true position of threaded holes 3

Technically / theoretically they are correct. As the pitch diameter moves away from MMC then you'd get a bonus tolerance. You have to think about the pitch diameter forming a cylinder with the OD equal to the pitch diameter. There are ways to measure the pitch diameter which could then be compared against the standard for the unified thread form to calculate the bonus, but this sounds impractical.

There are gages that engage with the pitch diameter of the threaded hole to accurately measure the location of the hole (e.g. Flexible Hole Location Gages at Thread Check) instead of the minor diameter for example (which would require you to state MINOR DIA. under the feature control frame) but this has nothing to do with a bonus tolerance.

Bottom line is that I would leave the modifier off the tolerance given its impracticality.

The tip from Prof Don will give the reply, hope this helps.

SeasonLee

SeasonLee,

I looked at the Tec-Ease tip and its not entirely clear how the pitch diameter comes into play. It looks as though the bonus tolerance is applied to the major diameter of the thread. Unless the designation of an M series screw is different from a United thread, the 10mm is the basic dimension of the major diameter. Therefore the 0.3 tolerance was applied to the major diameter to establish the virtual boundary of the thru hole of the gage. I'm not saying this isn't correct or applicable just not abundantly clear (at least to me). This example is also in the context of implementing a functional gage (something that can be cost prohibitive) and even the example acknowledges that determining the bonus tolerance is not easy and the payoff is small (translating to impractical in my opinion).

tk369,

I observe that you have a positional tolerance of Ø.010" on a 3/4-10UNC-2B thread. That is pretty darn accurate. According to my Machinery's Handbook, your pitch diameter is Ø.6927/.6850. Your bonus tolerance is significant, compared to your position.

Do you really need to be this accurate?

If all you are trying to do is pass a screw through a clearance hole, you need a postional tolerance equal to half the hole clearance. If you have a clearance hole of Ø7/8", you need a positional tolerance of Ø.062", and then the MMC does not matter much.

JHG

I have read recommendation to distribute clearance for positional tolerance as 60% for thread hole and 40% to drill hole. Then it will be Ø.062"*0.6=0.0372
For hole with min PD 0.6850 0.1 will apply.
if PD will grow then positional tolerance will grow accordingly and max will be 0.1+(0.6927-0.6850) = 0.1077

The big names in ANSI/ASME interpretation like Genium or Tec-Ease recommend MMC on pitch dia. not because of bonus tolerance, but "to be able to use a functional gage".

There is a flaw in that logic though: When you engage you thread gauge, threads have ability to self-center; and if your fixture has celf-centering device, it is no longer functional gage, but actualy checks / measures RFS.

I am afraid you are on your own. I couldn't find solid argument for either MMC or RFS on threads in years, so good luck to you.

We generally put MMC on threads.

This allows use of inspection tooling, it doesn't force it though. In fact, it doesn't even force you to take advantage of the MMC when you come to do inspection. If the part can me made to tolerance without taking into account additional tolerance from MMC then it doesn't need to be worried about.

I look at it this way, I don't believe putting it on the thread call outs causes any harm. Most of the time it doesn't buy you much though there are a small subset of circumstances where it may be beneficial.

I agree with what ak762 says, especially if tight tolerances are required. While 60/40 is a bit arbitrary the idea of giving more to the threaded feature is sound. Firstly, because there is usually an extra manufacturing (tapping or equiv) step in making a threaded hole V plain so more tol is needed. Secondly, the threaded hole generally doesn't generally get to benefit from MMC as much, if at all.

Also, just plain avoid tight tols on threaded holes. Don't use them for alignment - put other features on the parts such as hole/slot & dowel/roll pins or similar.

Rule of thumb, I try to avoid less than pos dia of around .014/.015 for threaded holes. Depending on the hole size etc. I usually speak to the machinist/shop before going much below .010 dia.

ak762,

A positional tolerance for a tapped hole of half the clearance, accounts for both tolerances. You are proposing to increase the positional tolerance a bit.

.125" x 0.6 = .075"

I am used to specifying small holes. My gut feeling is that it is harder to centre large drills. There is also limited value in very accurately centreing a large hole. Why pay for the effort?

JHG

drawoh, I think the point is that a tapped hole is generally more difficult to position compared to a plain hole, and also that a plain hole can benefit more readily from MMC.

So the argument is to give a little more of the pos tol to the plain hole, instead of 50/50 to both plain and threaded hole.

prdave00

I would like to quote the paragraph from the book below to reply your post.
Page 389 of "Geometric Dimensioning and Tolerancing Allpications and Techniques for use in Design, Manufacturing and Inspection" by James D. Meadows
<<
The question is often asked as to whether the RFS of MMC concept should be employed in threaded holes. When a screw is inserted into a threaded hole, there is some “play” (slop, if you will) during assembly. This slop between the screw and threaded hole is the result of the pitch diameter pf the screw being smaller than the pitch diameter of the threaded holes, and this slop or “play” helps us to more easily assemble the parts. Hence, there is more slop if the class of fit is a 1B instead of a 2B, and even less for a class 3B threaded hole. The larger the pitch diameter of the hole, the more “play” (slop) we derive.

If the “play” is utilized to help us assemble the products, it should be allowed as additional tolerance during the inspection procedure. This is bonus tolerance, and using the MMC concept in the control recognizes that. If you can’t measure the bonus tolerance, the dimensioning and tolerancing engineer can suggest gaging procedures that will automatically accommodate the allowed minimum bonus tolerance available for that hole (for example, functional receiver-type gaging).

If you do not wish to utilize the bonus tolerance because you can’t quantify its exact number of thousandths of an inch or portions of a millimeter, that is your decision. Use of the RFS symbol in the control will negate it in the inspection procedure. Still, for a tolerancing engineer (as merely a describer of physical phenomena) to say it doesn’t exist by putting in an RFS modifier instead of an MMC is not recommended. The RFS symbol implies that the hole contacts to meet the screw size—and that is rarely true.
>>

SeasonLee

SeasonLee,

Point taken and I don't dispute that having the MMC modifier is technically beneficial, but I'll stick by my guns that is not always practical. If tk369 is designing a one-off part and the location and orientation of the threaded hole is not critical, then I'm not sure there would be any benefit to require that the metrology lab calculate the bonus tolerance much less produce a functional gauge. I also don't get the logic that just because its in the FCF, doesn't mean that it has to be taken advantage of. (No offense Kenat) Shouldn't you then just design the clearance hole assuming the modifier won't be applied to the tapped hole during inspection? Or do you just wait until that feature fails inspection and then argue to the inspector that it might have passed if the bonus tolerance was applied? That doesn't sound very proactive or efficient, but maybe I'm way off base here.

I am trying to understand the behaviour of a screw in a maximum sized tapped hole, specified with a maximum position error at MMC.

Take the case that we are inserting the screw through a small, sloppily located hole such that the screw cannot centre in the tapped hole. It must contact one side of the thread in order to pass through the hole.

Take the case that we have worked out a screw torque, based on the standard equation T = CDF, where C is our friction factor. My textbook says this is 0.2 for an unlubricated bolt.

What really happens when you torque that screw down?

My working assumption for tolerancing is that the screw, centred in the tapped hole, must not contact the sides of the clearance hole. If the screw contacts one side of the clearance hole, and the opposite side of the tapped hole, you can still force it down, but you have reduced control over torque, and clamping force.

JHG