/nogo.

the pitch you seek is the threads per inch, so 1/4-20 has 20 threads per inch (-20) so for every turn it travels 1/20 of an inch or .050.... a 1/4-28 has 28 threads per inch, so a turn is 1/28 of an inch=.03571. etc.. metric threads make it easy, say m6x1 the thread moves 1mm per turn.. m4x.75 moves .75mm per turn etc..


so on inch threads you use this Feed in inches per minute = RPM*(1/TPI) where TPI= threads per inch

This is good information, just what I was looking for, thanks guys!

I don't know why I was over thinking the thread pitch (Thank you CNCWISS1) but I understand that completely.

I believe this machine will feed at IPR with G95, will give that a try. This also makes sense, thanks Bugz!

I'll let you know how things work out. Waiting on collets for the tap holder and still no manuals in the mail. By the time the manuals get here, I'll be able to write a new one from scratch! :)

depending on the machine, you may need to turn on the rigid tapping function with an m-code prior to issueing the G84!!!!

My personal preference is to use IPR, as a simple speed change will not require me to recalculate the feed!!!!

Safety first!

You need to use M29 S500 before the G84 line to synchronise the spindle I believe, and take out the S500 M03 part

Thanks for the replies. I read about using M29 in another post so I tried it on this machine but received an program error.

If the manual ever arrives perhaps I will learn how this machine rigid taps or if it does at all.

G95 feed per rev was an option on this machine and it would appear that this option is not turned on or not installed. Seems like it would be a parameter setting, but again back to the manual! Anyway, when issuing G95 I get a program error (G) which I take to be invalid G word. G94 feed per inch is the power up default. A G94 command works, no error.

There has to be someone out there that has used one of these machines!

In the meantime I just couldn't wait to break a tap, so I did. Broke a tap. I attempted to tap a #6-32 hole on a piece of 6061-T6. I drilled the hole at .1065 (#36) and was using a spiral point tap. I set the spindle at 320 RPM with a feed of 10 IPM (thread pitch of .03125 x 320rpm = 10 ipm). Using flood coolant everything was fine going in, worked perfectly! It was on the way out that I heard it snap! I was using the tap in a collet holder, not a floating holder.

Maybe when the collets for my floating holder arrive, I will give it a try and see if I can't break another tap! :) I also have some roll taps on order as well, I think that will also help.