I don't know what the normal life expectancy is, but I have been told that thread forming taps (with the correct size drill) will last much longer, especially on a blind hole like you have.
we've got a steel part which has got 2 m12 holes in it, the machine is tapping that thread using hss tap, the material is plain carbon steel, the thread needs to be 18mm deep in a blind hole 23mm deep.
what is the "normal" life expectancy of that tap in those conditions on haas vf2?
because ours made about 140 threads and then the spindle load got to 105%.
the tap was working at 60 rpm and 105 mm/min.
Similar Threads:
I don't know what the normal life expectancy is, but I have been told that thread forming taps (with the correct size drill) will last much longer, especially on a blind hole like you have.
There are to many variables to give you a life expectancy on your tap
ie tap material, hss,cobalt
coatingsolished,oxide,tin tic altin
which manufacturer
tension/compression holder,rigid tapping
type of taps hand tap, 2flute spiral point,3flute,high spiral flute tap ect.
material "steel" is it 1018 steel 12L14,4140 ect.
I do agree with brian257 a good form tap would be best do. being a chipless tapping process there would be no chips at the bottom of the hole to deal with
if it is 1018,12L14 most taps would be ok but if it is something like 4140 use a cobalt with tin/tic coating
What coolant and the coolant mixture will play a big part in life expectancy also.
I would just make sure you have a good GO/NOGO guage then you can track when your tap get to dull to produce good threads.
At 60 rpm, the tap will break before you see wear.
Two Haas VF-2's, Haas HA5C, Haas HRT-9, Hardinge CHNC 1, Bother HS-300 Wire EDM, BobCAD V23, BobCAD V28
this is what interests me the most of all the other answers!
I had a hunch that might be it, when looking in the books, the tapping feeds and speeds seem crazy to me, but also, some holes, seem to be better threaded if the speeds are greater, also the spindle load sometimes gives me worries.
spindle load can sometimes be greater with less aggressive speeds, but sometimes they arent.
this is something i can't yet understand, what is the best approach on tapping?
how do you know what can be done what cant?
I've tried using feeds and speeds by the book, once, on aluminium, m6 tap, the result was catastrophic, the tap shattered like glass on first hole.
I am usually using 50-300rpm for aluminium, 30-100rpm for steel (we mostly use plain carbon steel).
the feed depends on pitch, of course.
we are using only hss taps, different type for aluminium (yellow marking) and differnt for steel (blue or green), but it is all hss, for blind holes these:
http://img.directindustry.com/images...60-3155569.jpg
and for through holes these:
http://img.directindustry.com/images...02-9074550.jpg
so I'd like to know what would the correct feeds and speeds be for lets say m12, m6, m4, etc?
I doubt the manufacturers feeds and speeds, they seem awfully too agressive, yet mine seem too weak.
how do you determine yours?
rpm's can be dictated by your vmc
we have a haas vf2ss(2011) and okuma mc v4020 that i would start rigid tapping at around 50ipm and calculate the rpm's from there ie: an 8-32 rpm would be1600 rpm at 50 ipm (similar to an m4)
the 1998 vf2 the tapping is always between 300- 500 rpm due to the way the cnc handles the rigid tapping
the haas vf2ss and the okuma both are direct dive and read the rpms internally where as the vf2 has an encoder to read it and it takes longer to wind down and reverse the spindle so the lower rpm's are better for the machine
there are also tension/compression holders that would help if there is error between spindle reversal and z axis travel
rpm can make a great deal of difference at what you see on the load meter
geared heads swap to the low range and have an improved torque (lower load seen on the front panel)
direct drive motors generally do better at a higher rpm range than being very low (most lathes that i owned did not have there best torque until it got to about 400 rpm) same should apply to mills--newer mills swap the winding to get better torque at low range
for tapping blind holes i would start with something like this
cobalt substrate tin coated or ticn to increase hardness and lubricity
use a good brand ( walter is good)
rigid tap vf2ss or okuma mc v4020
m12x1.5
aluminum start at 1200 rpm
crs steel start at 500 rpm
adjust up or down depending on how it cuts
Brand:
Guhring
MSC Part #:
58540832
Mfr Part #:
9039750120070
3975
ok, ive looked at the rpm/power/torque curve for vf series mills, it looks like the peak torque is at about 2300rpm, does that tell me that I should work towards maximum torque when tapping?
we dont have cobalt taps, we have hss, coated or uncoated taps, they are pretty weak, I think, because you can easily break one if youre hand tapping an unfinished hole, especially small ones like m3, m4, m5, m6, larger ones are harder to break, but not impossible.
so those rpms you've mentioned give me the creeps.
like I said, I tried only once the by the book value and it exploded on first hole.
the point is, I want to know what makes a tap break?
why does a higher rpm not break the tap and smaller does?
I'd like to know the logic and science behind it to understand better how to achieve maximum life expectancy and least grief when tapping as it is hard to fix broken tap inside a hole, whether its blind or not.
Several points that I have made over and over in these threads:
1. Speed equals strength. To a point, the faster you turn the tap the stronger it is. Turning a tap very slow makes it break more easily all givens equal. I tap everything up to 1/2 inch at at least 1000 rpm. Think of a piece of straw that can be thrust through a tree at tornado speeds!
2. Most people use the wrong size hole for the tap they are using. The tap-drill charts that you will see everywhere are for no more than 1 to 1 1/2 the tap diameter. In other words a 1/4-20 tap call for a #7 drill, but that is only for a maximum of .375" deep. Machinery's Handbook will show the proper or acceptable hole size for different depths. For example and 1/4-20 at three times depth or .75" can be as large as .210" and it is still class 2b. That .009" difference in hole size is pure gold for saving taps and parts from getting destroyed. A .207" hole is good or (acceptable as class 2b) even for a hole that is only .083" deep or thick. You can check your Handbook by going to the "Recommended Hole Size Limits Before Tapping Unified Threads" chart. All of the charts for holes size were developed many decades ago when drills were not that accurate and drilled oversize holes. For example a .201" drill might drill a .204" or .205" hole. Now a days most drills drill pretty much at the size they call out.
3. I can't find the article right now, but studies were done showing that most threads in manufacturing are at too tight a tolerance and may be detrimental to their proper use. The majority of the time, 50% is all that is required. No matter how many threads you are into something, only the first 5 threads actually hold. After that, only if they fail do the others engage.
4. Fine threads are stronger than course threads, but take longer to install and take out and are more delicate in handling. That is why most used are course.
I had an engineer tell me once that threads and threading is the most misunderstood thing in machining.
Increase your hole size, increase your tap speed and keep the coolant flowing. Have fun.
Mike
Two Haas VF-2's, Haas HA5C, Haas HRT-9, Hardinge CHNC 1, Bother HS-300 Wire EDM, BobCAD V23, BobCAD V28
You're completely correct about this (there's only a handful of people that post about it from time to time, haha) but there's one small exception. In order to obtain the correct class of fit with different thread depths, the determining factor is the screw or fastener itself, whether it's actually installed that deep. It's a minor thing but people have pointed it out to me before, in cases where I took advantage of the deep thread then parts were rejected because the customer only planned to install the screw like 4 turns deep despite the print being specified deeper. So in that particular case there's conflicting information because the machining print was made without regard to the actual assembly in reality, and the designer was to blame...but the machinist takes the heat.
I think for most job shops that isn't a problem that would pop up too often, I mean you can't be second-guessing whether the screw will actually be installed that deep every time you get a print that has a threaded hole or two, but it's just something to keep in mind. If the person that made the print isn't aware of how the class is determined, there could be a mixup.
Technically speaking the machinist would be in the right, because the print holds specifications that are legally binding. but it still could sour a relationship when the customer is confronted with the fact that their engineer/designer screwed something up that cost real money...
That's for sure!
I used to do some parts for Boeing a long time ago. I even found mistakes on their prints. But, one thing I liked about machineing their parts was that if it had to be a tight tollerence they would ask that it be so, but if it was not critical they might make it plus or minus and 1/8". They understood that tolerance cost money and they wanted their money spent where it needed to be.
I still get customers who want sheet metal hole sizes on 1 1/2" deep threaded holes. That is just asking for broken taps. The reason is laziness and or ignorance in understanding tolerances and machining.
By the way, if the customer asks for 1" of thread depth and only plan on using 4 threads, that is a big error on their part. If I run into to these, I will often tell them about it. Did some recent parts recently where they wanted nearly 2" of 1/2-13 threads with a sheet metal hole size and I just told them what hole size I would use and that was it, 7/16". If they don't want that I don't make their parts. Too much material and time wasted if just one tap breaks. When I supply the big chunks of material and the holes come at the end, I'll just turn it down. Or, if they really want to insist, I'll just double or triple the price and then they can decide.
Cheers---Mike
Two Haas VF-2's, Haas HA5C, Haas HRT-9, Hardinge CHNC 1, Bother HS-300 Wire EDM, BobCAD V23, BobCAD V28
cant you just use smaller size end mill to get the broken tap out of the way and fix the part?
even if its necessary to weld the hole afterwards, redrill it and retap it?