Smart questions
Smart answers
Smart people

Member Login

Remember Me
Forgot Password?
Join Us!

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips now!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!

Join Eng-Tips
*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Donate Today!

Do you enjoy these
technical forums?
Donate Today! Click Here

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.
Jobs from Indeed

Link To This Forum!

Partner Button
Add Stickiness To Your Site By Linking To This Professionally Managed Technical Forum.
Just copy and paste the
code below into your site.

EnglishMuffin (Mechanical)
4 Nov 06 0:28
Suppose we have a cylinder, with an off-center slot extending right across one end face. Suppose the surface of that end face is defined as Datum A, and that the axis of the cylinder is defined as Datum B by using a datum callout on the diameter. Also, suppose one side of the off-center slot is defined as Datum C, and that its radial location  from the centerline of the cylinder is specified with a toleranced dimension of some sort. Now suppose that, using a positional tolerance, it is required to locate a circular set of six holes in the said end face, such that the hole pattern is centered on the axis of the cylinder (Datum B) and is angularly aligned using the full length of the slot (ie Datum C) in some specified manner.
If in the position tolerance frame we use the three datums A, B, C in that order, it would contradict the required 3 point/2 point/1 point rule used to define the datums in the ANSI standard, since C requires two points because of the fact that we desire to use it to define a line for angular orientation. (This does not lead to ambiguity in most of the examples shown in the standard and other texts, because they always show very short slots which in conjunction with Datum B can then provide a localized single point angular locator without ambiguity). If on the other hand we use the sequence A, C, B, as the standard seems to require, would the position tolerance then be referenced relative to a point at the intersection of datum C and a perpendicular lying on Datum A and passing through the cylinder centerline (defined by datum B)? If so, that would of course not meet the original intent. Or is it the case, as I have been told by certain others, that the position tolerance would be implied to be referenced to the B datum with C used to define only the orientation? I realize I am probably displaying my poor understanding of G D & T here. However, any comments ?
EnglishMuffin (Mechanical)
4 Nov 06 0:48
Actually, I've just noticed on this recent thread1103-169440 that the ANSI standard section 4.4.2 seems to indicate that it should be A,B,C in this case. But still interested in any comments.
Helpful Member!  drawoh (Mechanical)
6 Nov 06 13:37

   Your datum system is described explicitly in ASME Y14.5M-1994.  See figure 4-6.  Datum A locates one face, Z, at whichever three points stick down the furthest.  Datum B is a feature of size which locates in X and Y.  You should consider calling up B at MMC in your tolerance boxes.  Datum C is a face that controls rotation.  

   The ABC datum system immobilizes the part.

   Your ACB specification is different.  A locates the Z face.  C locates the X face, and B becomes a feature of size that locates the Y face.  Again, you must consider an MMC specification when you call up datum B.  I think this is a weird way of doing things, but perfectly legal.  If the holes must be located accurately with respect to the slot, it may even be a good idea.

   ACB immobilizes the part too, but in a different location.

EnglishMuffin (Mechanical)
6 Nov 06 20:05
Thanks Drawoh.

This question came up because of an argument between two people, and one of them casually asked my opinion. Person #1 is the best expert we have in the plant and is GD & T certified at technician level (he operates our large CMM and consequently gets heavily into the subject on a day to day basis). Person #2 is a representative of a large corporation for whom we are making the part in question. The actual part actually does not have an off center slot - it has two in-line short slots symmetrically disposed either side of the B axis, and which form a common datum C. But to frame the argument more clearly I am specifying the slot to be a single long one offset from the B axis. As I see it, the reasoning for both situations should be basically the same.

 Person #2 says it should be A, B, C. On the other hand, person #1 says (as I understand him):

1. Datum A is located by 3 a minimum of 3 points
2. Datum C is located by a minimum of 2 points
3. Datum B defines two planes regardless of whether it is placed in the second or third box on the callout. I think he also is implying that he would then locate B with a single point (minimum) at the center of the part.

He therefore argues that C should precede B. If he is actually right about statement "3" then that would conflict with your statements about the ACB sequence being different - the holes would aways be referenced to the B axis in two orthogonal directions.

I'm afraid I don't have a standard at my fingertips so I am unclear how much importance should be attached to how many points are needed and their exact relevence to datum precedence. But it would seem to me that once A is defined with 3 points, one can then go on to define B with 1 point, and one has now fully defined the location of 3 planes in translation, with two of them yet to be defined in rotation (although their relative perpendicularity to each other has already been covered). You could stop there if the hole pattern was not required to be oriented to anything, or if one of the holes was required to be a datum you could then orient the planes using one more point. So one could set everything up in that case with (3,1) points or (3,1,1) points, and in the original case with the C slot it would be(3,1,2) points. In this latter case, none of the planes go through "C". In the case of an A,C,B callout, one of the planes would go through C and the remaining plane would go through B and be perpendicular to C. It would appear to me that the 3,2,1 convention is only a guide, and does not always apply religiously, especially with round parts.

That's how I see it anyway, and I think it agrees pretty much with what you are saying. So with person #2, that makes three of us. But I guess it all comes down to whether person #1 is really correct in claiming that the "B" callout defines two planes intersecting the axis of the circular part, regardless of whether B appears in the second or third box, and whether the 3,2,1 point convention has to be slavishly adhered to. Note that on the thread I referenced on my second post, the statement is made that  section 4.4.2 says the datum planes always intersect on the axis, which if correct would partially support person #1.

Not being really familiar with the standard, I would be interested in your further comments and/or anyone elses.

ringman (Mechanical)
7 Nov 06 8:26
I believe that a problem that you are encountering is at least in part due to using ONE SIDE OF THE SLOT, as a datum feature, C.  The situation would seem to work better if only a point on the surface were designated as a datum feature.
It is difficult even on a computer to 'orient' a line to a surface.  By definition orientation requires a point.

That would serve to satisfy the orientation of the part more adequately and fit with your 3,2,1 point precedence considerations.

My opinion: A primary, B secondary, and C tertiary.

EnglishMuffin (Mechanical)
7 Nov 06 8:55

I don't see how you can angularly orient the two planes through B, using the orientation of C, with only one point, regardless of whether C is defined as only one side of the slot or the slot feature itself. With the A,B,C designation, the third plane does not necessarily pass through C, (whether it is actually offset from the center or not), so you you would have to use a minimum of two points lying on C in order to define its angle, at least as far as I can see.
But at least so far we all seem to agree that it should be A,B,C.
ringman (Mechanical)
7 Nov 06 9:20
Orientation is accomplished by the theroetical line thru axis B and point C.  There of course would have to be an angular relationship specified for the mutually perpendicular planes that are associated with axis B.

EnglishMuffin (Mechanical)
7 Nov 06 11:11
ringman - C is derived from an off-center feature (the slot)- so as far as I can see, you cannot angularly orient the two axes through B using C, with only one point on C - you would have to use two points - both of them on C. Drawoh seems to be in agreement with this, unless I misunderstand him. Even if C were a short slot at the periphery, as is so often shown in examples, it would seem to me that this still implies that strictly speaking one should use two points on C, although that would not lead to very satisfactory results in practice. I would have thought that if, on the other hand, the intent were to orient the axes through B the way you describe (which would work for a short radial slot) then the callout should strictly be A,B,B-C. But I could well be wrong - I don't understand G D & T very well - hence my confusion.
ringman (Mechanical)
7 Nov 06 12:10
Orientation is accomplished by the theoretical line thru axis B and point C.  There of course would have to be an angular relationship specified for the mutually perpendicular planes that are associated with axis B.
 (Copied from above with theoretical corrected.)

You are sorta right.  One point will not orient.  you have to have the B axis and the association of C as a point with a specifiied angle to orient.

Think of it if you will: Equator= Datum A, North Star and Earth = axis B,  Grenwich UK, prime meridian, = Datum point C.  Does that work at all for you?
With those you can navigate to WHEREVER.

You do know how to incicate a single point as a Datum feature rather than the entire surface?
kbro151 (Aerospace)
7 Nov 06 12:31
For this particular part, couldn't you use the center of one of your holes as datum C?  Then you could control the hole pattern and slot location to your satisfaction, and there would no longer be an arguement about how to define C or how many points it should take.
drawoh (Mechanical)
7 Nov 06 12:37

   Look at the drawing.  If the drafter shows the datums in order as A,B and C, then B is the secondary datum, and C the tertiary datum.  If the drawing shows A, then C, then B, C is the secondary datum and B the tertiary.  This has nothing whatsoever to do with the geometry.

   Both schemes are valid for the drafter, and they are different.  If you are reading the drawing, the precedence is whatever the drafter indicates.

looslib (Mechanical)
7 Nov 06 12:51
One of things I was taught in GD&T training was to think like the person inspecting the part and put the datums in the order that you would for locating the part for inspection.

"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli
Sr IS Technologist
L-3 Communications

EnglishMuffin (Mechanical)
7 Nov 06 12:52
ringman: I don't think you quite follow me - the slot does not go through the B axis - you cannot determine its orientation with a point on B and a point on the slot. And when you do determine it, as I understand it, you are supposed to be able to do it with points only, according to the standard. A minimum of two points on C should define the angle. Certainly if you are setting up a CMM, you always have to use points. And as I understand it, the standard does not allow you to use an "angle" to determine a datum directly from a surface unless the angle is first determined in terms of two or more points on the surfaces concerned.
EnglishMuffin (Mechanical)
7 Nov 06 13:10

I am not disagreeing with you - I am in conflict with person #1, but I don't know enough about the standard to know if it is being interpreted correctly or if there is something wrong with it. The issues boil down to this:

1. If you make B the secondary datum and C the tertiary, is  there a problem with the fact that you have actually utilized 3 points followed by 1 point followed by 2 points in defining the reference planes? Person #1 says there is, and it conflicts with the standard.

2. If you make C the secondary datum and B the tertiary, person #1 says that, according to the standard, B still defines two reference planes through the center of the part (ie intersecting on B) - whereas you (drawoh) seem to imply in your first post that this is not the case (ie one of them according to you goes through C). (This is what I would have said too).

Can you site exactly which paragraphs of the standard either confirm or contradict these positions ?
ctopher (Mechanical)
7 Nov 06 13:15
If you can show a pic, it would be more clear. I have trouble following the wording.

Systems Analyst, I.S.
SolidWorks 06 4.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 10-27-06)

drawoh (Mechanical)
7 Nov 06 13:20

   Let us assume that the drawings calls up Datums ABC.  My fixture consists of a base with a machined round pocket, and an aligning bracket.  

   The bottom flat face of the pocket defines Datum_A.  

   The diameter of the pocket is the maximum allowable diameter that defines B.  An MMC specification on B allows the part to move around a bit depending on the diameter tolerance.  If your tolerances do not call up B at MMC, you are going to have to shim your part in place, or make the B diameter very accurate.

   The part is now located in Z, X and Y.  It can still rotate.  

   There are several ways the drafter can treat your slots.  You can have a pin that picks up both faces of one slot.  You probably should call up this datum_C at MMC.  You can have an accurate sliding bracket that picks up one face of each slot, which does not require an MMC specification.

   Let's try again, this time with Datums ACB.  The fixture is now a rectangular pocket with two pins sticking up.

   Datum A is the bottom face of the pocket.

   There are again two ways for the drafter to treat your slots.   They can have each pin contact both sides of each slot at MMC, or they can call up one side of each slot to contact the pins.  We do not care where the other side of the slot winds up.

   Your part now is constrained in Z, X and rotation.

   The width of the rectangle locates the diameter of your part at MMC, defining the tertiary datum_B, and locating your part in Y.

   In the second scenario, if the slots are not located accurately to the diameter, your holes could be way off centre and still pass inspection.

   What is your part supposed to do?  If the holes must be centred on the diameter, then your drafter should have called up ABC.  If the holes must be located to your slots, then your drafter should call up ACB.

   Datum precedence is not the shop's decision.

ewh (Aerospace)
7 Nov 06 13:45
Very good explanation, drawoh.
ringman (Mechanical)
7 Nov 06 14:20
"Also, suppose one side of the off-center slot is defined as Datum C," (From orig)

I believe that this rules out the gaging using a pin to locate BOTH faces of the slot.

I understand that the slot does not align with the axis.  That is the reason for using only one point along with the B axis and a specified angle to fis the part for inspection.  

Then you could follow drawoh's explanation, with the exception of a single pin for orientation.
EnglishMuffin (Mechanical)
7 Nov 06 14:29

Well - I guess I am still not really getting my point across. I don't have a problem with anything you have said - I am not the person saying it should be A,C,B. The issue is not whether a particular interpretation makes sense, but what the wording of the ANSI Y14.5M - 1994 standard actually says and whether it makes sense. Is it, or is it not, stated in the standard that when a part is primarily round, with datum B (say) defined based on the round feature, that this always defines two of the orthogonal reference planes and that they both go through B (i.e. regardless of whether B is used as a primary secondary or tertiary datum)?. Person #1 says yes. I personally have no idea - is this statement contained in section 4.4.2 as someone says in thread 1103 - 96440 ? If this were actually the case, then it would effectively imply that A,B,C would be indistinguishable from A,C,B (disregarding the 3 point/2 point/1 point issue), wouldn't it ?
EnglishMuffin (Mechanical)
7 Nov 06 14:41
ringman: The point is that I am assuming that it is specifically desired to orient the pattern of holes so that one reference plane is parallel to C - at least, that is apparently the design intent of person #2's drawing. This part (which is actually quite large) is being checked on a CMM - there are no gauging pins involved.  I have heard the comment made that one of the problems with the ANSI standard in general seems to be that it was originally set up from the point of view of someone using functional gaging, not a CMM.
ringman (Mechanical)
7 Nov 06 15:37
What is the distance from the center of Dia B to the side of the slot and precisely how is it controlled?

Any way you can provide a sketch?

Again I will restate there is a  distinction to be made between orientation and alignment.  This may be the point of confusion between your Tech. and the Company Rep.

Personally I think the drawing as you state it has problems.
drawoh (Mechanical)
7 Nov 06 17:24

   If the drawing calls up ACB as the datums, in that order, the diameter only defines one plane.  The first plane is datum_A and the second is defined by the slot.  If you do not impose datum_C, the housing is free to wobble from side to side on one direction only.  

   This three points, two points, one point thing is for datums defined by flat surfaces.  It has no meaning when you use a diameter as a datum.  The diameter is a feature of size, which is why I kept mentioning MMC, above.  The slot too can be a feature of size, depending on how your drafter calls it up.   

ringman (Mechanical)
7 Nov 06 17:46

I believe that Datum feature B, in this case, is related to an axis regardless of the sequencing, and not a plane.

EnglishMuffin (Mechanical)
7 Nov 06 18:09
Now we might be getting somewhere .... which one of you is correct ? What exactly does the standard say ? I think conceptually and logically it ought to work the way drawoh seems to think, but the impression I get is that the standard is actually written the way ringman says. I also think conceptually that drawoh's view that the 3/2/1 thing only makes sense with flat surfaces makes perfect sense - but again - what does the standard actually say ? I have no clue - I don't have one. That is the big issue with Person #2 - the standard. I am neither person #1 nor person #2 - I am person #3 - i.e. an interested bystander. Also, there is no "drafter" involved in the argument - only a drawing provided by person #2, which Person #1 is trying to interpret and measure.
ringman (Mechanical)
7 Nov 06 19:55
If you prefer to think in terms of 3,2,1 points, try this;  Datum A, plane, 3 points,  Datum B, axis 2 points, (determines a line) and Datum C a single point rather than 2 points for orientation.

Again the example would be helpful in either case.

Sounds like the drawing needs changing, but if I understand you are stuck with it.  Been there, done that.
drawoh (Mechanical)
7 Nov 06 22:33

   ASME Y14.5M-1994 is a practical standard.  Theoretical planes and axes are useless as fixturing devices because they do not exist.

   If your datums are three orthogonal, flat surfaces, you can design a fixture with three real planes that make contact with your datum surfaces.  The three planes shown in the ASME standard are real metal surfaces that you can measure from.

   When you call up an outside diameter as datum, your point of measurement is the inside diameter of your fixture.  You can visualize planes and axes, but these are imaginary.  Reality is a hollow, round piece of metal.  Since there is a clearance between the hollow, round piece of metal and your part, you usually need to call up the datum at MMC.

ringman (Mechanical)
7 Nov 06 22:56
Many drawings require theoretical planes as the basis for dimensioning. Part in discussions involves the use of the axis and the mutually perpendicular planes associated with it in this case.

I agree you will not see the 'theoretical planes and lines' on the gaging or fixturing devices, but they are necessary evil,in the overall scheme.

ewh (Aerospace)
8 Nov 06 9:44
The 3,2,1 datum scheme is indeed for more than parts with flat planes.  While they do represent planes, those planes do not have to exist on the part except as datum points.
btrueblood (Mechanical)
8 Nov 06 12:09
Not clear to me you need datum A (face of cylinder) referenced at all, other than to control the depth of the holes.  To locate the holes on the endplane of the cylinder, with datums A=endplane, B=cylinder diameter, C=slot face, I'd call out the datum sequence as BCA, or just BC if the holes were "thru".
drawoh (Mechanical)
8 Nov 06 12:23

   This is a fundamental mental block with GD&T as per ASME Y14.5M-1994.  You must immobilize the part.  Your primary datum should be the best available fixturing feature of the part.  This this case, it is probably the flat base of the part.  

   Your datums are fixturing points, not dimension bases.  Of course, it is desirable to dimension from your datums, but not absolutely necessary.  

ringman (Mechanical)
8 Nov 06 12:34

Was the last statement a typo or just a slip.  I believe that datums are the basis for dimensions within the realm of Y14.5. "Best as I recall"
drawoh (Mechanical)
8 Nov 06 12:45

   My phrasing was not very good there.  

   It was suggested that the required datums were B and C.  The logic of this is that these two datums are sufficient to locate the holes and slots.  This is a logical point of view, and it was certainly my first impression when I started applying GD&T specs. to drawings.  It is wrong.

   The features must be located with respect to the specified datums.   There is no absolute need for the dimension lines to emanate from the datums, although it is good practise.

ewh (Aerospace)
8 Nov 06 12:56
Don't the features still have to be tied in some way back to the datums with basic dimensions?  Otherwise, wouldn't you be introducing tolerances other than those in the FCF?
JohnNabors (Mechanical)
8 Nov 06 15:53

Any way you could post the actual drawing in question?
ctopher (Mechanical)
8 Nov 06 16:03
That was my suggestion also.

Systems Analyst, I.S.
SolidWorks 06 4.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 10-27-06)

drawoh (Mechanical)
8 Nov 06 16:14

   For example, if the holes at the bottom of this thing are specified as a pitch circle, there is no explicit link to the datums.  They can be inspected from the datums, which is what matters.

btrueblood (Mechanical)
8 Nov 06 16:34

Not sure I follow you.  The axis of the holes are aligned with the cylinder axis, as I am envisioning the part, and  presumably, like a pipe flange, the holes are intended to be symmetric with the axis of the cylinder.  Fixturing on the flat surface does you absolutely no good for inspection, since it may or may not be perpendicular to the axis of the cylinder.  Also, if the holes are blind, you'll not be able to see, much less inspect/indicate to the holes if the datum A plane is lying at rest on a granite surface plate.  

I think, after re-reading, I follow you:  it's not up to the inspector to pick the datums, it's up to him to follow the drawing, and use the order of precedence stated on the print.  Agreed.  But I will continue to design my flanges referencing the cylinder axis as a primary datum; it's my part, make it my way! :)
ewh (Aerospace)
8 Nov 06 16:35
As long as there is an implicit link, such as a common center, or there is no FCF controlling the pitch circle.  If there is, the pitch circle either shares a center with a datum feature, or should be located by basic dimensions to a datum.  True position is established by basic dimensions per Y14.5.  I have seen no exceptions to this in the standard, but am interested to know if there are any.
ringman (Mechanical)
8 Nov 06 17:37

In your statement previous about the pitch circle.  What is the pitch circle related to?  What Standard are you currently using for GD and T interpretation?
Do you have access to either ANSI or ASME Y14.5?

Is there perhaps a company Standard that applies to your drawings?

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!

Close Box

Join Eng-Tips® Today!

Join your peers on the Internet's largest technical engineering professional community.
It's easy to join and it's free.

Here's Why Members Love Eng-Tips Forums:

Register now while it's still free!

Already a member? Close this window and log in.

Join Us             Close