Using width and length of a recess as dimensioning datums. 2

[Tunalover]

Folks-
I often work with designs where a rectangular panel is mounted to a hole pattern within a rectangular recess. The rectangular panel is usually carefully sized to closely fit inside the recess when the holes come in at worst-case tolerance conditions. If I were to use the length and width of the recess as secondary and tertiary datums, would I take all dimensions from the CENTERLINES of those two features? If this is legal, how would this be handled in inspection? Is this an inspection nightmare? It seems to me that one could gain bonus tolerances by invoking the positional tolerances when the length and width datums are at MMC.


Tunalover

 

[MintJulep]

Tuna,

I don't think you've given us enough to go on here.

Are the holes in both the panel and the recess clearance holes with a thru fastner and nut on the back, or are the holes in the recess threaded, or something else?

I would suggest not using the center line, as imaginary features do tend to be a pain for inspection.

 

[ewh]

Imaginary datums are poor practice. If the length and width are used as datums, the part would be inspected relative to the center planes of the datums, which would not be imaginary. To DIMENSION to the centerlines of the features will only cloud the issue.

 

[drawoh]

tunalover,

The easiest way to understand datums is to keep asking yourself how you would mount this thing for inspection. Datums on the mating part cannot work, especially if it is being fabricated in another shop.

The problem with dimensioning from centrelines is that your tolerance usually are ambiguous. This is not the case if you use positional tolerances.

I see two strategies for dimensioning your panel.

Apply +0/-something dimensions to the length and width of the panel. Apply basic dimensions to the clearance holes. The mount face is datum A. Datum B is across the width. Datum C is across the length. I apply two positional tolerances to the holes. The first is applied WRT datum A, and it is accurate enough to align the holes with the mating holes. The second WRT datums A, B and C ensures that the holes are positioned WRT the outline accurately enough that the panel fits into the pocket. This second tolerance should apply at the MMC of datums B and C.

Apply basic dimensions to the outline and to the holes. My basic outline dimensions would be MMC. Datum A would be the mount face. Datum B would be one of the holes. Datum C would be another hole located as far as possible from Datum B. I would apply one positional tolerance to the holes, assuring alignment with the mating holes. I would apply a profile tolerance all around the outline. This would be shown to slop inward because of the MMC dimensions noted above. ASME Y14.5M-1994 shows how to do this.

I am sure there are more ways to do this, but one of the above approaches should work.

JHG

 

[Tunalover]

drawoh-
I didn't ask how to dimension the panel.

One might think that it's possible to use datums assigned to the width and length of the recess in a feature control frame of a positional tolerance controlling the holes at the bottom of the recess. If one does, then don't the datums pass through the midplanes of the recess? If that's the case, then doesn't the fundamental requirement that dimensions originate from datums force one to dimension from the centerlines?



Tunalover

 

[drawoh]

tunalover,

It is hard to discuss the application of datums without the context of how you are going to apply dimensions and tolerances.

You can apply a datum to a surface such as an edge of your cover. Alternately, you can apply a datum to a width or length, meaning that the datum applies to a centreline. According to the ASME standad, this datum feature is subject to size variation, and it is necessary to specify RFS, MMC or LMC.

If you used the length and width as datums, then dimensions from centrelines with positional tolerances are a logical expression of your design intent and your requirements. In my second example above with the outline centred on the holes, it still makes sense. The only thing that messes up centreline dimensions is linear +/- tolerances.

JHG

 

[Tunalover]

drawoh-
For inspection, how would one establish one of those datums?


Tunalover

 

[MikeHalloran]

How to establish a usable inspection datum from the centerlines of a rectangular opening?

For someone who doesn't know what he's doing, the answer is easy...

Coupla racks on a common pinion, one for X, one for Y, or some a those spear point center finders, two for X, two for Y, etc.

Start talking like that to a gagemaker, he'll just look at you funny.



Mike Halloran
NOT speaking for
DeAngelo Marine Exhaust Inc.
Ft. Lauderdale, FL, USA

 

[ewh]

As drawoh stated, dimensioning from the centerline of the datum is a logical and appropriate way to approach the problem, provided you DO NOT label the centerline as a datum. This is a very common, but poor practice. If you feel you must label the centerline, put "CL" in front of the datum symbol.

 

[drawoh]

tunalover and MikeHalloran,

Since the length and width datums are applied at MMC, a fixture is fairly easy to make. You mill out a pocket that defines MMC. It acts as a NOGO guage on the outline. When the panel drops into the fixture, you can wiggle it a bit to line up the holes.

I haven't really thought this one through. It helps explain why ASME Y14.5M-1994 is so dogmatic about specifying material condition. Without MMC, MikeHalloran's suggestion about the racks and pinions might be the only way to go.

My alternate suggestion above was to use two holes as secondary datums. The fixturing for these is simple. You mill out a pocket at MMC containing a round dowel pin and a diamond dowel pin. More pins define the other holes. The cover must drop into the pocket, over the dowel pins. You can test the outline LMC with a feeler gauge.

I was told in my GD&T course that test fixture must use the datums as jigging points. I am not sure this is absolutely valid. I ignore the drawing, and I just the part up by its mount face, one edge and one corner. I carefully measure everything. Now, I look at the drawing and I see what datums I am supposed to measure everything with respect to. I have enough information to work out where the datums are and where everything else is. This _is_ a lot of work.

Centrelines are not defined anywhere in the ASME standard. The centreline is fairly obvious on tunalover's plate only until I come along and cut out a piece on either side of the top half. How there are two feature that might define that centre!

JHG

 

[MikeHalloran]

I was being facetious.

At first glance, you don't absolutely have to use the datums as jigging points; the math is just _much_ easier that way.

The other choice is, you are working in an arbitrary coordinate system that may or may not align with any features of the part, and after you measure all the part features relative to your coordinate system, you must then do translations and rotations to convert the measurements to the coordinate system defined by the datums, so that you can interpret whether the features are within the tolerance zones. Well, okay, a modern CMM can accept a part in any orientation, and you can touch the probe to the part in a few places and tell the machine to measure everything else relative to that.

And that's where the wrench gets jammed in the works. Suppose the datum features on the part are not perfect? Say your edges were nibbled with a square punch that was rotated a little from the punch's translation coordinates? Now you've got stair- steps where there should be a straight line. Put that part in the CMM, and where do you touch it to establish that line?

That's what they really meant in the GD&T course; the real datum coordinate system is defined not by the imperfect features on the part, but on the complementary set of 'perfect' surfaces on the fixture that unequivocally touch, align, and stabilize the part.



Mike Halloran
NOT speaking for
DeAngelo Marine Exhaust Inc.
Ft. Lauderdale, FL, USA

 

[drawoh]

MikeHalloran,

Actually, the standard takes all that into account.

Datum A is defined by the three points of your main surfaces that extend down the furthest. Not at all coincidentally, these are the points that will make contact with your granite reference block. The datum B edge is the two points that make contact with your second locating surface. The tertiary datum is the one point that makes contact with the third locating surface. Most machining and sheet metal processes create nice straight edges. If the edges are sloppy, you would have to jig everything as per the standard.

Yet another issue with a thin sheet metal cover is that datum A is being defined by something that is not rigid. In situations like this, I have left notes on drawings stating that datum A applies when the panel is compressed flat onto the reference surface. I could swear that this procedure is called up in the standard somewhere, but I cannot find it at the moment.

JHG

 

[Tunalover]

drawoh
You said "The centreline is fairly obvious on tunalover's plate only until I come along and cut out a piece on either side of the top half. H[N]ow there are two feature that might define that centre!"

Since the dimension to which the datum is attached defines only one feature of size, then it doesn't matter how many pieces are cut out of the plate; the datum is assigned to that dimension only.

ewh-
You said "As drawoh stated, dimensioning from the centerline of the datum is a logical and appropriate way to approach the problem, provided you DO NOT label the centerline as a datum. This is a very common, but poor practice. If you feel you must label the centerline, put "CL" in front of the datum symbol."

By Y14.5M, a datum assigned to a length or width BY DEFINITION is the centerplane of that feature. This necessitates using the centerline does it not?





Tunalover

 

[ewh]

Tunalover,
Yes, it does necessitate the use of the center line. However, that center line is NOT the datum, it is the center line of the datum, and should be labeled as such. To quote ASME Y14.5m-1994, para 4.3.2 "... The datum feature symbol identifies physical features and shall not be applied to center lines, center planes, or axes except as defined in paras. 4.6.6 and 4.6.7."
Paras. 4.6.6 and 4.6.7 refer to equalizing datums and datums established from complex or irregular surfaces, neither of which are involved in this situation.

 

[Tunalover]

ewh-
I agree that the datum feature symbol may be applied to a width because a width is a physical feature (of size in this case). Let's be careful about our terminology here. The feature is inevitably an opening or protrusion. While the WIDTH is a physical feature, the DATUM (not the datum symbol!) is at the midplane of the feature when it is applied to the width dimension. In this case, where should dimensions originate? FROM THE CENTERPLANE (centerline)?



Tunalover

 

[ewh]

tunalover,
I agree with you. My point is that it is improper to label the centerline as a datum. The centerline is not the datum, the feature is.

 

[drawoh]

tunalover,

Let us assume you place is rectangular and has four holes, one in each corner. Everything is symmetric. We use any of the dimensioning and tolerancing schemes described above.

The holes can be dimensioned from the centreline, or across the centreline. I would go for across the centreline, since you have dimensions coming from real features, but I would not reject the other approach if I were checking the drawings.

In a strict technical sense, a dimension from one edge would not be incorrect. The primary objection to this practice is that on a drafting board, you could miscalculate the dimension and mess up your design intent. On 3D CAD, you can force your model to centre the holes, and the numbers come out right. The GD&T will make sense out of all of it. Regardless, it is not a good procedure.

JHG

 

[Tunalover]

drawoh-
I've always taken it as "written in stone" that dimensions must originate from datums. Is this not strictly true? It's been a long time since I looked at Y14.5 on this point.



Tunalover

 

[drawoh]

tunalover,

An advantage of GD&T positional tolerances is that the dimensions do not have to originate from datums. ASME Y14.5M-1994 does not require it.

That does not mean that dimensioning from datums is not good practise. Dimensions from centrelines look ugly to me though.

JHG

 

[Tunalover]

Are there others out there who concur that dimensions need not originate from datums?


Tunalover