Close Window

CLICK FOR ARCHIVES

The Tolerancing Engineer Newsletter - June 2016
...by our client company personnel and James D. Meadows using our ‘GD&T HOTLINE’

Subject:True Position and Datum Selection Question



Hello James,


I'm a junior engineer and I just learned that we have access to your services with respect to
GD&T related questions.

I have attached a drawing I am currently working on. There is a true position callout for a dowel pin hole. The hole has a press fit with the pin and is going to mate up with a plate our customer has designed. The .002 tolerance at Maximum material condition is based on the tolerance they specified on the mating hole, but I'm unsure how best select datums to define my tolerance.

Currently I only have a datum A on the axis of rotation, which is used by other GD&T, but I know dimensionless to an axis of rotation is not good practice. I have considered making the OD of the large portion of the shaft a datum, but the OD currently has a lose tolerance so it does not
make an ideal choice.

Could you guide me as to what would be good datums that would be actually useful for machining and measuring? Thanks in advance for your assistance.

Christopher


Christopher,

Yes, putting a datum feature symbol, in this case A, on a centerline is illegal and ambiguous. Location basic dimensions are required for every hole location, and some kind of coaxiality control, like runout, is needed on every outside diameter of the part.

For example:



This is a simple illustration from one of my textbooks that should get you started. Your part drawing needs so much done to it, that to be more specific, I’d have to tolerance the entire part.

But, a good example of guidelines to follow when selecting datum features for parts such as these is given below:

STEP 1:
Find the primary datum feature by asking; “What surfaces seat?” or “What surfaces need the most physical contact when assembled?” or “What surfaces dictate the angle at which these two parts will assemble?” or simply, “What surfaces are we trying to bolt to?” The answer to these questions should all be the same.

STEP 2:
A secondary datum feature must be selected. Since the primary datum features have a lot of surface area and will stabilize the parts when holding/measuring other geometric relationships for angles and location, the secondary datum feature need not have as much stabilizing ability. It will be to locate other part features from, while the primary controls the perpendicularity of those features.

The secondary datum features will be chosen on the basis of; “What features mate and/or align the assembly?”

STEP 3:
The next step on each part is to tolerance the hole patterns. The important relationships that we must tolerance are:
a) Hole to hole distance (a basic bolt circle and the basic angles between the holes or pins)
b) Perpendicularity to the primary datum
c) Distance out from the axis of the secondary datum.

STEP 4:
Step 4 would require a coaxiality-type control be applied to the outside diameter of each feature that is not used as a datum feature. These controls would reference the same datums as the position control on each part. To center the outside diameter of each part to the datums shown, a control such as runout, total runout, concentricity or position could be used. This last control would act to complete the Geometric Tolerancing Scheme.

Granted these guidelines are generic and can change given the specifics of each part and whether more than one datum scheme is used. If more than one datum scheme is used, such as in the illustration from my book above, then the datum reference frames must be related to within a tolerance to each other.

An example of an assembly that follows these rules is shown below.



Assembly Illustration of Parts 1 and 2




James

 




Subject: Datum and Profile Question


Hello again Jim,


Hope all is well with you.


I’ve run into a small problem with a connection shape and its GD&T.







This image contains a close look at the area in question. The datum structure of this connection comes from an existing source and after a bit of review by Doug and I we thought Jim meadows may be able to point us in the right direction.

Starting at the beginning, Datum A is defined as the diameter of the connection geometry, no issues with that. Datum B defines its angle (30°) and distance (8.01mm) with a ‘Profile of a line’ control using Datum A as reference. Then the opposite and symmetrical ‘right hand side’ of this connection shape is controlled with and angle (60°) and a ‘Profile of a surface’ control using Datum A as primary and B as secondary.


This second, surface has us a bit confused. Why use profile of a line on one side and profile of a surface on the other? This entire shape is a surface that runs 19mm deep, wouldn’t we want to use profile of a surface on both?


Our second question in regards to this connection geometry is whether or not the ‘right hand side’ surface is even defined fully. The 60° defines the angle but doesn’t the 8.01mm distance need to be present as well?
Thanks in advance!


Best Regards,


Patrick


Patrick,


Your question about using profile of a line on one surface and profile of a surface on the other is a good one. I can't think of a reason they would want that. It's probably just a mistake. Can you ask them?


In the other view you sent (not shown here), it appears that datum feature E has been crossed out, but continues to be referenced in other feature control frames. That needs to be corrected.


And it seems that D needs a basic dimension and a datum reference to locate it in the left to right direction of the view in which it is depicted.


In the view shown here, datum feature A isn’t related to anything, but other features are related to it, which is fine, but there are a lot of features on the periphery of the part that have not been related to A. Usually, if a hole is the first datum feature, then the periphery of the part is profiled to the hole. Otherwise the hole is first positioned to the outside of the part. Neither has happened here. So, it doesn’t appear that any locational relationship exists, within a geometric tolerance, between the two.


James

 



Subject:Re: Movable Datum Targets


Hi Jim,


I have read over and over and over again pages 333-335 your Gray Book on Moveable Datum Targets, I have also read ASME Y14.5-2009 definition of Movable Datum Targets and when to use them and I also read ASME Y14.8-2009 and I still can’t grasp the definition of when and how to utilize them, what does it add to the dimension , “it is an optional clarifying symbol to indicate movement of the datum target simulator” that is verbatim from your book, how and when and how does the datum target simulator move in respect to the moveable datum targets, are the datum targets at all associated with the feature it is attached to and how does it add clarity when I and a lot of others don’t know how to use or define it, I mentor the designers and engineers with regards to GD&T , I explain GD&T and give definition to the language and advise them to purchase your book to better understand for themselves.


Hubert


Hubert,
I reread the pages from my book defining moveable datum targets. The only thing I can add is that they are used to stabilize inherently unstable parts and are needed because, if they were stationary, the part either wouldn't fit into the fixture, or the part would drop past the target simulators and not be stabilized at all. This works similar to a vice. Vices have one fixed jaw and one moveable jaw to be able to grip the part and hold it in place. That's the way the fixture would work with moveable datum targets. The only difference is that the moveable elements of the fixture would have to contact the surface by moving in and contacting the surface at 90 degree angles.


Here is an illustration from my GD&T 2009 textbook:


FIGURE 16-13 [Moveable Datum Target Symbol]



The following illustration shows a viable fixture within which the part may be mounted to simulate the datum targets.



FIGURE 16-14 [Workpiece Mounted in Fixture]



Moveable datum target simulators for C1 and C2 slide through tight fitting holes on the fixture and contact the part surface normal to the desired geometric configuration.

Hope this helps.


JamesMeadows


 



Subject: Specifying Axes and Overriding Degrees of Spatial Freedom


James,


You taught a GD&T class at my company before we converted to ASME Y14.5-2009. We recently switched to the 2009 standard and there is a new tool we are able to use where we specify the datum axes on the drawing and are then allowed to limit the degrees of spatial freedom that datums can control. First off, what are the degrees of freedom officially called and then how can we use this tool to limit which of them a datum can control.


John


John,
Here is an illustration from my GD&T 2009 textbook that shows what the degrees of spatial freedom are now officially called.


FIGURE 11-2 [Datum Reference Frame showing Six Degrees of Spacial Freedom to be Stabilized for any Part Configuration]

Only the datum axes may be specified on the field of the drawing as capital letters X, Y and Z. Then the spatial degrees of freedom may be specified as lower case letters in brackets after any datum feature referenced in the geometric control (feature control frame). This can override the ability of that datum feature to stem all of the spatial degrees of freedom that it would normally control, and allow another datum feature to subsequently be referenced to control the remaining degrees of freedom.
Here is an example of a cone’s z degree of freedom, which would normally require a basic dimension from the apex of the cone to locate the part’s hole, to be overridden by a secondary datum (B). A basic dimension is then given from datum B to locate the hole.


The following illustration shows a conical datum feature. In the position feature control frame the spatial degrees of freedom that each datum reference controls are listed in brackets after the datum reference.



a. What controls the rotational spatial degree of freedom (around the Z axis) known as w? Nothing
b. If datum feature B was referenced as primary instead of secondary, would it be necessary to specify the bracketed z after B in the feature control frame? No
c. If datum feature B was not referenced in the position control and no degrees of freedom were specified after datum feature A in the position control, how would the dimensions on the part drawing change? The 24mm basic dimension would go away and be replaced by a basic dimension from the apex of the cone.

I hope this helps.


James

Close Window

© 1997 - James D. Meadows & Assoc., ALL RIGHTS RESERVED

Site Designed & Maintained by VIRTUAL GOLDMINE