I have got a part for which one of the holes with a diameter of 14 mm has a profile tolerance for all around the hole surface of 0.5 mm. Is that meaning that I can go for the diameter between 13.5 to 14.5 mm? I do have a true position for the hole too, and in order to get the right bonus tolerance, I would like to know if I can get the diameter toleranced like that.

Second question is related to profile tolerance too. I have two parallel surfaces, for both of them I have a profile tolerance of 0.08 mm. One of this surface is datum too. I have a basic (boxed) dimension between these two surfaces, which is critical to the customer. How much can vary this basic dimension? +/- 0.08 mm or only +/- 0.04 mm (the tolerance given by one profile?

Thank you very much for your help.

The profile tolerance on a hole is NOT practical but does meet ASME Y14.5M-94. The hole should have been shown in positional tolerances but I have a feeling that the Designer is not too knowledgeable on GD&T.

The 14 mm size MUST be in a basic dimension (box around it) so it is theoretical. If one has a profile tolerance to datums A,B & C of say 0.5, it means that the outer boundary diameter shall not exceed 14.5 with the inner boundary not less than 13.5 from a basic dimension to B and C while perpendicular to datum A (most often).

Now comes the tricky part - how to measure it. It must be performed on a CMM and the Operator must set the hole up to datums A, B and C and the scan the hole all around and up and down. No part of the surface of the hole can be above the 14.5 and under the 13.5 boundaries. What a pain!!

Second Question

This is an easy one and very practical. A basic dimension is theoretical and has no tolerance. A profile tolerance of 0.08 means about the theoretical dimension one has a +/- 0.04 unless phantom lines are on the drawing. It is a bi-lateral tolerance. One must sweep the area with a dial or digital indicator setting the part up on the datum and moving the indicator to the basic dimension. When one sweeps the surface the indicator must not go above or below 0.04.

Profile in this situation controls the surface for flatness, angularity (parallelism) and also its location. Good stuff and this can be checked on the shop floor with a little checking fixture.

Hello, this is not always so simple, maybe more info is needed. If the hole has a standard tolerance for that size, which designers often specify on some 20 volume manuals then it could mean the hole is fixed eg +/-0.25 on dia and the hole shape ( you didnt say if roundness etc) can vary withi that by total 0.5mm also depending if that std means TIR( maybe as norm) The position tol, maybe for max/min material calc is different again and can be used for root sum square if you have a series of hole tolerances

cheers
alan

On the first question I will agree with AlanC. If not phantom line is shown that means we go with bilateral tolerance +/- .25 on the hole size and not +/- .5

I have got a part for which one of the holes with a diameter of 14 mm has a profile tolerance for all around the hole surface of 0.5 mm. Is that meaning that I can go for the diameter between 13.5 to 14.5 mm?
Yes, the holes surface must be contained within two coaxial circles (profile of a line) or two coaxial cylinders (profile of a surface), with the inner at 13.5mm and the outer 14.5mm. If datum features are specified in the profile note then the tolerance zone is constrained for orientation and/or location relative to them. If no datum features are specified the profile note constrains only size and the boundaries of form.

I do have a true position for the hole too, and in order to get the right bonus tolerance,
If the position note has a (M) tolerance modifier specified and the hole’s profile note has no datum features specified then the maximum potential “bonus” tolerance for the hole’s location would be 1mm diameter. Any in reduction in size, deviation in form, or deviation in orientation from the specified DRF will reduce the actual variable location tolerance “specified + bonus.” If the profile note for the hole has datum features controlling the hole’s location then the position note and the profile note are conflicting.

I would like to know if I can get the diameter toleranced like that.,
I don’t understand your question. You have described how the hole is toleranced.

Second question is related to profile tolerance too. I have two parallel surfaces, for both of them I have a profile tolerance of 0.08 mm. One of this surface is datum too. I have a basic (boxed) dimension between these two surfaces, which is critical to the customer. How much can vary this basic dimension? +/- 0.08 mm or only +/- 0.04 mm (the tolerance given by one profile?
If the surface that is designated as the datum feature has a profile tolerance of 0.08 with no datum feature specified it’s profile callout is only controlling the datum surface flatness. If the opposite surface’s profile note specifies the datum surface then all points of it’s surface must be contained between two parallel planes spaced 0.08 apart that are parallel to the datum surface and are located the from basic +/-0.04. So the answer would be the latter +/-0.04.

Paul

Wweng:

Profiles are not diameters but surface conditions. We have a bi-laterial tolerance of range of point 0.5 on the surface. This turns into +/- 0.25 from the theoretical.

The size of the hole is a basic 14 mm. In any spot on the diameter, we have +/- 0.25 and diametrically opposite we also have +/- 0.25 making the inner boundary diameter of 13.5 with an outer boundary of 14.5.

Paul:

There was no mention in the question about positional tolerances which, of course, should have been specified.

Read the original question again Dave. "Should" is "of course" your opinion!

You are correct Paul, the original question did state that they had a "true" position tolerance in addition to the profile tolerance.

I have to thank everybody for all the details given, you've been more than helpfull. However, in order to give more details:
1. For the first question, the hole has a profile tolerance and a true position given, at maximum material condition for the hole, with the basic diameter (boxed) at 14 mm. I know it's not usual, but the biggest problem that I have is the fact that sometimes designers don't have a clue about difficulties related to check all these geometrical tolerances on the floor, by operators.

2. The surface which has a profile tolerance (being also datum B) has a profile tolerance related to the datum structure A, B, C, while the other parallel surface has the profile tolerance given with respect to the same datum structure (A, B, and C). So Paul, in order to understand now, due to the fact that both surfaces have profile tolerances given with respect to the same datum structure, can I assume that both surfaces can vary within +/- 0.04 mm, allowing the distance between them to vary within +/- 0.08?

Thank you very much again.

The surface which has a profile tolerance (being also datum B) has a profile tolerance related to the datum structure A, B, C,.
The profile of surface |B|to |A|B|C| would only control Surface |B|'s orientation to |A|. That orientation must be contained between two parallel planes, perpendicular to |A| and spaced 0.08 apart.

while the other parallel surface has the profile tolerance given with respect to the same datum structure (A, B, and C).?,.
The basic dimension for the profile of the surface opposite |B| originates from the DRF established both surfaces |A| and |B|. Surface |B| will touch that DRF theoretically at only two places. There are many scenarios that one can imagine that would result in the point to point dimension between |B| and the surface opposite B but their extremes cannot be used to supplant the profile check of the surface to |A|B|. For instance if |B| was perfectly flat and perfectly perpendicular to |A| the opposite surface must still be within the basic displacement +/- 0.04. and the point to point dimension would effectively be the basic +/- 0.04. On the other hand If |B|'s perpendicularity to |A| consumed all of its 0.08 tolerance and the two of the highest points +0.04 touched to establish the DRF then the point to point dimension to the opposite surface if it also consumed all of the +/- 0.04 profile could yield point to point dimensions of +0.04/-0.12 from basic because the points opposite those that established B +0.04 opposite +0.04 on the other surface would yield basic +0.04 and the points -0.08 on |B| opposite -0.04 point on the other surface would yield basic -0.12.

Sorry for gauntlet! My wife always stops me saying TMD! (too much detail)

The point is... you cannot supplant the profile measurement with a size measurement!

So Paul, in order to understand now, due to the fact that both surfaces have profile tolerances given with respect to the same datum structure, can I assume that both surfaces can vary within +/- 0.04 mm, allowing the distance between them to vary within +/- 0.08?
So the answer is NO.

Paul

Paul,

Thank you very much for all the details. In our job there is never too much details.

One more question for you. I have a part with a datum B on a radial surface. In order to check the part, I have to rest it in a fixture that touches that radial surface. For that surface I have a profile tolerance given (0.25 mm) with regard to the datum structure (A, B, and C). If I take the part from the fixture (to check the profile, it is almost impossible to recreate the datum structure. How can I check this profile for that surface?

Regards,

Daniel

I can try to imagine the geometry that you are describing but like the scenarios you described earlier as more details emerged our vision of your problem improved.

A picture (or a sketch) is worth a thousand words.

Failing that give more details.

One excellent way to attack these problems in measurement is to probe, scan, or precision photogrammetize the surfaces and compare the point-cloud to a solid model on the computer. I know it sounds sophisticated but my podiatrist took a hand held box laser scanner connected to his old PC and with one scan had a point cloud of the contour of the bottom of my feet to make me a pair of foot beds.

Paul

Paul,

Thank you. It was a pleasure discussing with you all the issues that I had.
Hopefully we will be in touch for future issues.

My best regards,

Daniel Negrea