Surface profiel callout with NO DRF 2

[jammin7800]

Typically, when we DO see datums specified on a surface profile callout, that tells us to set the part up to datums and measure the surface relative to those datums. No best-fitting allowed.

Also typically, if we DO NOT see a datum reference frame on a surface profile tolerance, that tells us we are allowed to best fit that surface onto its nominal shape, using all 6 DOF.

I have a situation where a surface profile tolerance is on a print with NO DRF. The customer is telling me that it is IMPLIED that this is wrt datums, even though none are specified.

Further, he claims this is part of his company's specs. I looked at the spec, but this situation isn't covered. But the spec does reference ASME 14.5M-1994. So I looked at the ASME spec. I couldn't find it in there either.

So my question is this --- what does the ASME 14.5M spec say about surface profile tolerances that do not reference datums? Is it IMPLIED that datums are specified, or does no DRF mean best-fitting is allowed?

 

[SteveMartin]

I do not know of a situation in the ASME spec that uses an implied datum reference frame. I can't figure out how you would ever develop an implied frame - even simple parts have many possible datum reference frames. Bottom line - if you want something, specify it. Never imply.

I would ask the customer to walk you through where in his company spec this is addressed.

 

[dingy2]

ASME Y14.5M-94 does not state that datums are implied if the feature control frame does not include reference datums.

There are situations where one could have a profile of a surface - all around - with, possibly, a surface reference datum. In another situation, one might have a profile without any reference datums on surface that are coplanar which means one must treat this as a single surface on a single plane.

Dave D.

http://www.qmsi.ca

 

[SeasonLee]

Surface profile control can be used with datum feature references as a related feature control. When datum features are referenced. the tolerance zone is related to the datum reference frame.

Surface profile control can also be used without datum feature references as a form control. When no datum features are referenced, the tolerance zone applies where the part surface actually exists.

SeasonLee

 

[jammin7800]

So, then --- no DRF means best-fitting is allowed. Correct?

 

[pmarc]

In section 4.4 of Y14.5M-1994 standard there is a note (at the very bottom of page 52):

"When necessary to relate linear and angular dimensions to a datum reference frame, the desired order of precedence may be indicated by a note such as: UNLESS OTHERWISE SPECIFIED, DIMENSIONS ARE RELATED TO DATUM A (PRIMARY), DATUM B (SECONDARY), AND DATUM C (TERTIARY)." This note is not to be used in lieu of indicating datum references in a feature control frame for geometric tolerancing applications."

My understanding of the last sentence is that implied datums for a profile of surface callout (which is geometric control) are not allowed. Datums must be specified in a FCF if the intention is to relate profile of surface tolerance zone with any datums.

 

[SeasonLee]

I’m not quite sure the meaning of “best-fitting”, surface profile can be used to control four part characteristics: Size, Location, Orientation and Form. If no datum referenced on the surface profile means to control the form.

Let’s talk about the implied datum. A profile control may be used where it is intended to control two or more coplanar surfaces as a single surface, in this case an implied basic zero dimension exists between the coplanar surfaces that establish the true profile, the tolerance zone is a unilateral boundary extending away from the implied self-datum, a unilateral tolerance zone is automatic with an implied self-datum.

SeasonLee

 

[MechNorth]

By "best fitting" one can shift the workpiece about its 6dof to find the best fit of the workpiece within the maximum & minimum boundaries (i.e. offset geometries from the basic dimensions) to qualify the part. Yes, this is the case where no drf is provided in the FCF. Datums are never implied, regardless of what your client believes. The note PMARC cited from 4.4 is a bridge or incremental improvement for "old-school" drawings with +/- tolerances so that they at least know how to set up the part for inspection ... doesn't do a lot beyond that. Even then, the datum symbols must be put on the drawing so that they know what datum features need to contact datum simulators.

Jim Sykes, P.Eng, GDTP-S
Profile Services

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[jammin7800]

Thanks, Jim. That was our feeling too.