Results 1 to 20 of 46
Thread: measuring threads accurately
02-18-2012, 08:55 AM #1
measuring threads accurately
Hi Guys , What do all you recommend as a good way of accurately mesuring threads internal and external ? we currently use ring/plug gauges for some external/internal threads but this is proving expensive buying these for low volume runs .
We have for instance now a job to do an internal thread M56x1.5 Pitch and it has to be right , have any of you used thread wires and what are your thoughts ??
02-18-2012, 09:44 AM #2
Hertz liked this post
02-18-2012, 09:48 AM #3
02-18-2012, 09:58 AM #4
havent a clue on turning , only been doing it few months been cnc milling for 15 years . not very helpful guys
02-18-2012, 10:10 AM #5
I can't help with your question , but I think the problem here is that you mentioned internal threads and thread wires , wires are for external threads .
02-18-2012, 10:11 AM #6
02-18-2012, 10:13 AM #7
Thread wires are pretty much the last word for thread measurements, but you need good wires and you need to know the wire diameter accurately. The cheap import sets you see around now are worthless for fine threads. Wires don't help you for internal threads, and IMO these are best dealt with using plugs. If you get good at measuring external threads you can usually get by making your own plugs, but for serious high paying work it's best to buy 'em.
You can also do a pretty good job if you have an optical comparator. There are tricks you have to do if the helix angle is large, but that's not usually a problem. If your process is running consistently you can section an internally threaded part, lap the surface and look at that too.
02-18-2012, 10:38 AM #8
Bobw liked this post
02-18-2012, 11:14 AM #9
Get a high quality (recommend sandvik) full profile insert. Bore the hole out to about 0.1mm under the min. minor diameter of the internal thread, then start threading. Carefully increase the thread size until you hit the mean minor diameter.
We are ISO 9001 assured, and our QA system does not bind us to any particular method of gauging threads. I use wires on external threads and this method on internal. Occasionally I will make a plug gauge if it's an unusual thread, but for standard metric and UN threads you really can't go wrong this way.
02-18-2012, 11:26 AM #10
Gagemaker, which is the link litlrob put up. Basically they are a mic that you set up like a bore gage. We have a couple each of the id and od units and have had a lot of success with them.
02-18-2012, 11:40 AM #11
how do you know when your at the mean minor dia ?
02-18-2012, 12:00 PM #12
Only problem with wires is they dont measure the thread profile (eg 60deg) or the pitch of the thread.
02-18-2012, 01:04 PM #13
My answer to this question is to use thread micrometers for OD threads, combined with thread rings whenever possible, thread plug gages for ID threads.
Measuring threads is no simple task. Look at some of the contraptions that have been invented to measure them, and their expense.
A thread is one half of a simple machine. 3/4"-16 UNF-2A, for example, has a pitch diameter tolerance range from .7049 to .7094", for a total tolerance of .0045". Not that bad, until you consider that this is a measurement from gage line to gage line, half way down a tapered groove which is helical, perpendicular to the axis of measurement. Basically that means the pitch diameter is only one of the important aspects of a thread, and it isn't a straight-forward measurement.
Above, I recommended the use of thread micrometers. In my use, a thread micrometer will measure a thread pitch diameter +/- .0005". I would not trust it to accept or reject threads measured within .001" of min or max. Therefore, the 3/4-16 thread pitch diameter mentioned has to be maintained +/- .0013" in order to run parts without a thread gage, and I would get very uncomfortable making more than a few dozen parts like this even on a good machine.
This attitude is a compromise between doing it right, and doing it with what you've got. Doing it right entails meeting you contract obligations as specified by the purchase order and the engineering drawing, which either specifies or infers a particular thread standard like ISO 68. In actual practice, when you've got thousands of dollars on the line, a $250 set of thread gages which are calibrated by a good accredited lab which uses thread master gages to check and set your thread gages, is a necessary and practical choice.
So far I've only been talking about external threads. Measuring internal threads by any other means than hard gaging (thread plugs) is a tough choice to make. It's no problem to own and maintain thread plugs for common hardware sizes such as M8x1.25, #6-32, 3/4"-16, etc. When such a thread as M56x1.5 is specified, you're talking around $600 for a pair of thread plugs, with a couple of weeks lead time. If the quantity of these parts is low, you're really up against a wall.
In practice, good craftsmanship would tend to suggest that the machinist makes his own thread plugs on a lathe, for this job. Even a single thread plug gage can be a good asset here, sized to the mean of the mating thread's pitch diameter tolerance.
A machinist would make this thread plug and then monitor the product's thread using the feel of senses that come from experience making good threads. The machinist is not going to have good sense in making good threads unless he or she has spent a great deal of time in the company of genuine, calibrated hard gages and thread mics and thread wires.
Another good approach, in gageless situations of making such a thread as M56x1.5, is to obtain a mating part from the customer. There's no shame in asking for this, especially if you can explain to the customer that such a thread costs $600 minimum for hard gages, and that not everyone is as scrupulous in producing high quality threads as you are, and perhaps the mating external thread is close to tolerances itself.
You've seen this in your experience, because you are a bad-ass at measuring threads. And that is the moral of the story. Measuring threads isn't as straight-forward as you might think, and hitting tolerances requires a bit of study and a wealth of experience.
02-18-2012, 01:18 PM #14
Look at a table of thread specs for internal thread limits. The minor diameter is specified. Basically this is the size that you would drill in a smaller thread before tapping. Gregor suggested using a full profile insert in a lathe, which cuts from root to crest in the final passes.
Let's say M56x1.5 would be bored to 54.5mm diameter. Bore it to 54.4 mm. Start threading it with a healthy offset to the small size, start increasing diameter, and eventually the minor diameter will start to increase. The full-profile of the threading insert is producing the crest as well, so it's logical to assume that when the crests (minor diameter) is in tolerance, so is the pitch diameter.
Doing it this way means having the correct full-profile threading insert, the correct angular seat, in many instances, good tooling, and good craftsmanship.
How many turns of thread deep are you making? What material? What machine? How many pieces?
And what are you planning to do? Just curious.
02-18-2012, 01:26 PM #15
apestate , thanks for such a in depth and informative reply , thats great im gonna ring the customer for mating part now . and will order a range of thread wires for myself for external threads as at the moment i have nothing .
I know my knowledge of all this is limted by by asking thats how we learn
02-18-2012, 01:39 PM #16
hi apestate , im just making some large thin special lock nuts they are 8.5mm long with an od of 65mm with flats around the od just like a nut , which i plan to machine using the C axis on our cnc lathe , the qty is 80 and the material is 817M40T (EN24T)
thanks for your interest
02-18-2012, 01:45 PM #17
I like the idea of using a full profile insert and checking the minor dia. but this is putting a lot of faith in the insert profile which has it's own manufacturing tolerances and errors.
The bigger problem here is making sure the insert and holder is square to the world within a few tenths.
When making and measuring these inserts you quickly realize that a very small amount of cock in alignment throws the minor cutting edge way out.
If making lots and lots of small run different sizes I would think about investing in a Mits Contracer but they are expensive, slow and you still have to accurately check the minor.
The attachments built by member Gordon B. Clarke would do a decent job on a budget and be accurate enough for most. Flexible Measuring Systems
02-18-2012, 02:30 PM #18
Have you been able to find the proper specs for this thread? That's not easy, either. Back when I was tooling up, I had Excel calculate out any theoretical thread with tolerances, but I wasn't completely sure about the class tolerances because I didn't have the actual international standard in hand in order to figure it out. Maybe someone else can post the tolerances for M56x1.5 internal?
02-18-2012, 02:38 PM #19
Turningboy, here are the sizes for a M56x1.5-6H:
Min. minor: 54.376
Mean minor: 54.526
Max. minor: 54.676
So, bore out to 54.2 or thereabouts, drop the wear offset -.2 for your threading bar and start threading. Repeat the threading cycle, adjusting your wear offset as you go, until the inside diameter of the thread measures about the 54.526 that you're aiming for.
Remember that this will not work with a partial profile insert, it has to be a 1.5mm full profile.
817M40T makes for lovely shiny threads
02-18-2012, 03:06 PM #20