[subi4ester]

Just got a new VF3 / 50taper and having some issues rigid tapping a blind hole. Im about 100% sure Im not doing something right so Im asking for some insight as Im new to the cnc machining world. Work piece is A36. Im spot drilling first, then drilling a 27/64 hole 1.75" depth and then rigid tap 1/2"-13 to 1.25" depth, ER16 collet. RPM @~530, feed @ 50%(20.5692 feed rate) First attempt I managed 5 holes before breaking tap (typical 3 flute) while retracting and using sythetic coolant in machine from flood nozzles. Next attempt tried a 4 flute tap, broke while plunging first hole. Fellow employee suggested shutting off coolant and applying tapping oil to tool before each hole. This ended up working, but kind of a pain to feed hold and apply oil before every hole. There is 22 tapped holes in each part. I just dont see it being practical to babysit the machine. Im assuming my feed rate must be wrong or ??? Please help!
Boss is becoming skeptical of this new maching being used for tapping holes....Id rather find out what Im doing wrong so I can use the machine properly and not tap everything on the manual mill.

Monday I will have some spiral taps to break, hopefully not...

[Geof]

Are you going 1.25 deep in a single shot?

I woiuld Repeat Rigid Tap this depth, something like 0.4, then 0.7, 1.0 and 1.25.

I would run at 1000 rpm and use coolant but increase the concentration to something like 10 to 15%.

I would also use spiral flute taps.

[Dane Lindon]

1) 50 Taper machine, and your using a ER16 collet for a 1/2-13? Floating tap holder with drive collets work great with rigid tapping. It gives the tap axial and radial float so the tap has a chance to change direction. There is a bit of mass in a 50 taper spindle that suddenly changes direction. The last thing you want is for the tool to spin in the collet, defeats the rigid tap feed algorithm.

2) HSS tap SFM for A36 is 25-40. I would start at S260 F20. You need to tap at 100% feed, otherwise the tap lead will not be correct. (simple math- S260/13=20 the 13 is threads per inch)

RPM @~530, feed @ 50%(20.5692 feed rate) Your lead is 25.766 per inch

3) 75% thread engagement would indicate using a .4375, 7/16 pilot hole. (you will find over time that most drill guides use too small of a pilot.) Look up the tolerances for a 1/2-13 UN 2B in the Machinery's Handbook and set your pilot to the top of the minor diameter range. You will not break as many taps.

4) You will want a tap that lifts the swarf out of the hole. Also you don't want the tap recutting the chip upon retract. Take a look this style of tap. http://www.besly.com/catl/catl4113h.htm It has a long enough flute to tap the full hole without recutting. What you don't want to use is some hand tap, picked up from the local hardware store.

5) A36 is a good candidate for form tapping. The best part is that you don't have to worry about chip control. Take a look at this... http://www.ctemag.com/pdf/2006/0602-Tapping.pdf
But, you will want to use a tap holder, not a collet.

I know of a Haas VF3 that taps 3/4-10, 2.0 inches deep in 4140HT day in day out since 1997. I'm sure your machine can handle it. (seems it can break 1/2-13 taps like match sticks.)

Good Luck.

[HuFlungDung]

ER16 is definitely too small to drive that large of a tap. I used to have trouble making an ER16 drive a 3/8 UNC tap even with a floating tapping head.

I always apply tapping fluid to my taps because I get mad when a tap chips early in its life. Coolant is not a tapping fluid, IMO.

I agree with Geof about repeat tapping, although I would probably only use one repeat because I use tapping fluid.

Best way to figure out what works best: hand tap a hole full depth using coolant for a lube. Hand tap another hole full depth with tapping fluid. Hand tap another hole with a retraction half way down. Feel the difference.

Haas makes some kind of a lubricant squirter that will shoot a shot of lube at the tap. I presume such a thing was invented because there is a need for it.

If feasible, program all your tapping near the end of the program. This way you are going to be there soon to change the part anyways, so you spend a couple of minutes with a brush (door interlock disabled, but still keep your face behind the glass because when a tap shatters it can explode like a bullet). Also blow coolant off the part before tapping to avoid blowing off the spent lube into the coolant. There may be some lubes that are coolant compatible and won't create an oil slick.

[Delw]

with a tap that big in A36 wouldnt it be faster and much more effecient to thread mill the hole with a 60º thread mill cutter?

I been thread cutting in alum 3/8s and bigger and it seems to be much faster, and I am using gages and havent had any problems.
I am just asking as I don't do alot of thread tapping or threads on a mill, and after 3000+ tapped holes in one job order I still stand next to the machine when its tapping with my finger on the feed hold button. if could find a millling cutter for a 4-40 I would be milling them instead of tapping LOL..

Delw

[subi4ester]

Ok, I'm an idiot, Iam using an er32 collet. I will have the spiral flute taps Monday and try them out. I will also try a 7/16 pilot hole and correct my feed to 100%. I do have all the tapping at the end of the program so I will do the door hold override and oil by hand depending on how it goes.

[subi4ester]

Are you going 1.25 deep in a single shot?

I woiuld Repeat Rigid Tap this depth, something like 0.4, then 0.7, 1.0 and 1.25.

I would run at 1000 rpm and use coolant but increase the concentration to something like 10 to 15%.

I would also use spiral flute taps.

yes in a single shot, I will also try the repeat rigid tap.

[Dane Lindon]

Back a few years ago, when rigid tapping came out, I asked the machine salesman what tooling I would need for tapping. He stated that collets would be fine. Haas Applications also stated that collets are sufficient with rigid tapping. Any way, suddenly our tap usage went up. We had broken taps in forgings and castings that cost more than the floating tap holders. I had the operators go back and use the floating holders with rigid tapping. Tap consumption was reduced below historic usage. We no longer needed to burn out broken taps. The key is that it allows the system enough give that the tap is no longer the weak point. I favor the Bilz WFLK Quick Change Tension & Compression Chucks pages 55,56
http://www.bilzusa.com/News/Uploaded...2007-small.pdf

When you get a chance, check the shank on the tap you are using. If it is spinning you will see the shine, and if it is your collet is now junk.

As mentioned before, coolant concentration does have measurable effect on tapping. Keep it heavy.

I wouldn't be to hard on yourself, its not like your the first one given a new machine, and expected it to work as promised. I'd eat some crow, if it meant not having to manual tap that many holes.

[BobWarfield]

Some great tips in this thread, thanks for sharing guys!

Other thoughts:

Lots of machining calculators are available that can help with the speeds and feeds. With my G-Wizard, for example, I would've started with the thread:



You can see your tapping drill sizes there for cut and form taps, as well as pick up the pitch. Then go to the Feeds and Speeds:



You'd have seen the feedrate and spindle rpm issues right away there. Your CAM program might be able to do it for you too, depending.

The other thought I had is on the tapping fluid. I hate the thought of having to brush it on (though I suppose it isn't so bad).

Seems to me you could find a defined place to put one of those no-spill-if-you-tip-it-over containers and program the machine to dip the tap each time. Might almost be worth it to epoxy some magnets to the container if that makes it easier to set it down, or make some kind of bracket to attach it to your machine's table at a location where the spindle can access it.

Lastly, if you do the math on how much the OP's alternate feedrate was stretching the tap, he would never have noticed that particular issue with a tension/compression holder as it would have had enough travel to compensate.

Cheers,

BW

[Geof]

Of course you can be lazy like me.

Always use 1000 rpm even up to 3/4"-16, although I will admit a Super MiniMill complains a bit at this size, 1000 rpm means your feed calculation is trivial.

Always use coolant, just enrich it to about 15%; I cannot imagine the tedium and wasted time in stopping a machine at every tapped hole on a run with thousands of holes.

We do production on aluminum, leaded steel and hot rolled steel tapping 1/4" and 5/16" and when I am doing tooling I will tap anywhere up to 3/4NF, and have never used anything other than rich coolant.

Another point about speed is that if you go too slow on Haas machines they seem to have difficulty maintaining synchronization; there was a thread about this a year or two back. Also I have found the chip flow seems much smoother at 1000 rpm versus something like 400 rpm for the same tap.

[WOLOG]

I have a VF-5/50 and I tap quite a bit. I use a tension and compression holder for most of the larger size taps. I use Emuge taps more than most. They are more expensive but when you look at the costs leading up the final tapped hole on the part, then the tap becomes cheap. I have also figured out that if you call Emuge tech support before you order a tap, you can't go wrong. I often open the door to squirt a shot of cutting oil on the tap before the hole. That is the way it is. An extra minute or two of cycle time beats the heck out of starting a new part because of a broken tap.

[roundman]

I like Emuge taps (my personal favorite also) also but we hardly use them where I work. They like two fluted taps mostly and believe they will do anything. Now I have used a lot of molly dee for tapping and believe in it but I only use it as a last resort and prefer coolant use always if it works. I have used the spring loaded holders and they are fine also but have had trouble with tapping depth from time to time when I have a close callout on depth. Roll form tapping is my favorite kind of tapping it proves to me there is a merciful God. Good luck.

[makingchips]

This is what I use works great.

From HAAS website.

G84 or G74 Peck Tapping – You can also peck tap into a hole to go deeper (for tough/hard material) if Parameter 57 bit 6, REPT RIG TAP, is set to 1 (On). Then all you would need to do is repeat the tapping cycle at the same XY location, going deeper in the Z axis on each command line. See the following examples.


Example 1:

G90 G54 X1.5 Y-0.5
S450
G43 H01 Z1.0 M08
G84 G99 Z-0.25 R0.1 F22.5
G84 Z-0.5
G84 Z-0.75
G00 Z1. M09
Example 2:

G90 G54 X1.5 Y-0.5
S450
G43 H01 Z1.0 M08
G84 G99 Z-0.25 R0.1 F22.5
X1.5 Y-0.5 Z-0.5
X1.5 Y-0.5 Z-0.75
G00 Z1. M09

Note: On Mill software versions12.09 and above, REPT RIG TAP has been moved from the Parameters to Setting 133. This is now an On/Off setting that is much easier for the user to change.

MC

[subi4ester]

So far today so good but still stopping to oil between holes, running about267 rpm, last part I will try 1000 rpm, seems fast but who am I to question? Let er fly!!!

[Geof]

I hope I don't get egg on my face.

[subi4ester]

ok, didnt get to try 1000 rpm today, last part is put off until tuesday, boss wants to show off machine when customer is there....

thanks for all the infomation everyone put in, lots to learn:cheers:

[swain]

Don't try something new when customer comes....Its sure to mess up!!

Having done a ton of ridgid tapping in the last 11 years on my haas...I can vouch for most of the stuff said here.

First off...I had a problem that most people won't have. For some reason I had paid for ridgid tapping and the factory did not turn it on. The setup man missed it. And It would tap several holes...then break. Didn't take me long to find the code in my manual and turn it on myself.

ER32 collets are fine for tapping...even tho I have a cat 40 machine. I did end up buying tap drivers...the ridgid ones...no float. I only did this for easy set up as I can change tap size ect in 5 seconds.

If you are Blind hole tapping...Spiral flutes are a must. Be careful on the spindle speed tapping. Different materials will draw the chips out in different ways. On the few problem tapping setups I have had in mild steel...my fallback is to tap it at 100 rpm. May be slow...but I have NEVER broke a tap at that speed. And I have tapped up to 1 1/2 threads on a production basis.

One last thing...to answer the setting of your rapid overrides to 50% while tapping that someone mentioned. As soon as the control reads the G84 tap cycle..(or whatever cycle you use) it uses the commanded feedrate and ignores the override. I still try not to do it tho.

I have only stopped machine and added sticky tap oil for very tricky tapping situations. Doing this adds tramp oil to your coolant tank.

My .02 cents...

Good Luck..Good Day

S

[subi4ester]

Don't try something new when customer comes....Its sure to mess up!!

One last thing...to answer the setting of your rapid overrides to 50% while tapping that someone mentioned. As soon as the control reads the G84 tap cycle..(or whatever cycle you use) it uses the commanded feedrate and ignores the override. I still try not to do it tho.

yeah, customer must be stopping by wednesday now, didnt show up today and I went ahead and finished the part. Next run of parts with taped holes I will try some faster speeds.

I guess I was kind of misleading when I stated the 50% thing, I set the feedrate to 50% for the tap in Mastercam and the feed @ 20.***whatever was what the program had calculated. Seems to be working now, I cant override anything during taping cycle at the machine.

[themil]

I am not a programmer but it sounds like your programming is sound. If this machine has solid tapping as an option it should solid tap all day long. It sounds as if you have a problem with servo tunning. If the machine is set up correctly you should have no need for a floatying holder, this defeats the purpose of solid tapping.
I believe you have a problem with the machine not with the operation of it.

[Geof]

I am not a programmer but it sounds like your programming is sound........I believe you have a problem with the machine not with the operation of it.

His programming could be sound but he had the wrong type of tap, a tap drill that was too small and inadequate lubrication; he is also working with a material that is sometimes difficult to tap as the properties vary even within the same length of stock and hard inclusions are not unknown in A36.