Dimensioning surfaces

[TrailMaker004]

We have a question of expression/interpretation. In the attached sketch, the primary datum is a contoured surface -this is not new for us as we have worked with this many times before. The contour is defined by the baic dimensions and the profile tolerance. The (2) .437 dia holes are located in X & Y by the .500 basic dimensions.

Our question is this: since the X position of the holes are dimensioned by the .500 basic(s) from the (2) opposite end surfaces, and the 5.000 length can vary as much as +/-.006 in actual length within its profile tolerance (+.003 per side = +.006 total, -.003 per side = -.006 total), will those holes be tied to those end surfaces with respect to their X position, and thus vary in X position consistent with the +/-.006 potential length variation of the profile? Or, as some suggest on this end, because the 5.000 is a basic dim, the hole locations are tied to the implied centerline of the 5.000 basic, and their X location will not be affected by any actual variance in the profile of A regardless of what surface they are dimensioned from.

The reason the holes are being dimensioned from the end surfaces is because there is a family of parts and dimensioning from the centerline vs as described above would require a large tabulation to cover all versions.
Thanks.

 

[SteveMartin]

First: what spec governs this sketch? I'll assume ASME Y14.5M...

To answer the question as put forth: The allowable profile tolerance has no effect on the allowable location of the holes. Their allowable location is defined by their basic location and given position tolerance. If you want the holes to be relative to the as-produced sides you could define a datum on each side and give the holes seperate position tolerances relative to the relevant datums.

I do have some other questions/concerns regarding the drawing, but since they don't pertain to the asked question I'll leave them off of this response.

 

[TrailMaker004]

Thank you. ASME 14.5Y is correct.

So if I understand you correctly, their location with respect to each other will not vary if the part grows or shrinks within its allowable .006 profile tolerance, even though they are dimensioned from the end surfaces. Is it then fair to say (at least conceptually) that their implied position is defined as 2.000 from the centerline of datum A?

Also, please feel free to express your concerns about the sketch. Just for background, datum surface A is a mating/interface surface, and will functionally orient the part in the next higher assy and foster the alignment of the .437 dia holes to that same mating part. We have the capability of "best fit" or iterative alignment on our cmm's when a contoured surface is the primary datum. In this case, surface A will constrain both leveling and rotation of the part.

 

[JMarv]

If you want the holes to be relative to the as-produced sides you could define a datum on each side and give the holes seperate position tolerances relative to the relevant datums.

Aren't the as produced sides already defined as a datum? Wouldn't they they be part of the surface that defines datum A? Please correct me if I'm looking at this wrong.

Joe
SW Office 2008 SP5.0
P4 3.0Ghz 3GB
ATI FireGL X1

 

[dingy2]

I kept looking at this sketch and asked myself how the holes are oriented to datum A???? Now, if the flat surface was datum A with a profile controlling the 4 inch radius, then the holes would be 90 degrees to datum A. That makes more sense to me.

As far as locating the holes from both ends, I agree with SteveMartin. Have one end as datum C while the other could become datum D. We then would have two (2) positional tolerances, one for each hole. One hole would reference datum A, B & C while the other would reference datums A, B and D. I do scratch my head on the rational but anyway, it meets the design intent relayed here.

That is my 2 cents worth.

Dave D.

http://www.qmsi.ca

 

[dtmbiz]

It was not mentioned in the OP post as to which ASME Y14.5m year. In 1994 this callout for datum A is not legal. I have not
used 2009 in production; however from what I have read, datum A callout doesnt work either. I see a profile of an elongated feature
that a profile callout is used indicating a plane thru the center and parallel to the flats. It is not clear to me in this example as to what feature(s)
of the profile is datum A.

In the example posted the datum symbol for A hanging of the profile FCF is ambiguous at best and is probably an incorrect way to identify the center plane (5.000 dim) of the to surfaces as datum A. If the datum symbol for A was opposed to one of the arrows for dim 5.000 BSC, then I could see that the center plane is the intent for datum A, I would not use the current dims from the flat though. If that were the case I would identify the flats as datums, as stated in an earlier post.

It seems to me that your question regarding the tolerance of the overall 5.000 dim effecting the hole locations from the end(s), would be best answered as pointing out that a feature is not measured from another feature directly, but rather from the datum simulator. If the intent is for the center plane to be the datum A, then a datum simulator (e.g. surface plate) would be the origin for the measurement. If it is one of the flats then again the measurment is from a datum simulator, NOT the feature itself.

I am not sure i would use the flats in this case because of their small size. Not only should datum selection reflect part functionality and interface, but also practicallity.

I also see the drawing is incomplete or it doent matter that one axis is not constrained yet?
There is not a control for the bottom flat in the front view. IMO you need another arrow from the profile FCF to it, or possibly the "all around" symbol.
Not sure why datum B is not qualified to datum A, but seeing the tolerances that are shown that it should be considered.

The DRF is the origin for measurements and not the features themselves.

 

[nobigdeal]

I think that the drawing is legal per the 2009 standard(ASME). Unfortunately, the standard does not give very good examples and, in my opinion, leaves it a bit open-ended. See section 4.17(a) where it states that irregular features of size... may be used as datum features and also 4.17(b) states that there are times that those irregular features may not obviously show a derived point/axis/plane and that the designer may specify the fitting desired.

With that said, based on the principal that datums are simulated by their "True Geometric Counter-part", I would say that the DRF of A-B fully constrains the part. Datum A would constrain all degrees of freedom except for translation perpendicular to the datum feature (which is what Datum B constrains). Picture a fixture with the shape of the profiled feature, when the part sits in the fixture it cannot translate in the "X" or "Z" direction. Adding another datum would over-constrain the part.

Where the basics come from on the print does not determine how they are being located, they just establish where they are nominally. The feature are located by Datum A in the "X" direction and by B in the "Y" direction.

Sorry so long, but these things are hard to detail in writing sometimes, hopefully I've said something that makes sense.

 

[dtmbiz]

From what I see on the ref para's and figs, I do not see anything like the example posted. These examples state and show that features that establish datums are clearly defined. It also states that the irregular shape "contains" an center point, axis or center plane. These datums are indicated with the datum symbol in the appropriate place (eg the "anchor / suction cup" of the symbol directly across from the size dim, which then indicates a center plane in figs 4-33, 4-34, 4-35; 8-24).

2009 is the same as in 1994 in the respect of basic DRF concept; 3 planes that are mutally perpendicular and intersect.

As I posted earlier that if the datum symbol were attached directly across from the 5.000 BSC dim then it would be clear that it is the center plane; if on the flat on either end then it is a flat surface (plane).

In any advent the posted example is not clear considering the number of features contained in the profile. I question whether or not the bottom flat is. IMO it is not and the part is not constrained in the Y axis of the (front or bottom) view shown.

I only see the datum symbol attached to the profile FCF in an example pointing to a hole in which case it is clear to interpret that the hole's axis is the datum.

 

[nobigdeal]

If you re-read 4.17(b) it states "In other applications where a boundary has been defined using profile tolerancing, a center point, an axis, or a center plane may not be readily definable" and it refers to figure 8-24 which shows an irregular feature of size being located by it's "boundary", not by a plane, axis, or point. It states that this type of feature can be used as a datum and "when RMB is applied (which it is in this case), the fitting routine may be the same as for a regular feature of size, a specific fitting routine may be defined, or datum targets may be used". So, it seems to me that, an irregular shape (such as the contoured surface in this print), controlled by a profile tolerance, may be used as a datum.

As with many complex datums, it may not be difficult to make a gage, but using a CMM software to do the "fitting" that the standard refers to is less clear.

One thing I would consider adding to the print for clarity would be an "A-->B" specification to show that the profile feature is the entire contour and not just the 4" radius. Just a thought.

I worked with a customer that had 2 parts that mated on a complex shape and we were able to define the shape as a datum and added a note clarifying how they wanted to fit to that feature (LS algorithm, etc.). This worked very well to closely simulate how the part functioned. Any other datum reference frame wouldn't have been a functional DRF. The reality is that many parts mate on something other than a plane or a regular feature of size. It would be nice if all parts were "prismatic".

 

[JMarv]

I only see the datum symbol attached to the profile FCF in an example pointing to a hole in which case it is clear to interpret that the hole's axis is the datum.

I don't think the FCF is pointing to the hole. It looks to me like it's pointing to the R4.000 surface.

For the sake of clarity I redrew this in CAD. Solidworks wouldn't let me attach datum "A" to the leader, but it did let me attach it to the FCF.

Joe
SW Office 2008 SP5.0
P4 3.0Ghz 3GB
ATI FireGL X1

 

[nobigdeal]

JMarv,

I don't think "dtmbiz" was referring to the drawing on this post but to examples in the standard. Thanks for taking the time to draw it in SolidWorks though.

 

[JMarv]

nobigdeal,

Thanks for the clarification!

Joe
SW Office 2008 SP5.0
P4 3.0Ghz 3GB
ATI FireGL X1

 

[dtmbiz]

Nobigdeal,

There is no example in the standard(s) that I can find
(because they dont exist) that does not define a DRF of 3 mutually perpendicular and intersecting planes. This should be clear in any callout.

The DRF is a fundmental concept of ASME Y14.5m and needs to be clearly defined, irregular shape or not. Irregular shapes do contain these components and can be defined.

Now would you please identify these 3 planes for the DRF that the example drawing defines?

 

[nobigdeal]

dtmbiz,

Yes, there are always 3 mutually perpendicular and intersecting planes, but in many cases those planes are purely theoretical and do not always have a direct feature that they are derived from. For example, based on the standard, it is possible to have a DRF that does not constrain all degrees of freedom. Take fig 7-25, 7-26, 7-41, 7-50, etc, that only have a primary and secondary datum. Can you tell me what feature derives the third required plane? Or the many example of composite positions and profiles with the lower portion of the composite only having a single datum, what feature derives the second and third plane? Many parts do not have features to create a nice 3 plane DRF, and if we try to force them to, we only induce biases.

 

[SteveMartin]

Since you asked for the rest of it...

I am only familiar with the 1994 standard (haven't had a chance to read up on the latest yet), so some of this may have been clarified in that document.

I don't know what surfaces the profile tolerance is supposed to apply to. My guess is that it's intended for the three radii and not the three flats, but I'm not confident in that guess. I think it could use an 'all around' symbol, or an A to B indication. If it's just an A to B, then the remaining surface(s) need their own control(s), which may well be a second profile.

There's no thickness defined associated to the datum B callout.

I find the datum A callout unclear how you're supposed to restrain the part/determine your DRF. Just because an irregular feature 'can' be a datum doesn't mean it 'should'. Do you really contact the whole surface with the mating part, or does some portion contact and the others clear? If you do need/use the whole complex surface I think you may need to go beyond just symbols and have a note explaining how to hold A. I haven't given it a lot of thought, but I can't figure out how to fixture on datum A.

 

[TrailMaker004]

Thank you all for your valuable input. I did get the answer I sought.

I agree, an A to B indication should be included to define the extents of the profile.

Steve, I do not believe one would not be able to fixure to this datum surface. A DCC CMM with scanning software such as PC_DMIS CAD ++ must be used. The CMM would "pepper" the entire surface of datum A, including the (3) radii and the (2) short flats on each side with a scan of 50 to 100 points. The software then compares the point cloud scan to the model. Then to align, the software does a "best fit" alignment to the cad model. With this part, the pitch, yaw , and roll are constrained though that. A vertical midplane is also established setting the "X" origin. The "Y" origin is established by datum B. The flat bottom surface is non functional so we thought it unnecessary to associate a datum to it. In the application, the part will locate and orient itself entirely off surface A. The mating interface has the inverse profile of surface A, so the entire surface of A is important. The two holes must also align reasonably with holes in the mating part. The mating part is dimensioned similarly, using the inverse profile as datum A.

In our industry (medical device) we are seeing more and more parts being designed with contoured mating surfaces, so for us using those surfaces as datums will become more and more common. Fortunately, we do have the CMMs and software necessary for this. Thanks also for pointing out the datum flag should be attached to the FCF not to the leader line.

Thanks again to all for your time and help.

 

[dtmbiz]

I couldn't disagree more.

First of all read 1.1.4 regarding figures in the standard. Not all figures are complete. I would say this is the case for 7-50. The others show cylindrical features of size as secondary datums, with a plane as primary. All cylindrical features of size are considered to have two planes that intersect the axis. When "clocking" is not required, the tertiary datum is not added. Both of the planes in a cylindrical feature of size are not always used. In cases when there is a tertiary datum

A datum is a theoetically exact, point, axis, line, or plane. (defined by drawing or model)

A "Datum Feature " is identified via symbol relating to a feature in the model or drawing. It is defined by [physical] contact of the feature with a "datum simulater" (eg attribute gage; CMM probe) by which the "simulated datum" is establilshed.
This is not theroetical, it is the consistent positioning of the part to be inspected in the same position and orientation with a consistent origin to measure X,Y,Z; and/or polar coords . This is the DRF concept.

Composite and multi-segment can have less datums in the FRTZF than the PLTZF. The PLTZF defines the DRF with the all 3 planes. Consider the FRTZF as refinement.

Quote:
"Many parts do not have features to create a nice 3 plane DRF, and if we try to force them to, we only induce biases."

Show me one part that does not have the features to create a DRF by the standard's definition: 3 planes.

How do you "force" a part to contain a feature?

"...induce biases"? Do you mean comply with the standard?

Sorry Nobigdeal, but you sound frustrated and maybe venting a little? I have found in my experience that we tend to over complicate many callouts. Some are complicated but stick to the basic concepts, fundamentals and definitions found in the standard and/or company amendment, step thru it logically....

Back to basics....
It would be definitely worth the time to review 4.1 and 4.2.2 of the 1994 standard; 4.1 of the 2009 standard.
DRF=Three mutually perpendicular planes that interesect.

 

[TrailMaker004]

Datum A includes the entire profile surface: the 4.00R, the (2) 25R, and the short flats on both ends. I an sorry I failed to indicate that better.

PC-DMIS CMM software accepts contoured shapes like this as a primary datum. I do not understand exactly how the algorithims work, but conceptually it produces the results we want that replicate the device function. I assume the 3 necessary planes here are formed from the 1) axis of the radii, 2) a midplane of the 5.00 basic and the 3) midplane of datum B.

Keeping in mind the interface function as I described prior, how would you assign the datum structure?

Thanks again to all for their most valuable input.

 

[ptruitt]

There was discussion about fitting a complex surface and some software called "Smart Profile" by Kotem Technologies came to mind. I have not used it, but may use a service provider to evaluate some pre-production castings in the near future. On one of the parts, I want machining on the outside of the part to be relative to a best-fit of the inside as-cast surface of the part.

 

[nobigdeal]

Sorry if I seemed to be venting at all, I was actually enjoying the discussion. I do realize that it is often difficult to read the "tone" when people are posting. I'm one of those weird guys that actually enjoy a lively debate because I think we can learn a lot that way. Sorry if I got a little carried away.

This may be leading a ways off of addressing the original post so I'll try to hold off from sharing too much more. Just a couple of final thoughts...

I agree with your fundamental statements of datums and DRF's. But, I do think that the standard has opened up the possibility of using complex features as datums (para 4.17(b)). I also think that there is a lot of clarity needed moving forward and I'm sure certain industries will push this forward. It will be interesting to see what comes in the next revision of the math standard.

I work for a independent metrology company and we have many customers that have a need to use a complex surface as a datum (or are using profile without datums). I'm very familiar with using software like PC-DMIS and SmartProfile which seem to be on the cutting-edge to handle more complex GD&T. We have successfully been able to evaluate parts with a complex datum or without datums.

I think we have to acknowledge that there is a lot debate about these issues among people that are smarter than I am, including people that are on ASME committees.

As far as examples of parts that don't have an obvious 3-plane DRF, I can't post customer prints, but I'll just mention some types of parts that would present a challenge to defining a 3 plane DRF. One would be medical implantable devices that are completely free-form in shape. Another example would be a custom hearing aid that is the shape of your ear canal. We see many parts that have one flat surface where the part assembles and the rest of the part is completely free-form (these parts are often controlled with profiles and one primary datum). Of course, there are also parts that we get from other industries that lend themselves very well to an obvious 3 plane DRF.

Just curious, dtmbiz, do you accept the idea of having a non-fully constrained DRF? For example, having only a primary datum and controlling the part using profile tolerancing back to the single datum? Just wondering. This is where I brought up inducing biases, what I meant was, if we put datums in the DRF that are not functional, when we inspect the part we will make the part look worse than it functionally is (easier to show than to explain). I'll let you answer if you want, and like I said, I'll try to stay calm and keep from continuing to go down rabbit trails I am fine with what you are saying and I'm sure any prints you would generate would completely comply with the standard. And I do try to be open to having my understanding corrected. Maybe we should start a separate post, although I should probably just get back to work...

Thanks.