thread depth measurment
thread depth measurment
(OP)
I am trying to determine the most commonly accepted way of measuring the depth of a threaded blind hole. The drilled hole is plenty deep to go past what is needed, but our QC is rejecting based on their method of measuring the threaded portion depth. Any ideas would be appreciated.





RE: thread depth measurment
"whistle" notches for a "go" depth and a "nogo" depth on a thread plug gage.
Another down and dirty way is to count gage rotation until the gage bottoms out. turns X pitch of threads = depth
RE: thread depth measurment
RE: thread depth measurment
+/- .005 on a thread depth seems kind of tight to me.
The only way I can think of holding +/- .005 would be to thread mill them.
As to the varying chamfer depths , what up with that?
Are these parts being made on a drill press ?
You may have to control the chamfer depth and dia and have them agree to check the depth of the thread from the bottom of the chamfer if thats at all possible.
Good luck
My company sometimes makes what would seem the easiest things to do difficult as well.
RE: thread depth measurment
RE: thread depth measurment
RE: thread depth measurment
Is there any way to get the different parties together to find out the REAL needs and function of the parts? It seems that could save a lot of money for the company and headaches for the employees.
RE: thread depth measurment
RE: thread depth measurment
click on the "combi" link ,
An expensive solution if the problem is only your internal inspection.
RE: thread depth measurment
RE: thread depth measurment
DO NOT BUY THAT GAGE!!!!!
They work too good and they don't apply to a standard callout. You'll be beating your head against a brick wall for the rest of your life trying to machine every single thread in the shop to +/- .005 because they'll buy one for everything...and REJECT GOOD PARTS!!!!
ANSI/ASME B1.2 (get a copy of ASME B1.1) recommends that the length of the go gage should approximate the length of engagement. In other words, grind a gage to depth, if the thread is fully engaged, it is good. The spec says that the depth of engagement callout applies to the MAXIMUM MATERIAL CONDITION...i.e. when the thread and drilled hole are at their smallest and the pitch at its tightest. In all other cases, i.e. REALITY, one must take into consideration variations from MMC and the pitch tolerance of the thread. ASK THE INSPECTOR TO TELL YOU WHAT THE ACTUAL TOLERANCE ON ***THIS*** THREAD IS (pointing at one he doesn't like. By this time he should be bleeding from the ears. If he can't answer the question, he has to back off and accept the ground gage method.
RE: thread depth measurment
RE: thread depth measurment
RE: thread depth measurment
Someone higher up the food chain should take the flak for this IMO, how can a problem like this be allowed to continue when a simple tolerance change would solve all the problems?
RE: thread depth measurment
I agree, by all means, kick it up the food chain, but if this is an old job that somebody else made without a problem for the last 10 years you're gonna look as dumb as a pole trying to explain why YOU can't hold tolerance. And if you're trying to get a customer to issue ECN's on every drawing Joe Blow in engineering pegged to +/-.005 since he started with the company in 1975, Good Luck!
RE: thread depth measurment
Should he start “guessing” what tolerances should be or mean on all parts, right up to the point products start failing because something he thought didn’t matter actually does?
For all we know this maybe his way of raising the issue, I am sure we have all been told to do things we see as dumb despite questioning them with the relevant people. As I see it the parts are not correct to drawing and as such should be failed.
RE: thread depth measurment
I don't have the ANSI on dwg interpretation within arms reach, but the source inspector here says the default is Minimum Depth.
Here it is straight out of Large Unamed Aerospace OEM Design Manufacturing Standard.
Section blah.blah.blah
The length of thread dimensioned on the drawing shall be occupied by fully formed threads. Unless otherwise specified, the length of external threads and the depth of internal threads indicated by untoleranced dimensions is to be considered MINIMUM.
Doesn't get any clearer. Get an extra turn on that gage and she'll fly. Ship it Paco.
Do any of your customers have a Manufacturing Standard?
RE: thread depth measurment
UNLESS OTHERWISE SECIFIED, the length of external threads and the depth of internal threads indicated by untoleranced dimensions is to be considered minimum.
Bilettguy you are correct it doesn’t get any clearer, if a +/- limit is specified then that is what applies and as the parts fail because of this the inspector is absolutely correct to fail them.
RE: thread depth measurment
http://www.hemcogages.com/index.htm
http://www.lionprecision.com/thread/tsf.html
http://www.threadcheck.com/
RE: thread depth measurment
RE: thread depth measurment
As above the inspector is absolutely correct to reject the parts.
RE: thread depth measurment
You may be technically correct, however do you really think the engineer or the draftsman who created this part design actually did a tolerance study and determined that the tolerance must be +/-.005 on the thread depth? What if the part has a thread .001 too deep does your gage tolerance catch the difference. No because first a thread gage is a combination gage covering thread form, pitch diameter, helix angle, and straightness. Secondly a thread gage is made to low limit of a thread PD which I could prove would allow a thread on high limit to be gaged incorrectly just because of the clearance on the threads. How are you going to provide gage repeatability/accuracy. The old 10 to 1 rule applies so is you depth control capable of +/-.0005 accuracy and repeatability? I would also guess the amount of torque applied to the gage would also provide error in reading the depth. I would also contend the gage itself will act as a tap if reseated multiple times in the same hole increasing thread depth with each gaging.
RE: thread depth measurment
Having said that I seriously doubt any true engineer or draftsperson would put a +/- .005 dimension on the depth of a thread, as it is near impossible to achieve or measure.
Again only my opinion but the solution to the problem is to get the drawing changed not buy some expensive gauges that would only prove that the tolerance is stupid, as stated in my original post.
This seems to be a growing problem at least in the UK that we are forced to chase stupid tolerances because no one can find an engineer that will sign off a change, surely the solution to all this should be no more than a phone call and or email?
Even worse than any of this is the attitude that I have a problem I cannot solve so I will fire the inspector who fails the parts given above.
People question why work is sent to the Far East and engineering is struggling in the USA and Europe, this is a perfect example we are handing it them on a plate.