How does Rule #1 apply to 2 holes... 1

[Runz]

How does rule #1 apply to two hole that are shown on the same center axis?

If I have a hole through a part that has a postional tolerance of say .015 and the feature tolerance is Ø1.0000±.0005, then the axis of the hole must be within .015, but the form of the hole straightness/roundness) must be no worse then .0005 at LMC. This ensures that my pin at MMC (Ø.9990) would go through the hole

What if a notch is machined between the two holes, but a centerline is shown through both? Does this rule still apply? Will the pin be assured of fitting or is a dual frame needed to control the hole to hole relationsship? Could the second hole be off by .0075 and still be within print?

Thanks,

 

[PhilBW]

Rule #1 applies only to individual features. The axis of one hole will need to be designated as a datum, and the other hole will have a tolerance with respect to that datum.

 

[Runz]

Thanks Phil.

There was a difference of opinion here. Some thought because the centerline was shown between both holes, they assumed the same controls as though they were one feature. Others thought as you mention.

Thanks again!

 

[ewh]

A datum axis may be established by coaxial datum features, and would normally be used as a primary datum. The control would look something like this:
| TP | dia .XXX | A-B | C |

 

[drawoh]

Runz,

Check out ASME Y14.5M-1994, Figure 5-51. It may answer your question precisely.

The figure describes a hole with one diameter specification, passing through three slots. There is a composite positional tolerance, one of which has no datums. The positional tolerance with datums controls the position of each of the four resulting holes. The other positional tolerance positions the holes to each other. You will find the figure much more understandable than my explanation.

A lot of this is controlled by your design and how you prepared your drawing. Is it obvious that the two holes line up and are controlled by the same diameter specification? Is it possible to fabricate the two holes with one tool in one pass?

JHG

 

[dingy2]

The easiest way to control the C/L of the holes is to reflect them with a positional tolerance at MMC. One does not need to have a datum to use positional tolerances.

I would reflect the holes with a 2 X and size and then place the feature control frame below.

The shop floor will love this callout since they would make a checking pin the virtual condition size. This is a quick check.

Hope this helps.

 

[ewh]

dingy2,
Could you tell me where in ASME Y14.5-1994 it is stated that no datums are needed for true positioning? I was taught that true position is always relative (to a datum or datums).

 

[dingy2]

On page 147 in the ASME Y14.5M-94 is an example of your situation. The top half of this composite feature control frame reflects position of the holes relative to datums. This is called the Pattern Locating Tolerance Zone Framework.

The bottome section of the feature control frame reflects the holes to each other. This is called the Feature Relating Tolerance Zone Framework.

Make sure that you have the positional tolerance at MMC so that it can be confirmed easily on the shop floor. Without MMC, the product would have to go to the CMM room (co-ordinate measuring equipment).

Also, the tolerance in this feature control frame can be down to zero meaning that the size variation will give one the tolernance.

Hope this helps.

DD

 

[ewh]

Thanks, dingy2!

Does this only apply in regards to coaxial features?

 

[dingy2]

This applies to coaxial features with no datum and one could even different size holes. If one has different size holes, make sure that you place the number of holes at the bottom of the feature control frame and state that they are coaxial. If one had 4 coaxial holes, one would place "4 COAXIAL HOLES" but, again, make sure that you have positional in MMC.

This is an easy check on the shop floor.

I would not worry about rule one in this case.

DD

 

[ewh]

Thanks DD,
I was asking because lately I am seeing drawings using a composite true position without a datum callout in the second line, like the situation you described, except these are being applied to thru hole positions on a lofted surface; coaxial conditions do not exist, and no two hole are oriented the same. Am I correct in flagging this as a mistake, or is this a situation where it is allowed? Thanks again, I appreciate understanding this standard better.

 

[dingy2]

Do NOT flag this. We have a situation where there may be a cluster of holes. The top section of this composite feature control frame reflects the pattern location relative to up to 3 datums - primary, secondary and tertiary.

The bottom of this composite feature control frame reflects the holes in the pattern relative to, usually, the surface. In other words, you have a requirement of hole to hole and perpendicular to the datum surface.

In a composite feature control frame, the datum reference in the bottom section is for orientation and in many cases, means perpendicular.

Hope this helps.

GD & T is not easy and sometimes the standard leaves a lot to be desired.

DD

 

[ewh]

You deserve a star.