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.
Tek-Tips is the largest IT community on the Internet today!
Members share and learn making Tek-Tips Forums the best source of peer-reviewed technical information on the Internet!
-
Congratulations cowski on being selected by the Eng-Tips community for having the most helpful posts in the forums last week. Way to Go!
thread depth measurment 2
- Thread starter morach
- Start date
-
1
- #2
One way to gage the depth of the thread would be to grind
"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
"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
- Thread starter
- #3
We have tried the second method. QC recognizes this as a good method, and uses it, but says "varying chamer depth affects the measurment". We have also ground a screw to as close as our visual inspection can determine to the start of the first full thread. from there "counted" the # of turns on the screw. We are trying to get an ECO through that would change the callout from +/- .005 to a .xxx min thread required. One other method nobody can agree on is to measure the length of our ground screw, the length of the part, and do first grade addition/subtraction to get a depth.
All three methods will work to varying degrees , however
+/- .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.
+/- .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.
The most common method for a blind hole is a minimum full thread (MFT). I see little reason to control a thread depth as long as the fastener does not bottom out. If the part requires a thread depth as an actuation stop or for a stick out requirement for a stud then thread milling may be required. Threaded fastener typically can have up to 2 1/2 thread of imperfect threads and be acceptable and the top of the thread you make can also have this imperfect thread. Your QA department is splitting hairs. If this part is for another customer call him and clarify the callout.
- Thread starter
- #6
This is a "as cost effective as possible" standoff. It measures .375 od x .750 long. one end has a 6-32 thread the other has a 10-32 x .380 deep callout. The sheet thickness is .09 thk 6061-T6. the screw is a 10-32 x 3/8 long. I am beating a dead dog on this one. Until we can agree on one testing method we will continue to fight the same fight every time this part comes up for re-order.
-
1
- #7
Unless I am missing something here it seems like a bit of engineering is needed. My guess (and that is all it is) would be the drawing has some general limit on it say up to .500 +/- 0.005 the inspector looks at that says 3/8 is less than .500 so it has to be +/-0.005 and whilst he or she is correct it doesn’t matter a jot as long as the screw doesn’t bottom out.
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.
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.
- Thread starter
- #8
Thank you all for the input. Ajack1, you are not missing anything. The engineer signs off on the lot because the screw doesn't bottom out. Unfortunately, the inspector makes life hell for the rest of us until the review board dispositions the parts and engineering does sign off. A simple ECO would solve the problem. I was just wondering if there was a more common practice for measuring the depth than what we are doing.
click on the "combi" link ,
An expensive solution if the problem is only your internal inspection.
- Thread starter
- #10
Good Gawd I hate standard tolerances...that and Mech Guys who never browsed a Machinery Handbook or a supply catalog.
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.
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.
After thinking this one over for a little bit, I think you need a new inspector. Stick to your guns on the turn counting method and let the rejected good parts pile up to the ceiling if you have too. This is called "Industry Accepted Practice"...at least in this country. I've been in the business for over 25 years getting work through some really tough inspection departments. I've had undersized threads, oversized threads, no threads, bad threads, torn up threads, wrong threads, and threads not deep enough, but I can't for the life of me recall ever getting rejected for being TOO DEEP by some yahoo who measured a thread depth with a handless thread gage and a depth mic. What this guy is doing is bad for you, bad for the company and bad for your customer. Don't feel bad if you get him fired. There's a lucrative career in the fast food industry waiting for him.
That seems a bit tough BilletGuy. Is it the inspectors job to “guess” if a part is suitable or not or to measure if it is within limit, however stupid it may be?
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?
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?
Well, no, its not the inspector's job to "guess", it's the inspector's job to "know". The point I was trying to make before is that according to The Book, the standard 3 place decimal tolerance on the drawing does not apply to the maximum depth of the thread in the same way the major diameter of a .112-40 UNC 2A isn't .117/.107. Everything I've seen calls it a "minimum" length of engagement. So right about now, the inspector is guessing the parts are bad and he's wrong...according to spec. if he's measuring that depth +/-.005. Besides, just because you have a stupid callout doesn't mean you have to be as dumb as the screw that goes in the hole.
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!
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!
Sorry I still don’t agree, where exactly in the book does it state that +/- 0.005 does not actually mean +/- 0.005?
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.
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.
Here, open up good 'ole Handbook H28, the Federal Spec for screw threads. There's a standard gaging practice section that in my 1969 version starts on page 6.0. Section 5.6 GAGING FUNCTIONAL DEPTH LIMITS OF PRODUCT INTERNAL THREADS. It starts out talking about depth limit steps on gages and states "There are 2 types of specifications refering to the depths of internal threads. One type specifies MINIMUM DEPTH ONLY and therefore requires only one depth limit on the gage. The other type specifies minimum and maximum values for depth of the thread and requires 2 depth limit steps on the gage.
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?
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?
"There are TWO types of specifications referring to the depths of internal threads. One type specifies minimum depth only and therefore requires only one depth limit on the gage. The other type specifies MINIMUM and MAXIMUM values for depth of the thread and requires TWO depth limit steps on the gage.
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.
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.
Here are three thread gage companies that we have done business with. All were quite helpful with several major problems.
- Status
