True Position using Bolt circle and Angle

[Jaydenn]

Hi,
Quick question.

Imagine you have a square part with 2 holes.
One hole is right on center and it is datum A.
The other hole is drilled somewhere else, on the same face.

It is dimensioned using a bolt circle and one angle.

Now, the only thing I need to control tightly is the radial distance from datum A. So I apply a Positional tolerance of .001" to datum A.

My question is this...Do BOTH dimensions need to be basic? or just the Bolt circle?

The angular position can vary by 50 degrees so I do not want to include it in the tolerance.

Know what I mean?

Thanks,
J

 

[KENAT]

To use positional tolerance the locating dimensions need to be basic.

You could perhaps use a bilateral positional tolerance more like you typically would with a slot. So separate FCF for the radial displacement V the angular. I've never seen this with the dimension scheme you are proposing but have with rectangular dimensioning schemes.

KENAT,

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

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

What is Engineering anyway: faq1088-1484

 

[Jaydenn]

So, how then, can I control the radial only position of the hole and NOT control the indexing of the same hole?

Is their even a way using GDT?

I added a sketch. the ONLY thing I want to control is the dimension shown.
The small hole shall be free to rotate about the center.

Now, I know I could simply put a linear tolerance on it, but I am curious if GDT has a way to do it.

J

Oh, BTW, this is not a real life situation, just something I thought up on a lazy Thursday afternoon.

 

[drawoh]

Jaydenn,

Let's see if we understand your design and requirements.

Your plate is attached using two screws. Both screws must pass through their clearance holes. The locatation and rotation of the plate is much less critical.

Apply a dimension and ±[&nbsp;]tolerance between the two holes. A GD&T positional tolerance controls two dimensions, and so far, you are controlling one. For screws, as opposed to bolts, your tolerance should be ±<screwclear>/2, or ±<boltclear>.

You could apply a tolerance to your angle, but this would be hard to inspect, and meaningless if you do not apply it carefully. I would apply a GD&T positional tolerance to your second hole, using the base, the first hole and some clocking feature as datums. This would control only the rotation of your plate, so it would not be very accurate.

Do not bother to draw the pitch circle. It has no meaning if there is only one hole on it. Your angle would be a basic dimension. I would be tempted to replace the angle with a linear dimension from your clocking feature, which also would be basic.

JHG

 

[KENAT]

I just tried to give you the GD&T answer. You split the radial and rotary tolerances and put in separate FCF. Take a look at figure 5-42 in ASME Y14.5M and paragraph 5.9.2.

If you don't have the standard to hand I'll try and post an example.

KENAT,

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

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

What is Engineering anyway: faq1088-1484

 

[JLang17]

What if you gave the small hole X,Y dimensions from your datum A, or large hole, and then apply positional tolerance and reference datum A. This will maintain the distance you desire and since there is no clocking datum, the small hole can orbit around datum axis A.

 

[powerhound]

If you use a positional tolerance then your dimension between the two holes must be basic. A +/- tolerance would be illegal. If this is one part of a mating assembly then using position would probably be the best way to go. If the holes are used to mount 2 separate objects that are not really related to each other then a +/- tolerance might be okay but either way, you should drop the bolt circle, as drawoh said, as it is pretty much meaningless when there's only one hole.

Powerhound, GDTP T-0419
Production Manager
Inventor 2009
Mastercam X3
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[KENAT]

I'm pretty sure the OP's real question is fully answered by figure 5-42 or the standard and the related text.

Attatched is an approximation of that figure (don't ding me for minor issues, I rushed it).

http://files.engineering.com/getfil...a72c-df804e1d876d&file=5-42-APPROXIMATION.tif

KENAT,

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

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

What is Engineering anyway: faq1088-1484

 

[HGMorgan]

We had one like this a while back.
Large ring with 32 ea .500 dowel holes to hold circular Thompson rail to position.
T/D had TP Dia of .005, and some of the holes were failing the CMM survey.
Changed the CMM output from XY TP to radial +/-.0025 and every hole passed.
T/D changed the call-out to Rxx.xxx +/-.0025

 

[drawoh]

HGMorgan,

As I noted above, a GD&T postional tolerance controls error in two dimensions. Most of the time, including your case, this is what you want to do. Your original positional tolerance of Ø.005" does this. I suggested a ±[&nbsp;]tolerance for the OP because he does not require this for his particular application.

Your ±.0025" tolerance on the radius does not control the angle. Nor is your ±.0025" equivalent to a positional tolerance of Ø.005". By my figuring, your postional tolerance reflects a clearance around your pins of .010". The required tolerance on your pitch diameter would be .0035". The tolerance on your radius should be half that.

Your angle tolerance is a function of the pitch circle diameter. For a 12" pitch circle, you need an angle tolerance of approximately one arc minute.

I have all this worked out on my website. I am planning to do a re-write, but the math is good. Note now I worked out reducing the diametral tolerance to loosen the angle tolerances, and note how futile this is.

Either your original tolerances were too tight, or you are making parts that do not work.

JHG

 

[ewh]

It is an imaginary situation for the purpose of understanding GD&T application.
Good post though drawoh.

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[HGMorgan]

drawoh-
I would suggest that the posts in this thread be studied a little deeper.
As Jaydenn noted in the original post:
"Now, the only thing I need to control tightly is the radial distance from datum A."
And:
"The angular position can vary by 50 degrees so I do not want to include it in the tolerance."

In his case, and, in ours, only the radial dim is important; it is not desired to control the feature in two directions. That is why our Customer's Tool Design Dept agreed with us and changed the drawing to Rxx.xxx +/-.0025

I would suggest that GD&T True Position Diameter tolerance be studied a little deeper. TP Dia is a circular tolerance zone. A TP Dia tol of .005 means that a feature can be off .0025 in a straight line from the center of the zone (radial). On a radial dimension, you can only be off in one direction....


The customers tolerance may have been too tight, but they are the customer, and, we helped set the correct call-out and tolerance that allowed a product to be manufactured at a lower cost yet still meet function requirements. Obviously the product works because there have been several hundred airplanes built in those tools since we sent them in.

Thanks for the offer to visit your web-site.

 

[drawoh]

HGMorgan,

The OP has a centre and one hole. He is trying to put two fasteners through one or both features. For this purpose, the angle of the second hole is irrelevant. All the angle controls is the rotation of the part, which I understand is much less critical. My first dimensioning proposal is a solution for this. The problem and the solution are somewhat unusual.

In your case, you have 32[&nbsp;]dowels spaced around a circle. The angles are critical. Your holes and your pins must be spaced accurately enough for all to interface. This is the conventional GD&T tolerancing problem. You have to control position in two dimensions. You cannot just specify or assume an angular error of zero.

It sounds like your process achieves angles accurately, but has trouble with pitch circles.

JHG

 

[KENAT]

drawoh, I think you're reading too much into the OP's example. His real question appears to be about bidirectional tolerancing, which I'm pretty sure figure 5-42 in ASME Y14.5M and paragraph 5.9.2. fully addresses.

KENAT,

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

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

What is Engineering anyway: faq1088-1484

 

[axym]

I think we're having trouble here because of the mixture of geometric and plus/minus tolerances on the same feature. I can help with the meaning of the GD&T, but I'll leave it to the rest of you to try to interpret of the plus/minus stuff.

Let's look at the Position control described in the original post (with the center hole as the datum feature). The tolerance zone would be 0.001" in diameter, and would be located at a distance of exactly 1.456 (this dimension must be basic) from the datum. Because there are no other datum features referenced, the tolerance zone's "angular" location (relative to the sides of the part) would not be controlled at all. So the Position control that Jaydenn described would provide the intended "radial only" control. The "angular" location would have to be controlled by some other tolerance. Since the angular tolerance is so huge, a plus/minus tolerance on the angle relative to one of the sides is probably adequate.

If you want to use GD&T to control the angular location more loosely (or more tightly) than the radial location, the bi-directional method in the Fig 5-42 diagram is the way to do it. KENAT's diagram has the angular location toleranced more tightly than the radial. Note that KENAT's diagram shows the hole referenced as secondary, and has a tertiary datum feature with a basic angle. All correct.

Evan Janeshewski

Axymetrix Quality Engineering Inc.

http://www.axymetrix.ca