LinkBack URL
About LinkBacks
You want to use 3 Flute Spiral Flute Taps. They draw the Chip Out of the Bore. Use Tap Magic or MollyDEE Tapping fluid.
If at all possible try to drill the hole a little bigger. You just have to watch your tolerances.
| | |
Hey,
So I was having massive tap breaking problems trying to Rigid Tap Steel that was Rockwell C 53. I'm using a Haas TL-1 and drilled a through hole with a Solid Carbide #41 Drill. At first I learned how holding a tap in an ER-16 collet is unacceptable because the taps wobbled immensely. I decided to use my drill chuck to hold the tap more true. I was also making sure to apply thread cutting oil before tapping.
The problem I was having when running the program the taps kept breaking. Surpsingly Geuhring HSS taps with a Green Band performed the best, actually they were the only taps that even did the job once. Even odder was that I was holding them with an ER-16 collet before realizing the taps weren't running true. My Solid Carbide taps all broke. I was using modified bottoming style taps.
I tried spindle speeds of 120, 60 and 40 RPM with feeds of 3, 1.5 and 1 respectively. None of this worked I just continued to break expensive taps. Does anyone have advice for tapping in steel that is this hard with such small taps? Is there something I'm missing? Any and all advice on rigid tapping is welcome. I'm a young machinist so I'm always looking for general and specific advice.
-JWB
--We Ain't Building Pianos (TCNJ Baja 2008)
You want to use 3 Flute Spiral Flute Taps. They draw the Chip Out of the Bore. Use Tap Magic or MollyDEE Tapping fluid.
If at all possible try to drill the hole a little bigger. You just have to watch your tolerances.
Toby D.
"Imagination and Memory are but one thing, but for divers considerations have divers names"
Schwarzwald
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
www.refractotech.com
you could probably open the hole up a little as Toby had meantioned , if you look in the machinist handbook you will be able to find the max drill size , the tolerancing will be specified by the class of thread and the effective thread depth
tapping oil is a must , I've always liked the Spar-tap oil
A poet knows no boundary yet he is bound to the boundaries of ones own mind !! ........
http://microcarve.microcarve.biz/
Open the hole up as big as possible. Use 60% -65% threads (you could go even lower down to 55%), they will still have all the needed strength. The #41 drill puts you in this range. Reference the Machinery's Handbook, they have a good section about threads and tapping.
If possible go with thread milling. This is a valuable tool, it can save time as well as costs. I'm not saying it's the end all be all, but it is a tool to be used when appropriate. I thread mill a #4-40 blind hole in 440C stainless. It works great and is faster than a conventional tap. I can adjust the hole to be .0005 oversize to compensate for shrinkage from hardening (we are milling annealed then heat treating).
If you need to tap, find a tap recommended for hard tapping, 53 HRC is pretty hard for tapping. I think a spiral point would be better, they push the chips ahead and out thru the hole. A bottoming tap pulls the chips up out of the hole, which is a harder operation. I would shut off the flood coolant and use a fluid in the hole & on the tap. Use an oil, people here have suggested a few.
If your tap slips then it will not be in sychronization with the down-feed, we use tap collets with a square hole in them. They seem to hold better, the square keeps them from slipping.
Good luck!
Still working in the "D".
did you try a form tap?
Using a Roll Tap might cause more problems in Hardened Materials. Rc53Originally Posted by 1234567
Toby D.
"Imagination and Memory are but one thing, but for divers considerations have divers names"
Schwarzwald
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
www.refractotech.com
I suspect that you are using the ER collet incorrectly. Snap the collet into the nut before you put the tap into the collet. The nut has an eccentric clip which engages the slot in the collet. If you put the tool into the collet first, the collet will never clip properly into the nut, and the clip eccentric will force the collet off center. Also, there will be considerable difficulty removing the collet from the holder, and great danger of cracking the female taper.
If your toolholders have already been abused, it is possible that the female taper is already cracked and this could lead to runout.
I have no real advice for tapping something that hard with HSS taps. There is not enough differential between the hardness of the tap and the hardness of the material. Maybe a powdered metal tap might be obtainable with a bit more hardness. I can imagine the potential crunch of a solid carbide tap cutting full form. I wonder if anyone makes a set of carbide serial taps: taps with truncated crest, each one in the set being a bit less truncated than the previous one. I imagine these would be done in bottoming style because you want to lessen the cutting engagement length.
First you get good, then you get fast. Then grouchiness sets in.
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Are you tapping blind or through holes? I have gained a lot of admiration for "peck" tapping with a 3 or 4 flute gun tap. If your controller can handle peck tapping, simply add a "Q.### (depth of peck) value after the G84. Gun tapping a blind hole might be a little risky if you don't have adequate extra depth to allow the chips to easily compact . I also use a sulphur based tapping paste called Fucs Renocut SC tap cmpd. The stuff is awesome for hard alloys. I've tapped 600 brinell hardened irons with this paste, and a carbide tap! Good luck,
Rich K.
Posting Permissions
| | |
