Calculating Positional Tolerance 7

[JLang17]

I am familiar with using the X,Y tolerance range to calculate a diametrical positional tolerance (the square with a circumscribed circle method) using the SQRT(X^2+Y^2) equation.

I have a very simple drawing of a plate with a bunch of holes through it and all dimensions are +-.01. I need to apply GD&T to the drawing. Is it correct to simply use the above method to calculate all the positional tolerances? (in which case the tolerance would be the same for every hole since all dimensions are +-.01) It seems too easy.

I have no knowledge of the pin/shaft to go through the holes, or if it's a hole on another plate to be alligned. Is this information needed to apply a positional tolerance to the hole?

 

[KENAT]

There is a difference between calculating equivalent positional tolerance for +- tolerance and applying the correct tolerance.

Your equation will get you the equivalent positional tolerance, .028".

To get the correct tolerance (ensure fit/function) yes you need the mating part information and to use the equation stated in Appendix B4 of ASME Y14.5 (also in my spreadsheet on thread1103-221602 sept 4th post) or equivalent.

KENAT,

Have you reminded yourself of faq731-376 recently, or taken a look at posting policies:

http://eng-tips.com/market.cfm?

 

[KENAT]

Just realized, I'd assumed it was a fixed fastener situation, if not then the floating fastener calc should be applied.

KENAT,

Have you reminded yourself of faq731-376 recently, or taken a look at posting policies:

http://eng-tips.com/market.cfm?

 

[SeasonLee]

JLang17

You need to times 2 ( X2 ) on your equation above to get the correct data.

There are two simple ways to get the positional tolerance :

1. Positional tolerance = Overall Plus / Minus tolerance X 1.4142
Example : ±.01 = Overall .02 tolerance
Positional tolerance Ø = .02 X 1.4142 = .0283

Overall Plus/Minus Tolerance = Positional tolerance Ø X .70711
Example : Positional tolerance Ø.0283
Overall ± tolerance = .0283 X .70711 = .020 overall = ±.010

2. If you don’t like calculation, you may convert it from the chart ( as attached )

Hope this will help you

SeasonLee

 

[KENAT]

Whether the OP needs to X2 depends on if they enter the total tol range or the deviation from mean, they don't explicitly state which they are using.

KENAT,

Have you reminded yourself of faq731-376 recently, or taken a look at posting policies:

http://eng-tips.com/market.cfm?

 

[drawoh]

JLang17,

The positional tolerance equivalent to ±.01" X/Y tolerances is Ø.028". This is all assuming that your X/Y tolerance was intended to allow a hole to be .014" out of position. It is always possible that the designer was trying to do something else.

A convenient estimate is that a clearance hole for a bolt requires a positional tolerance equal to the hole clearance, C=DRILL-SCREW. For a screw in a tapped hole, the geometric tolerances should be C/2.

Note that drilled holes are oversized and screw major diameters are undersized. I call up my clearance holes as +TOL/-0. In the case of the screw, it is assumed that the material being clamped is thin. Otherwise, you must account for the perpendicularity of a screw in an angled hole. Also, it is assumed that both parts are being made to the same tolerance. If you are clamping a casting with cast-in holes, to a machined mount, you may want to mess with the model a bit.

JHG

 

[KENAT]

I know some people don't like the formatting etc. but take a look at the spreadsheet. It uses the terms/formula from 14.5 which is basically the formula drawoh gives. The tab 'example 3' may be especially useful.

http://files.engineering.com/getfil...849f922&file=APPENDIX_B4_ASME_Y14.5M-1994.xls

KENAT,

Have you reminded yourself of faq731-376 recently, or taken a look at posting policies:

http://eng-tips.com/market.cfm?

 

[wgchere]

All this calculating is fine, but the whole point of True position GD&T is to buy off the parts that would normally fall outside the square tolerance and within the circular tolerance. Additionally, it allows for easier calculation of mating holes and "bonus tolerance."

So, if the problem is just converting Cartesian tolerances to diametral tolerances, I'd say use the chart. If the object is to re-engineer the parts to maximize the GD&T, then you probably want to fire up the calculator. But even in that situation, I tend to stick to standard tolerances (Ø.014, Ø.028, Ø.042, etc.) and I tend make the holes the nearest drill size up, instead of the exact hole size (unless you need the exact hole size, of course).

 

[KENAT]

wgchere, it's to buy off parts that fall outside of the square so long as they work. Typically when I see nice round numbers such as +-.005 or +-.010 it's because people have invoked block tolerance. This for hole patterns usually means they haven't correctly considered tolerancing. So I stand by my distinction between equivalent and 'correct'.

I agree with choosing standard drill sizes whenever possible, along with typical drill tolerances but never understood the obsession with 'standard' position tolerances. I always use the largest that the fastener/drill/function will allow.

KENAT,

Have you reminded yourself of faq731-376 recently, or taken a look at posting policies:

http://eng-tips.com/market.cfm?

 

[JLang17]

Thanks for the responses. Now I have another question, which I'll try to explain the best I can.

I have tapped holes called out for #6-32. Most charts will tell you the screw size is 0.138 and the tapped hole size is 0.1065. Once the hole is tapped, it is increased to 0.138. So now the screw size and hole size are the same. If I want to position at MMC (let's say +-.005), I'm left with a negative tolerance since the screw is increased to 0.143 and the hole is decreased to 0.133.

OR do I consider the chart to be at MMC? So it would read screw size 0.133 (+-.005). And hole size 0.143 (+-.005). This then would work fine, but I don't know if these charts are suppose to be read at MMC.

 

[KENAT]

JLang17, I always use the screw max dia for my calculations. You don't need to worry about what the tap size is, you need to worry about what the clearance hole size in the mating part is.

I think you may be totally confused. The chart SeasonLee posted is just for converting +- dimensions to equivalent positional diameter. It isn't for calculating the required tolerance to ensure fit.

Use instead the equation drawoh gives which is the same as in my excel sheet. Take a look at the examples in my excel sheet hopefully they'll help you.

Simplistically for fixed fastener:

1. Subtract the screw max major dia from the minimum hole diameter.

2. Divide the result between the threaded & clearance hole.

It's often better to give slightly more of the position tolerance to the threaded hole as it doesn's benefit from MMC and with 2 operations (drilling & tapping) generally has more tolerance accumulation.

If you're still confused post the clearance hole diameter & it's tolerance and I'll try to find time to do a worked example for you.

KENAT,

Have you reminded yourself of faq731-376 recently, or taken a look at posting policies:

http://eng-tips.com/market.cfm?

 

[drawoh]

JLang17,

My quick and dirty assumption about screws is that they do not move in their holes to accomodate the mating part. MMC is not relevant to tapped holes.

Take the case that this is my drawing, and that my primary requirement is for the screws pass through the clearance holes.

[ol]
[li]I call up the 6-32UNC hole with a positional tolerance of Ø.015". If I ignore the angle of the tapped hole, I can assume that a screw in the hole can occupy space anywhere inside a diameter of .138"+.015"=.153".[/li]
[li]On the mating part, I call up a hole Ø.194"/.154" with a positional tolerance of 0 at MMC. Obviously, the fabricator is going to go bigger than .154" so that they have some positional slop. [/li]
[/ol]

If the mating part is thick, or otherwise, I cannot ignore the perpendularity of the tapped hole, I will have to control it, or increase the clearance hole to account for the leaning screw.

Try working this out and see if it makes sense.

JHG

 

[JLang17]

Ok, I think I understand now. My last post was quite silly since I wasn't even dealing with the mating part's hole. But looking at the same example, if the mating part's hole is 0.138 and the screw is 0.138, both at MMC, then positional tolerance will be 0. The tolerance will increase if the screw gets smaller and/or the clearance hole gets larger...correct?

 

[drawoh]

JLang17,

No, your tapped hole positional tolerance is based on what your fabricator can do. It cannot be zero. A clearance hole of Ø.138" requires the tapped hole to be located perfectly. I enlarged my clearance hole to allow for the tapped hole's positional tolerance.

JHG

 

[KENAT]

Jlang17, your math/reasoning is correct but as drawoh points out realistically that's not practical.

Expecting to hold a threaded hole at 0 positional at MMC is not realistic since threaded holes don't really benefit from the MMC concept (except in certain gaging applications which is why it is still correct to put MMC in the FCF for threaded holes).

I'm loathed to give a rule of thumb as someone will shoot it down but I'd avoid putting less than .01 dia positional tolerance on threaded holes where ever possible.

KENAT,

Have you reminded yourself of faq731-376 recently, or taken a look at posting policies:

http://eng-tips.com/market.cfm?

 

[JLang17]

I think I'm getting it...If I have a screw max diameter of .138 and a clearance hole min diameter of .168, the positional tolerance for both holes is .015. Although if I apply the 60/40 split, the screw is toleranced at .018 and the hole at .012.

I would want to check the manufacturer's capabilities to see if these tolerances are doable. And if they are not, I would want to increase the clearance hole size to allow for greater tolerances.

Does this all sound correct?

 

[ewh]

The mating clearance hole CAN be zero (at MMC), but as noted, is this what you really need, and is it worth the cost?

"The ambassador and the general were briefing me on the - the vast majority of Iraqis want to live in a peaceful, free world. And we will find these people and we will bring them to justice." - [small]George Bush, Washington DC, 27 October, 2003[/small]

 

[KENAT]

JLang17, you're getting there, you're even catching on to the idea of giving a bit more tol to the threaded hole (not screw itself).

The tolerances you state are definitely achievable. The real trade off is functionally how tight do you need V how much it costs. Very tight tolerances can be achieved but start to cost more. Ask your manufacturer at what point loosening the tolerance doesn't significantly reduce cost, if function will support it this is where you want your tolerance to be.

A related tip, tightly positioned threaded holes used to control location of mating parts often aren't the best idea. I may be cheaper to add one or two pins with mating hole/slot to get location, and just use loosely toleranced threaded holes to keep it together.

KENAT,

Have you reminded yourself of faq731-376 recently, or taken a look at posting policies:

http://eng-tips.com/market.cfm?

 

[chancey]

Thanks for sharing that spreadsheet KENAT.

 

[fcsuper]

I think this is likely one of the best threads on this boards in a very long time.

Matt Lorono
CAD Engineer/ECN Analyst
Silicon Valley, CA
Lorono's SolidWorks Resources
Co-moderator of Solidworks Yahoo! Group
and Mechnical.Engineering Yahoo! Group