Tolerances for Basic dimensions, continued... 2

[ewh]

israelkk,

Don't think of it as a debate. The standard is a complex one, and I'd say that most of the people who use it don't understand it fully. I definitely don't, but I do have a basic working knowledge of it and turn to the standard often to improve my understanding of it. The worst thing we can do if we don't understand why something is toleranced the way it is is to blindly accept that because it's been used that way before, it must be correct.

You are correct in that you can use basic dimensions without establishing features, by using other dimensional tolerances. Examples are angularity and taper. I have gotten into the habit of establishing datums before I dimension, thus my erroneous comment.

However, to properly use a geometric tolerance on a hole, you must establish what that tolerance is relative to, which would be datum(s). It can't be relative to itself.
For true position, per Y14.5M-1994, para 5.2.1.3, "It is necessary to identify features on a part to establish datums for dimensions locating true positions." For your example to be correct, one of the holes would have to be a datum, and the others located relative to that.

I am definitely open to correction on this, to better understand the standard myself. I won't accept "because that's how it's done" as a valid reason, but will gladly accept any argument documented by the standard.

Eric

 

[btrueblood]

drawoh,

I've read through your last reply dated 10/26. I'm beginning to think that without some drawings/sketches etc. to look at, this whole thread is pointless, since I can't seem to explain my dilemma (sp?) properly. This is not intended as a slam on anybody, just a limitation of trying to converse about gdt without benefit of graphics.

You stated a bit earlier "Your hole must be positioned with respect to something for your dimension to be useful." Essentially, you need the dimension to refer to some comibnation of a feature and/or a datum to be valid.

I agree with that statement. But ,in your reply to israelkk's plate problem, how are you defining the position of the holes relative to the plate edges (which you defined as datums) if you don't apply a basic dimension from those datums to one or more of the holes? Perhaps you simply are giving a general example of "I don't care where the holes are located, so no dimension is required." Fine, I can see your point. If we did care somewhat about the location of the holes relative to the plate's edges we could put a dimension to those edges, with a tolerance of (let's say) +/- 5mm. We then apply the t.p. tolerance to the bolt holes, assuming we've defined the distances between the holes using basic dimensions, and give a t.p. tolerance of (let's say) 1mm, to ensure pattern alignment and fitup to the mating parts. I am SO WITH YOU SO FAR!

But, let's continue: since the 80mm bolt spacing (I assume you mean this spacing dimension to be a basic dimension from one hole centerline to another) does not reference any of your datums, what effect does specifying the datums have on the t.p. tolerance and location of the holes, if any?

Secondly, you stated that you would put a profile tolerance on the outer boundary surfaces of the plate -- why?

Thanks for sticking with this so far, I think we may be getting somewhere (I just can't seem to locate where that is, anybody seen a datum?)

 

[btrueblood]

ewh wrote: "Thanks for the explanation. As I stated in my first post, I was refering ONLY to the 1994 version. Your points are valid for the previous versions."

Yeah, I know. I'm going to go back and re-read the 1982 STANDARD (I was basing earlier statements about the STANDARD given what I was taught, and what is written about the standard in the Drawing Requirements Manual that refers to the 1982 standard.) I'm not sure that the STANDARD in 1982 was any more clear than the current one regarding whether datums are required in a t.p. tolerance block, the DRM is pretty clear that they weren't.

Regarding an earlier statement about the costs of getting parts made using gdt, I had to chuckle. The problem I am describing to you is one in which I want to give tolerances that are as loose as possible yet still allow the part to function (mating holes line up). In many cases, I am now dealing with parts machined from castings. The extra cost of machining datum features to the level of precision required for locating bolt holes can't be justified.

I used to be a rocket engineer, and know how to over-specify tolerances too. It is difficult sometimes to think about how loose we can let things get and still have them work. It's easy with gdt to grossly over-specify tight tolerancing; my questions are how we can loosen the tolerances to the working limit, and therefore justify the use of the powerful tools that gdt gives us.

BTW, in my prior role as a rocket engineer, we bought a few parts from MOOG. They were invariably more complex, costly, and/or heavy relative to competitive devices. Very few 2nd generation propellant valve contracts went to MOOG. Don't get me wrong - they did nice work, if you could afford the price tag. But one of the reasons I don't work in the field anymore is that price competition has finally reached the aero industry in the wake of the "end of the cold war"; I got out before getting the axe.

 

[ewh]

btrueblood,

Using a profile tolerance as suggested by drawoh simplifies the geometric callout, as you can control the form or combinations of size, form, orientation, and location.

Eric

 

[ewh]

btrueblood,

I know where your coming from regarding Moog. I worked at the Engine Controls Division until they had to close it down (actually consolidated it with another division). Our servovalves were (and probably still are) engineered to a high standard of quality, but at high cost. My reference to them as an excellent company refered more to how they treated their workers than to their share of the marketplace.

Eric

 

[drawoh]

btrueblood,

On the +/- tolerance example, I explicitly applied dimensions from the edge, for precisely the reasons you mention.

ASME Y14.5M-1994 defines the meaning of whatever I put on my drawings, including any +/- tolerances. In the case of an apparently symmetrical part, ASME says that it _is_ symmetrical. The ten millimeter space to the first set of holes is implied.

The section on establishing datums is long and complex, largely because of the problems you mention above. In the case of a rough casting or a weldment, there are two ways to avoid machining datum surfaces.

1.] Define datum targets. Datum A becomes three explicitly defined points on the bottom surface. When I get your drawings, I know where to place the three pins in my inspection fixture.

2.] Phyically fabricate in datum surfaces. This is explicitly recommended by foundries in their design manuals.

In either case, you do not want the datum surfaces removed or modified by machining. Everybody in the process jigs to the same points.

JHG

 

[btrueblood]

ewh,

"Using a profile tolerance as suggested by drawoh simplifies the geometric callout, as you can control the form or combinations of size, form, orientation, and location."

Yeah, I got that. But it also, in some cases, requires more inspection, or at least more complex and costly tooling to inspect. This in many cases weighs against dimensioning parts the way he described.

If (as in my case) the part were a cast bracket with the holes required to be located with looser precision relative to the edges of the part, but located much more precisely relative to each other, applying a profile tolerance would be inappropriate, wouldn't it?

 

[ewh]

btrueblood,

You may be right that a profile tolerance in this case is overkill. I would still approach it by establishing primary, secondary and tertiary datums (face and two perpendicular sides). No control would be required of these datums. Think of them more as "labels". I would then locate one of the holes loosely to those three datums, and make it my fourth datum. The remaining holes can be tightly controlled to that fourth datum (and loosely to the other three if desired). This should be simple to set up and inspect.
You DO NOT have to approach it this way. The only datum necessary for the control you seek would be that of the hole, so as to control the location of the other holes relative to it.
Of course, since your drawings specify the 1982 standard, there may be other ways to accomplish this. I have mentally superceded the older versions with the 1994 version, so as to confuse myself as little as possible. Sometimes it works, other times not (which is why I always keep a copy of the new version close at hand).
I hope I have explained my reasoning clearly.

Eric

 

[drawoh]

btrueblood,

In my example, all the profile tolerance does is define the outside edge. The holes are located by a pair of position tolerances, one of which locates the pattern, and one of which locates the holes within the pattern.

ASME Y14.5M-1994 explictly does exactly what you want here.

Also, ASME Y14.5M-1994 states that if the angle is not specified, it is assumed to be perpendicular to whatever the angle tolerance on your title block states. On my title block, this is +/-1 degree. This is extremely inaccurate, and I think it affects your holes. I have not checked carefully.

JHG

 

[btrueblood]

ewh,

Yes, I get your point about locating one hole loosely to the datum, and then controlling the remaining holes. Would the equivalent of your method for a round part be to designate the o.d. as a datum, locate one hole to the datum, and designate that hole as second datum, then control remaining holes to second datum?

As far as specifying the '82 spec., I'd like to not do so, since as time goes on fewer and fewer people will have access to, and understand the implications of, the old spec.

Drawoh, thanks, now I get it. I see how you used symmetry -- this surprised the hell out of me (still stuck in 1982). In the 1982 standard, symmetry was eliminated (replaced by true position), suddenly here in 1994 it comes back again. Or are you saying you used "implied symmetry"? When doing so, do the title block tolerances apply, or the tolerance on the hole, or the tolerances given for the outside edges of the part? So, could I have eliminated the profile tolerance in your example, and still control the holes (loosely) relative to datum targets, and more tightly relative to themselves? Remember, in my design, the position of the holes, relative to part boundaries, is and needs to be as "loose" as possible.

I really do appreciate your sticking with me on this, I'm starting to see the "right" approach to "best define" the engineering intent, using the '94 standard. I'm beginning to see how to "loosen up" tolerancing and still use gdt. As I said earlier, it's not easy when all examples given in texts & standards are for tightly controlled geometries. Maybe I should look at the casting/foundry drawing standards as well?

 

[ewh]

BTRUEBLOOD,

"Would the equivalent of your method for a round part be to designate the o.d. as a datum, locate one hole to the datum, and designate that hole as second datum, then control remaining holes to second datum?"

Yes, as long as the hole pattern location relative to your o.d. isn't important.

Cast parts are a different animal. As drawoh stated earlier, cast parts have to have the datums machined into the part after they are cast to establish the three basic datums. In my experience, these datums are the bottom surfaces of flat bottom holes or spotfaces. The difficulty lies in accurately locating them to cast features.

Eric

 

[btrueblood]

Thanks Eric.

 

[CanEngJohn]

Ok so lets think from a functional point of view.

I'll take a plate and create the hole pattern and relate all positions to a bolt circle diameter center. All hole true positions are to the bolt circle diameter center.

My datum A is one side of the plate. Datum B is the center of the bolt circle diameter.

All dimensions in the plate are relavant to A and B including the outside edge which has a profile tolerance. Heck, I would manufacture it this way. Make the holes and position then clean up the edges to the holes(if required).

 

[ewh]

CanEngJohn,

"All hole true positions are to the bolt circle diameter center."
"Datum B is the center of the bolt circle diameter."

You cannot locate a hole to a feature that does not exist until the hole does.

You cannot call a hole center a datum. para 4.3.2 "The datum feature symbol ... shall not be applied to center lines, center planes, or axes..." You can call it the center or axis of a datum, but only for subsequent features, not for the holes that define that bolt circle. As a bolt circle, there is no feature to reference if you are going to locate the holes in that circle to it. Circular logic, the chicken or the egg kinda thing. Like calling out a hole as datum A, then locating that hole using true position relative to datum A.

I'm not saying you couldn't make the part this way, just that you cannot dimension it per the standard in this way.

Eric

 

[drawoh]

btrueblood and CanEngJohn,

Strictly speaking, the dual positional tolerance applies to each hole in the pattern, not just the first one. The pattern could be rotated as well as shifted.

A pitch (bolt) circle can be located from an edge datum the same way the rectangular pattern is. It is likely that if you have a pitch circle, you also have a big hole in the centre. This is perfectly usable as a datum, especially if your design intent was to centre the screws on that diameter.

JHG

 

[btrueblood]

drawoh, ewh:

Please check my work

For the round plate (no hole on i.d.), using drawoh's suggested method, the flat surface of the plate (perpendicular to the holes) is designated datum A (with suitable targets if required). The o.d. of the plate is designated datum B. The holes are shown patterned on a bolt circle with a basic dimension given, and angle spacing per a second basic dimension (or by specifying spacing in hole callout). Two t.p. tolerance frames are specified, the first referencing datum A with a tight tolerance, resulting in tight control on pattern (also tight control of holes perpendicularity relative to flat surface, but oh well). The second t.p. tolerance frame references datums A and B (secondary) with looser tolerance that keeps the holes roughly located within the boundary of the part (if the designer chooses the tolerance appropriately).

Thanks again,

Ben T

 

[ewh]

One of the reasons I suggested separating out a hole as a datum is to avoid the tight perpendicularity issue, but that method is also a good one, and will accomplish what you want.

 

[drawoh]

btrueblood,

If you want bolts to go through your holes, you want the perpendicularity. The perpendicularity error is a lineary dimension measured all along the length of your hole. If your case, this is 1mm.

JHG