brain freeze on positional calculation 3

[joebk]

I must be losing my mind, this should be straight forward.

Here is an outline of the situation...

Customer has supplied us with the following:

1) their part drawing indicates 4 tapped holes with positional tolerance (at MMC) of 0.3 mm (T2)
2) fastener MMC (i.e. max) diameter = 9.525 mm (F)
3) clearance MMC (i.e. min) hole size = 9.58 mm (H)

I am attempting to calculate the positional tolerance available for the corresponding hole pattern on our part according to section B4 in ASME Y14.5-1994. Equation is as follows...

H = F + T1 + T2

so, using data from above

9.58 = 9.525 + T1 + 0.3
9.58 = 9.825 + T1

solving for T1

T1 = 9.58 - 9.825 = -0.245 mm

If I understand correctly, the relatively tight clearance between the fastener (F) and hole (H) and the positional tolerance (T2) of the tapped hole can result in interference at MMC. So something needs to change in the design i.e. larger clearance hole for the fastener (gonna have to convince the customer).

Please note that I do have calculations that take into account out of squareness of the tapped hole. I did not include these in this post for the sake of simplicity.

Am I doing this incorrectly?

Thanks for your help on so simple a question.

 

[GDTGUY]

It looks like you did your calculation correctly. This is a typical fixed fastener application. Another way to look at it is the total tolerance budget that is available for the parts based on the specified hole/fastener sizes stated.

T(total) = H - F

T(total) = 9.58 - 9.525

T(total) = 0.055 total tolerance that can be split between the two parts.

Since your customer has already stated that they will use 0.3 on their tapped holes, your tolerance budget has been busted big time. Your only means of recovery is to either request them to reduce their tolerance to a percentage of the total tolerance budget, or to start opening your hole size MMC to accommodate the virtual condition size of the tapped holes.

Note that the ASME Y14.5M-1994, B4 calculations assume a projected tolerance has been applied to the tapped holes. If the tolerance is not applied as a projected zone, you will also need to take in to account the possible out-of-squarness condition for the tapped holes.

GDT_GUY

 

[drawoh]

joebk,

What is the point of applying MMC to a tapped hole? Tapped holes centre the part.

MMC makes perfect sense for a clearance hole.

MMC for the tapped hole is meaningless, so let's ignore it.

You have a 9.525mm diameter fastener whose centre is located somewhere inside a 0.3mm diamter. This means your fastener can occupy any part of a 9.83mm diameter located exactly at nominal. You must clear this.

Your clearance hole of 9.58mm diameter cannot be guaranteed to work.

A 9.84mm diameter hole located exactly at nominal will work. If you make your hole larger than 9.84mm, you can allow some positional error.

10.5/9.9mm dia, located to a positional tolerance of zero at MMC.

The squareness of your tapped hole should not matter unless you are clamping a thick plate.

 

[joebk]

I am not totally sure what was intended by MMC on the tapped hole. I ignored it just as you stated drawoh.

I guess I should have included the calculation including provisions for out of square. If I factor in the thickness of the plate (P=4.5 mm max) and the min depth of engagement (D=12.7 mm min) I calculate the following for the min hole size (assuming zero positional tolerance with MMC).

H=F+T1+T2(1+(2P/D))
H=9.525+0+0.3(1+((2X4.5)/12.7))
H=10.04

The thickness of the part seems to be significant in this case (unless I have totally screwed up the calculation?).

Thanks for all of your help!!

 

[dingy2]

MMC on a tapped hole at MINOR DIA is conducive to checking fixtures for the shop floor. If you do not have tapped holes at MMC, their position cannot and will not be checked on a regular basis once the run has begun.

If one applies MMC without MINOR DIA noted under the FCF, then it would apply to the pitch cylinder which is rather difficult to confirm.

Taking parts to the CMM room on a regular basis is not cost efficient and that is what is required if the tapped holes are not at MMC.

Dave D.

http://www.qmsi.ca

 

[joebk]

Good point Dave, I must admit I didn't think of that (I should have)! So I have learned a valuable lesson, this is something I will have to keep in mind from now on.

There is no indication on the drawing concerning what feature of the thread is being referenced, this might be covered by our customer's corporate drawing standards.

At the place I work almost all GD&T QC is done on the CMM because the manufacturing quantities are low enough that we can't justify functional gages for some of our jobs. This being said, there are many jobs where we should be using functional gages and are not. But this is something that is beyond my control.

 

[joebk]

here is the million dollar question...

I have made my case to the customer and they are not willing to modify the design to prevent interference. This is based on the fact that the parts currently used in the assembly are subject to these specifications and there are no issues with interference. They feel that increasing the clearance hole size will result in to much "slop" between the holes and the fasteners. No point in discussing this further because I am unable change this.

I made the argument that SPC or some other process control method might be reducing the possibility of interference significantly although it is theoretically possible to have interference.

I do not think it is reasonable to define a specification that can result in interference and then rely on SPC, six sigma, or some other statistical method to prevent problems. Even with SPC methods, the parts are still OK at the extremes of the tolerance ranges (and might not work). I have to many encounters with Murphy's law for this to make sense to me. Perhaps I am in the wrong here?

Has anyone had to deal with a situation such as this? Any words of wisdom? Thanks again!

 

[PaulJackson]

joebk,

Can't help you with the potential interference from the stack or the reluctance of the customer to change the numbers but fasteners bend and stretch so they probably can tolerate a little greater probable interference than other situations.

Threads have their own unique problems in both design and measurement. I prefer tolerancing them RFS for the reasons drawoh mentioned above and for the following reasons.

Some threads are tapped, some are roll formed, and some are self tapped by the fastener itself.

Most of the high volume production processes that I have been involved with prefer roll forming where the thread is formed by metal flow (no chip removal required) and the minor diameter ends up smaller than the pre-drilled hole. If a roll-formed thread is not fully developed (worn tool) the minor diameter will often be larger than spec. That makes the thread weak! Attribute position gages do nothing to monitor this failure mode but a no-go size pin gage can help to spot it (I know that all size conditions opposite the MMC size should be checked with spread gages and no-go pins should't exist but not in this case).

Tapped holes (cut with tools or fasteners themselves) get their minor diameter from the drilled or cored hole and if an attribute go position gage was of any use it would be at this stage in the process checking both the virtual condition location and minimum depth of the drilled or cored hole.

The biggest problems with threaded holes in production are:

Threads too shallow (worn tooling or broken tap) which causes fasteners to fail to provide clamp load.

Threads to weak (minor not fully formed) which causes fasteners to fail by stripping the threads from the hole.

Threads undersize (worn tooling) which may either cause the fastener to not fully seat failing to provide clamp load or cause the fastener to break from stress.

If I was concerned about gaging...the more frequent checks would include Go, No-Go thread fit and Min full depth for all threads...plus Go, No-Go minor diameter size for rolled threads. Since the position tolerance is typically generous I would less frequently check the minor RFS (various ways) or pitch RFS (with expanding split threads) in layout or use a go position gage on the minor MMC for tapped threads or use a go position gage on the pre-drill MMC size for rolled threads.

The advantage of checking the thread position RFS is that sample sizes reduce drastically to predict capability.

Paul

None of the production inspections that

 

[drawoh]

PaulJackson,

I think this is a separate issue. Crunching the numbers might help me understand Dingy's post, and it will give us a sense of perspective.

I want to specify an M4 tapped hole, and a clearance hole in the mating part. The two parts are located by their datum features and for the sake of this discussion, it does not matter where these are. Assume the mating part is thin and I do not want to mess around with the perpendicularity of my tapped hole.

I call up an M4X0.7 6H hole at a positional tolerance of 2mm diameter at MMC, minor diameter.

My clearance hole is 4.7/4.3mm diameter with a positional tolerance of zero at MMC. I have allowed 0.1mm diameter for any perpendularity error. I am lazy, but I hate surprises. If the fabricator tries to do 4.5mm diameter, they have to achieve a 0.2mm positional tolerance, and the diameter can still go 0.2mm over.

From my Machinery's Handbook, and based on the 6H tolerance class, my minor diameter is 3.422/3.242mm diameter.

Would I be correct in assuming that Dingy's inspection tool is a 3.42mm diameter pin with 0.2mm diameter slop? Perhaps it is a precisely located 3.22mm diameter pin.

This makes me nervous, as a designer. What we have here is a 0.4mm tolerance zone due to the LMC condition. I need a 4.5mm diameter clearance hole to guarantee assembly. My clearance hole callup would be 4.9/4.5mm with a positional tolerance of zero at MMC.

The pitch diameter is 3.663/3.545mm diameter. We inspect this with a thread guage. The go gauge must go in. The no-go must not go in more than three threads. This is an inspection procedure entirely separate from checking the location of the hole. The actual minor diameters can be checked with 3.242mm and a 3.422mm pins. The 3.22mm pin noted above would pass some invalid minor diameters, but that was not what we were checking.

The obvious point here is that checking the form of the tapped hole is completely separate from checking the location of the tapped hole. A less obvious point is that if someone wants to make a pin fixture to inspect the location of tapped holes, I the designer, must prepare the drawings, and the design, accordingly.

I was going to argue that tapped holes are an order of magnitude more accurate than location tolerances. There is a reason we should keep Machinery's Handbooks on our desks.

JHG

 

[PaulJackson]

Drawoh,

You as the designer need to verify that the MMC size of the fastener’s major diameter clears the virtual condition size of the clearance hole. That is the functional requirement and the design parameters should support that. I suppose that the position tolerance the major diameter of the fastener relative to the pitch cylinder would be included in that stack but few if any go there in determining the probability of interference, they just use the MMC size of the fastener.

That being said, inspectors or gauge makers must devise a way to check the position of the threaded hole. It’s complicated! You can see from my post that I started to explain something “None of the production inspections that…” but didn’t finish. I was going to say that neither inspectors nor machine operators like twisting those fixed size or expandable thread devices into the holes to check the position of a thread so it seldom is done like that. Typically the measurement defaults to the minor diameter of the threaded hole. Believe me that CMM operators use DCC software routines written to probe the minor diameter with the same lead path as the thread to estimate its location (either on the minor peaks or between them) if they have newer software, others just bang around in the holes. Dingy’s advice (I think) was to declare (in the specification) that the position applied to the minor diameter and to check that with an attribute (functional) gauge because checking the minor with a virtual condition pin is commonly done no matter what the design states. However, the minor diameter is typically in a clearance condition relative to the fastener no matter what interference the fastener has with the clearance hole (fasteners bend, deform, and stretch).

Here is the dilemma with threads, the designer figures the functional parameters for threads and protects against functional interference and inspection checks something totally different. It happens every day. (I think) Alex at GM sought to align these practices by declaring that the position tolerance applied to the minor diameter… but constraining the minor is not the critical functional requirement. I saw this when I was aligning the joint venture transmission designs between Ford and GM.

I am reluctant to chase the numbers that harmonize the major, pitch, or minor interference of the design to the clearance hole because I think that designers should primarily protect the design for function and subdue their concerns about how the tolerances are inspected. So I would say that the focus should be on the major diameter's interference with the clearance hole (considering or not its position with the pitch cylinder). Inspection is an art…like design…that guards or predicts the probability of failure with many variable parameters. There are significant considerations in designing that make one far superior to another but (I think) that typically involves how the design portrays the tolerable functional variation in its integrity, simplicity and measurement stability.

Paul