Rigid tapping recommendations

[Hy D. Tran]

Aluminum (I won't allow my students to do anything but machinable wax or aluminum on our CNC), say 1/4-20. On machinable wax, the rigid tapping cycle works beautifully with a #7 drill & 1/4-20 tap, set at 100 rpm. When I do it on aluminum, it's BANG instant broken tap.

 

Someone recommended that I use a slightly larger drill (e.g. #5 rather than #7). Any other hints? Any recommendations (specific brands/models would be great) for taps, & settings for the rigid tapping cycle (e.g. rpm, clearance planes, etc.?)

 

Thanks!

[cadcam]

Are you doing a cutting tap or a roll tap?

What feed are you useing for that feed are you letting the mc do it for you or are you setting a feed.

 

Waht is the Machine and what are you using for a holder?

[MACHINEMASTERG]

your feed has to sinc with your rpm ex... 200 rpm is 10.ipm for a 1/4-20 ...320rpm is 10.ipm for a 10-32 etc...etc...hth

[rchoward]

is your machine parameter set for rigid tapping

 

does your machine have rigid tapping

 

if not the thread may look okay in plastic but in alum it will break because it is not really working to sinc up especially at 100 rpm it would be hard to tell

[Jack Mitchell]

Hy D. Tran,

quote:

---

(I won't allow my students to do anything but machinable wax or aluminum on our CNC)

---

Personally, I WILL NOT allow my students to cut machinable wax, wood, or aluminum; when taps are broken in real materials I have only my knowledge and this forum to resort to; feeds, speeds, and the like are not much concern to me - what is a concern is your choice of materials and the implied education from such.

 

Machinable wax with a ¼-20 (5000 ~ 10000 rpm.)

Aluminum with a ¼-20 (1000 ~ 3000 rpm.) – It all depends on how bad your attitude is on any given day; don’t ya know?

My personal best was only capped by the maximum rpm of 6000 on a 4-40tap in hard plastic – this was so effortless that I am embarrassed to say that I did it.

 

I do not dislike you per say – I have a very large problem with professors that hand off such professionalism in toy materials (I am also a professor with an attitude and the real trade experience) Admittedly, I have a problem with such questions as these.

 

The rpm is so grossly under-revved that I cannot render a professional response to the original question.

 

Regards, Jack

[Guest CNC Apps Guy 1]

As a Mastercam Instructor for nearly 3 years and a Machinist for over 10, my experience has always been "real world is best". It is taken more seriously by the student, and can be appied easier in real life.

 

If you're having a problem with taps breaking and you're using the correct size drill, and the post is outputting the correct feeds/speeds, then I would look at the tool holder. Are you rigid tapping with a tension and compression holder or vise versa?

[Trevor Bailey]

You may also want to look at the type of tap you are using. More specifically, one that pulls the chips out or one that pushes the chips to the bottom. If using one that pushes chips to the bottom of the hole, you may simply be threading too deep to the "shoulder" depth of the hole. You may aalso want to make your cutting fluid a little richer.

 

Above all though, make sure that you are also checking the hole size, teeth chipped on tap, good spindle, etc...

[Reece L Gibson]

Mr. Tran if you are using the Rigid tap function,program the depth say .1 thou shy and run the tool.

Look at the bottom of the hole(if it is a blind hole)and it will tell you the story of packed chips or hitting the bottom of the drilled hole.From there you can change the depth in the program and re-run the tool. This will show two things, one: is how the rigid tap cycle works, and two: how not to break off taps in parts. If it does not make it to stage, you probably have incorrect information in the tapping cycle.Check your programming mannual for correct format.

[Saultspics]

We tap 1/4-20 drilled with #7 all the time in aluminum on our cnc. We use taps that the chips come up out of the hole.

 

Stephen

[Hy D. Tran]

CNC is a Fadal with rigid tapping cycle. I tell MasterCam to use rigid tapping, & let it calculate feed rates from speeds. Standard toolholders, no tension/compression or tapmatic.

 

Cutting tap, not roll-forming.

 

Don't have the budget to let (too many) things break, which is why I'm sticking to wax & aluminum. Didn't mean to try to project an attitude, just don't have the money.

 

Thanks for the suggestion to find taps that suck chips up. Will try that next. Don't quite have the guts to try 1000 rpm (or 6114 rpm for 400 sfm!) This is not so much a MasterCam issue, but a machining issue where I have no experience. (Our machine shop people are all conventional, so I'm sort of swimming on my own). The G-codes put out by MasterCam look very much like the canned cycle in the Fadal.

[Trevor Bailey]

Some brands of taps are really crappy to say the least. You may want to slow all feeds/feeds down along with getting a tap that pulls threads up. To do this in MC, in the parameters section when selecting a tool and MC gives the RPM, type a "/" right behind the RPM given and then give and amount to divide by. By doing this, the feed should automatically update the feed also.

 

Just another suggestion.

[Noel]

Hy IS YOUR POST OUTPUTING AS A G84.1 OR AS A G84

THE LINE SHOULD READ AS FOLLOWS G84.1G98Z-.55R0.4S100.F5.0

YOU COULD ALSO TRY SETTING THE R VALUE TO .4 TO GIVE THE MACHINE NTIME TO ACCELERATE IN TO THE CUT.I USUALY DRILL #5(.2055") FOR 1/4-20 AND TAP WITH A GREENFIELD EM-TI 3FLUTE LEFT SPIRAL RIGHT CUT TAP. hOPE THIS HELPS

 

NOEL

[jeff]

We have an Okuma MX-55VB and we are tapping a 5/16-18 tap,standard Morse 2 flute spiral point at 2100 RPM in 1018 steel.

Only because the machine won't allow me to go faster.

[Philcott]

Hi Hy,

 

When ordering spiral taps be aware that spiral flute taps pull the chips up and out of the hole where as spiral point taps push the chips into the hole. Therefore use spiral flute taps for blind holes and spiral point taps for through holes. Better yet, for aluminum, use form taps as stated above, but beware you CAN NOT use the same tap drill size. Drill size for 65% thread on a 1/4-20 would be a number 1 (.228 dia) wire size drill.

 

Phil

[peturk]

Another possibility.

 

If you're using rigid tapping with no radial float in your holder and you aren't careful about spotting and drilling the hole, then you can break the tap because it is not concentric with the hole.

 

The most critical part of the tapping cycle occurs when the tap reverses direction. If your machine does not reverse quickly enough, perhaps because of it's capabilities, especially in gummy material like Al-6061, you can experience problems. That is one advantage of using a "tapmatic".

[out2thow]

The type of tap is very important, and make sure you stick to the uses, ie: Hand tap (4 flute) for hand tapping only, Spiral flute (blind holes) spiral point(2 or 3 flute) for thru holes only.

 

Also be aware of the speeds that you are trying to ridgid tap at, i've seen many break because it was too fast for the machine to synchronize, buy yourself a floating holder. Be sure to use a nice round number for feed like 5,10,15,20,25 etc and multiply it by the #tpi to get the RPM.

 

One other thing worth mentioning is the machine, you wouldn't happen to be using a newer HAAS machine would you?

 

I have noticed by default they will reverse the tap and extract it 4x faster than going in.

 

To correct this use J1 (J2=2x J3=3x....up to 9x)

G84 Z-.75 R.1 F10.0 J1 (no decimal - i think)

this will retract the tap at same rate going in, i dunno why HAAS has done this....perhaps to get kick backs from tool manufacturers for a increase in tap sales?? You can also change this in the settings screen, can't remember the setting number though, something about ridgid tapping retract speed.

 

Hope this helps

 

out2thow

 

[ 05-31-2003, 08:02 PM: Message edited by: out2thow ]

[Hy D. Tran]

Thanks for all the helpful hints.

 

I went & bought new taps (local DoAll sales folks suggested OSG/Ossner spiral flute taps; cost a bit under $8/ea).

 

That fixed the problem. I'm up to 1000 rpm in aluminum now.

 

By the way, the post processor does generate a G84.1 line.