Close Window

CLICK FOR ARCHIVES

The Tolerancing Engineer Newsletter - April 2013
...by our client company personnel and James D. Meadows using our ‘GD&T HOTLINE’

REGISTER NOW FOR
A UNIQUE PUBLIC WORKSHOP PAIRING…
both courses presented by GD&T ‘expert’ James D. Meadows

Geometric Dimensioning and Tolerancing [per the ASME Y14.5-2009 and 1994 Standards

...and the Differences between them] (2 ˝ days) December 9-11, 2013 – in Huntsville, AL

and/or (take one or both courses)...

Tolerance Stack-Up Analysis [for Plus/Minus and Geometric Tolerancing]

(2 ˝ days) December 11-13, 2013 - in Huntsville, AL

See details or call (586) 677-0555 to register and inquire about discounts.

 



Subject: Basic dimension conflict?

Hello Mr. Meadows:

A colleague and I are having a discussion about whether there’s a problem with what is shown on the attached snippet of my drawing:



I’m using the slot to define a datum plane “E”. My datum is then used for the true position control of some other features not shown on the snippet. What I’m wondering is whether or not there’s any conflict between the theoretically exact size of the slot (6mm) .2362”, and what is shown as the fabricated size of the slot .2373/.2366?

This situation arises in my CAD system (SolidWorks) because the hole gets drawn to its nominal size of 6mm, yet applying an F8 fit to the hole, (and then converting to a limit dimensions) changes the actual hole dimension to read on the +/+ side.

I know that the ANSI standard says that tolerances are not inferred from a dimension which is basic; but it admittedly looks a bit strange on the drawing. Can you help me clear up the confusion?

Thanks,

Craig

Craig,

Dimensioning the width of the slot at both basic and then as a limit dimensioned size is wrong. Choose one. I’d choose the limit dimension. That has a size tolerance and a position tolerance. The one that has a basic width would need to be profile toleranced, since profile is the only geometric tolerance capable of tolerancing a basic size.

Jim Meadows
 



Subject: Threaded Features as Datum Features

Jim,
Long time no speak.

What is your opinion regarding threads as datums? Is that a loaded question? In my particular case I’m trying to protect the Virtual Condition boundaries between two very long parts that mate together. One part is a shaft with external threads and the other part is a hole with internal threads. The debate is which features would make better datums? The shaft/hole or the thread/thread on each part? My thoughts are since I can calculate the Virtual Condition on a shaft/hole much easier than the Virtual Condition on threads; I’ll make the threads my datum and geometrically control the shaft/hole to the threads at MMC. In my mind, a GO thread gauge could hold the threads and the run-out could be measured on the shaft. The concern is the “slop” between a thread GO gauge and the actual thread size. But I’m allowing for the “slop” as pattern shift because the datum is at MMC. Am I crazy? Not certifiable, but just in regards to this topic. Thanks for the help and happy holidays.

Brian

Brian,

Even though people normally try to avoid threaded features as datum features, it sounds as though you’ve thought it through and have it all worked out.

Good luck.
Jim
 



Subject: SURFACE PROFILE REQUIREMENTS

Mr. Meadows,

I took a training course that you presented at our facility several years ago for GD&T. I have a question that I was hoping you could shed some light on. I have a part with complex curvature that contains no good datum features (see attached). I want to use a surface profile callout as shown applying the control to only the top curved surface, but it’s not clear to me whether or not I need a datum A (which would be the bottom curved surface) listed in the feature control reference frame. Would you please explain the best approach for this example along with your rationale? What is the difference between using datum A or not using datum A with respect to surface definition and inspection?

Thanks for your help,
David




David,

If the profile control is meant to apply “ALL AROUND” or “ALL OVER (to all surfaces in all views) there is no need to reference a datum. Without a datum they can scan the surfaces and allow the computer program to determine if all points reside within the tolerance zone. This would control the size, shape angle and location of the surfaces.

The way you describe the control, it would only apply to that one curved surface (the top), and would only control the shape of that single surface, and the tolerance zone would terminate at the sharp corners. In that case, you might want to reference datums to give orientation and/or location of the surface being profiled from the others.

Jim Meadows

Jim,

So according to the approach described in your 2nd paragraph, you are saying it is acceptable, but not required, to use the other complex curved mating surface as datum A? What are the pro/cons to using or not using datum A? I have a QC guy here that is adamant that datum A be included, so I am trying to get resolution for this design.

Thanks for responding.
David

David,

Referencing datums in a profile of a surface control is optional. If you wish to relate that surface to a datum plane or axis to hold an angle or location, then reference one or more. If all you want to control is the shape of that surface, then don’t.

I’m just surprised you aren’t defining more of this oddly configured part with basic dimensions and profile tolerancing than just that one surface. It seems like you’d want to define the entire periphery with a profile tolerance to control its size and shape, as well as the angles and location of all elements of all of the surfaces on this part. But, I don’t know what the intent of the rest of the part definition looks like, since you only described to me a partially defined part.

You could define this entire part with basic dimensions and basic radii, then give it an all-over profile control that applies in all views. The entire part would then be completely toleranced and it could be done with no datum references.

Jim
 



Subject: GD&T Questions for a long cylindrical part

Hi Jim,

I hope you’re doing well.

I write to you with GD&T questions (as usual). Would you mind reviewing the attached prints (deliberately incomplete on certain features) and letting me know if you’d be interested in helping me?

Q1. What would be your recommendation on holding OD to ID of a long cylindrical part like this?
Q2. I’d like to get your thoughts on positioning Datum D (threads) to Datum C (predrill for datum D threads), which in turn is held to datum B (smaller through hole on center to predrill).
Q3. I'd like to get your thoughts on tying a feature such as Datum E and Datum C to datums A and B(M). I think datum A is a no brainer. Would it be better to position Datum D (threads) also to datums A and B(M), like datum C’s feature control frame?
Q4. I'd like to get your thoughts on GD&T around a slot feature
Q5. A first mating part is attached to the datum A end of the part, keyed by datum E and bolted on via the datum D threads. This first mating part has an arm with a through hole in it, designed to target the .281
hole on the cylindrical part (the .281 hole is shown on sheet 2). A second part, that is designed to mate with the cylindrical part, is inserted through this first mating part (into the .281 hole).
There is a strength concern at the thin wall section around the .281 hole - the GD&T on the .750 OD and .281 hole is meant to reflect this. I understand LMC would be the ideal condition but considering gauging, I thought MMC may be the way to go. Would you agree with the way it is dimensioned?
I took non-important dimensions off – please let me know if you feel you need more info.
Please let me know if we could discuss these questions by email or over the phone, or better yet if you will be in Memphis in the near future.

Thank you.
Ken

Illustration of Long Cylindrical Part:




Ken,

I’m doing well.

Addressing the matter of the order of how the datum features are defined, datum feature B is perpendicular to A. Position isn’t correct there. But, there is some question in my mind whether datum feature A should be the primary datum reference, since it has so little surface area. If something must seat well (3 points of high point contact) on A, then it would make sense. If not, or it is just a stop, well…in most of these coaxiality controls, it could be eliminated.

Positioning The OD to datum feature B works. The only thing total runout would add is a cylindricity (3D form) control to the location control that position gives you, but since the size tolerance is tighter than the geometric tolerance, it wouldn’t even do that.

Positioning C to B works. I won’t mention the same question I have over and over about datum A as primary.

Positioning the threaded feature to C for coaxiality works, but a question needs to be asked at this stage, “Why are you switching datums so frequently?” A good answer would be that the mating feature only interacts with the threads and C, and doesn’t reach into B. Also, we try not to make datum features of threaded features (D). This is especially a good thing to consider, since the slot (E) isn’t positioned to D. It’s positioned to B. Could everything be positioned to B?

The order of the datum references used for the position control for the .750 diameter is especially odd. If the OD is centered to the thread (D) in one direction, shouldn’t it be positioned to the thread in the other? If D was primary, that would happen, then the slot (E) could be eliminated in this control. But, if you want to center the OD to the slot in one direction (let’s call that the X direction), then center it to the thread in the other direction (the Y), then this order (E then D) is correct. I’d hate to have to design a gage to check it though.

Treating an elongated hole as though it is two round holes that somehow got connected by a width is not something we often do. Why not just get rid of the diameter signs and position the entire elongated hole to H and E (in that order-so that E is just controlling clocking/angular orientation).

If I didn’t cover everything, write back.

I hope this helps,
Jim

Jim,

Thank you for your reply. It definitely helps, and I hope you wouldn’t mind if I dive into this deeper:

I have the same concerns with the small surface area of datum A. The reason it was chosen as primary is because unfortunately, it is quite possibly the feature with the largest contact area with the mating part, which I named the “first mating part” in my original email. It has 3 mating features: datum A, datum E and datum D.
Datum E isn’t “mating” per se – it provides rotational clocking so that it can used to accurately insert the 2nd mating part into the .281 hole. As such, it is possible that datum E actually doesn’t make contact with the “first mating part”.
When using this particular family of devices we recommended tightening the bolt that holds the “first mating part” to this “as much as possible by hand”. As such, it is possible that the cumulative contact area between the threads (datum B) and the bolt is larger than the contact surface datum A sees. However, it was not chosen as the primary datum since this cumulative contact area is not quantifiable, and since I am uncomfortable using threads as primary datums in general. Having said this, I still thought it was important to keep it in the Feature Control Frame since it appears to be an important feature to the function of the assembly and hence the part.
I would like to hear your comments on this.

I’m glad to hear positioning the .500 OD and .272 predrill to datum B works. My quality engineer asks how you would inspect this, seeing that datum B is over the majority of the 20” length.

Absolutely, everything can be positioned to B. This again becomes an inspection question.
The reasoning for the threads (datum D) being held to the predrill (datum C), which in turn is held to the ID (datum B) is that this is the order of manufacturing process.
The reason datum E is held to B and not to D is also that datum E is manufactured onto the part separately from the predrill and threads.

Regarding the .750 diameter, I don’t understand your comment “If the OD is centered to the thread (D) in one direction, shouldn’t it be positioned to the thread in the other? If D was primary, that would happen, then the slot (E) could be eliminated in this control. But, if you want to center the OD to the slot in one direction (let’s call that the X direction), then center it to the thread in the other direction (the Y), then this order (E then D) is correct.”
This may not matter, but here’s the background. I focused on the GD&T around the .281 hole first. Then, I used the same GD&T on the .750 OD because there is a strength concern in the relationship between the .281 hole and .750 OD.

Thank you again.
Ken

Ken,

To address the last thing first, when the OD references A/E/D, A serves as a perpendicularity datum, E centers the OD to the slot centerplane and D centers to the axis of D in the direction that E hasn’t controlled. This is unusual. Normally, you would want to center the OD to the axis of D. This would eliminate the need to reference E, since, at that stage, it could only serve the purpose of anti-rotation of the OD and that isn’t needed.

The order of the manufacturing processes for the assignment of datum references is really a minor factor. This isn’t a process engineering drawing. It’s a finished product requirement based on functional needs. Every time you change datums, you accumulate tolerance error, and if one of your concerns is wall thickness, it could adversely affect that. If one datum feature is used, such as B, to center everything, then one gage could be made to inspect all features referenced to the same datums (as a simultaneous requirement). That’s if they want to gage it. If not, one set-up would be required to measure everything that is referenced to the same datums.

One thing that is gnawing at me about the comments you are making, is that it seems you are allowing the manufacturing and inspection people to dictate how you are specifying your functional requirements. That only works if the changes you make to appease manufacturing and inspection results in a product that is just as functional. If not, if it was me, I’d insist that the functional requirements not be abandoned.

My comments on using datum A as a primary datum remain the same. If A is needed to dictate the angle at which the parts assemble, then use it, and use it as primary (or else it’s useless). If A is just a stop, then don’t use it, if all you are trying to control is coaxiality of one diameter to another. If the parts are to be gaged, a threaded feature as a primary datum feature isn’t difficult to simulate.

It sounds from you description of how the part works that, for the hole that becomes H, since E is only being used as a datum to stop rotation, it must be used after the datum that is to be used to locate/center the other diameter(s). In this case that would mean that instead of E/C, it should read C/E.

There’s probably a bit more I should comment on, but I'll let you think about this for now.

Jim
 



Subject: Virtual Condition question on I.D.'s

Dear Mr. Meadows,

My name is Eric and you taught a class at our company in Chicago, Illinois last year. I have a question because I am not sure of something.

We have a part that has two concentric bores. One bore is labeled Datum –B- and is 3.379-3.378 in size. The other bore is 4.251-4.250. Based on the attached PDF what would the VC of the 4.251-4.250 be 4.249 at MMC with the 3.379-3.378 bore at 3.379 due to the bonus tolerances?

4.250 (Bore at MMC)
-.000 (bonus tol on bore size)
-.001 (bonus tol due to 3.379 size on the 3.379-3.378 bore)
=4.249

Thanks
Eric



Dear Mr. Meadows,

Thanks for the clarity. The Datum feature B would have a perpendicularity control of .0005 relative to A. My intent is to setup the part so that a functional gage could be designed and used for resting on Datum A and would check Datum B and 4.251-4.250 bore positions. FYI, the Datum surface A, B, and the 4.251-4.250 features are machined in the same setup.

I get:
4.251 = LMC of counterbore
+.001 = Geo. Tol. @ LMC
4.252 = Outer Boundary of counterbore
+.001 = Pattern Shift Datum B M
4.253 = Outer Boundary counterbore w/ shift
+.0005 = Position of Datum B
4.2535 = Outer Boundry of the counterbore

4.250 = MMC of counterbore
-.000 = Geo. Tol. @ MMC
4.250 = Inner Boundary of counterbore
-.001 = Pattern Shift Datum B M
4.249 = Inner Boundary counterbore w/ shift
-.0005 = Position of Datum B
4.2485 = Inner Boundary of the counterbore

Thank you,
Eric

Eric,

4.250 is the virtual condition as defined in the ASME Y14.5 standard. Virtual condition for a hole is; the MMC minus the geometric tolerance that applies at MMC (4.250-.000=4.250). The datum feature shift derived from using a circled M after datum feature B is often a factor in calculating tolerance stacks where this hole is one of the pertinent features in the stack, but the virtual condition definition does not include that shift. This is just semantics. If the datum feature/pattern shift is a factor in your calculation, use it. Just don’t call the result a “virtual condition”.

As an aside, unrelated to this discussion, the datum feature B needs a perpendicularity control relating it back to datum plane A. Without it, datum feature shift and the virtual condition of datum feature B wouldn’t be possible to calculate.

Jim Meadows



 

Close Window

© 1997-2015 James D. Meadows & Assoc., ALL RIGHTS RESERVED

Site Designed & Maintained by VIRTUAL GOLDMINE