Position Tolerance to Three Datums

[zofiron]

Hello,

I apologize in advance for my basic understanding of things, I've only been in my trade for a few years. I've learned enough to know what I need to make good manufacturing decisions, but I feel that I'm a bit lacking in knowledge regarding inspection.

Here's the situation: I've got a part that I'm not sure my company is inspecting properly, but nobody here is explaining it to me in a way that makes sense with any of the research and learning regarding GD&T that I've done over the past few years. I'm not able to share the actual data or prints, so I've made a mock drawing (isometric view) that mimics the part surfaces, holes, and tolerances.

See the attached pdf - I'm interested particularly in how the nearest hole (position diameter of .003 to datums A, C, D) would be inspected relative to the datum scheme. My understanding of this positional tolerance is as follows:
A theoretical true position is created at the center point of that hole relating back to the established datums.
A cylindrical tolerance zone with a diameter of .006 is created through the material that the hole is in. (This cylindrical tolerance zone would be normal to the face of that surface, or the theoretical angle of that surface relative to the established datums?)
The axis of the hole (actual condition) must fall within that cylindrical tolerance zone.


The way it is being explained to me, we are analyzing a theoretical true position of the hole center, then comparing x, y, and z values of our actual hole center. We then use the formula (SQRT(xdev)^2+(ydev)^2+(zdev)^2)x2
To me, this seems like it creates a spherical tolerance zone rather than a cylindrical one. I would have thought we would only calculate the x deviation and y deviation of the hole, because in my mind, the diameter is a 2 dimensional tolerance in which we would measure x and y in relation to the plane the hole is on, then just the axis of the hole has to be good to that plane.

Could you please help me understand this correctly?

 

[3DDave]

The first flaw is that flatness applies to the three surfaces individually; profile would be a better geometric characteristic control.

The analysis is wrong because it is dealing with a point in space, but the tolerance controls where the axis is. The theoretical X-Y point for the axis is the projection of the nominal axis onto theoretical datum A.

Compare the distance of the axis of the feature to that axis over the length of the feature. It has nothing to do with the plane the hole is on, which should have its own independent tolerance.

Graphically, the axis is to be within a cylinder of the given diameter centered on the nominal axis.

 

[Hugh Man]

Every point along the axis of the hole is a nominal [x,y,z] distance away from the [0,0,0] origin point. You can imagine as the 3 flat surfaces grow towards max material, that will change where the Z0 of you coordinate system is relative to the perfect one and with it, shifts up the cylindrical tolerance zone that it expects the axis of the hole to fall in.

Also from what I'm seeing here, are you only inspecting one point of the feature? The center of the cylinder? If so, this isn't fully checking the position of the feature, only checking location at a single cross section. The axis orientation could still differ from nominal and could walk right out of the tolerance zone. Need to check at least the beginning and end of the feature to see the position and orientation of the axis.

 

[drawoh]

zofiron,

That is not a very good drawing. A good assumption about GD&T datum features is that they are for fixturing. Most of the time, you call up the same datums in the same order. The datum[ ]A features are the three upper surfaces, not three side faces, I hope.

Your hole, datum feature[ ]C makes sense to me. The hole is perpendicular to datum[ ]A and located from the face datum[ ]B. You need profile tolerances to control the remaining sides of your part from the top faces, the side face and the first hole.

How are you going to fabricate and inspect that angled hole? This is a very nasty thing to apply an accurate tolerance to. Your sphere locates only one end of the feature. Your feature is a cylinder with an axis. The axis must be located within a .006"[ ]diameter cylinder.

--
JHG

 

[dingy2]

First of all, datum A should be shown with a Profile of a Surface tolerance rather than flatness. Flatness is only used on one uninterrupted surface while the Profile of a Surface creates a common plane of which the 3 surfaces share. One would set up on the 3 surfaces with 3 solid jacks and sweep the surface with a dial indicator on a stand. The total variation or TIR cannot be over .003. Pretty easy stuff to perform.

Your positional tolerances (if high volume) should be in a Maximum Material Condition (MMC) including datum holes C & D rather than RFS. An attribute gauge would be appropriate and would achieve a high degree of confidence. Set up on datum A, have sold pins (virtual condition size) in datums C & D and a moveable pin (also virtual condition size) would go into the hole from top to bottom to meet this requirement.

If in Regardless of Feature Size (RFS) then you need a good CMM to measure it with any degree of confidence. I don't know what in the world the guys in Quality gave you but it certainly is suspect.

The drawing should show the top of the angled hole with basic dimensions from datums C & D and the surface angle should also be shown in a basic dimension. A diametrical tolerance zone of .006 really means that the hole cannot move radially (any direction) more than .003 off theoretical centre and must be confirmed at the top and bottom of the hole perpendicular to the angled surface.

Again, this is a mess without a Coordinate Measuring Machine or gauge if in MMC. Please note that anyone trying to explain the measuring method to you may not look you in the eye.

Good luck!!

Dave D.

http://www.qmsi.ca

 

[zofiron]

Thanks for the responses!

Just to clear some things up: this is not a design/drawing that my company has created internally. Rather it is a customer-driven drawing that we must adhere to the best we can. Unfortunately we see incorrect GD&T quite often, though I didn't know about the flatness one being used incorrectly there because we see it used across multiple surfaces to create datums quite regularly. Not arguing that it's not incorrect or anything, just an observation. Also, just to be clear again, the pdf I provided is a representation of what the drawing shows, not the actual drawing. But yes, datum A is the tops of the three surfaces of the pads on top.

All the tolerances are RFS. Unfortunately, we only see MMC or LMC every once in a while. It seems many engineers in our trade don't use the tools they are given.

We are checking the part with a laser tracker.

I just want to be sure I understand the check process of that hole correctly. I believe I understand most of the things you all have said, and I think it aligns with the way I was understanding this. Please tell me if any of this is correct or incorrect:
The tolerance zone is a cylindrical zone with a diameter of .006
The center point of that diameter would be an X, Y coordinate (basic dims) from the origin (nominal location) on a theoretical plane which the hole should be normal to which is created from the datum features
That diameter of .006 at that center point is projected through the thickness of the feature (the pad that the hole is in) normal to that same plane (XX degrees from datum A) to create the cylindrical tolerance zone
The axis of the hole we are checking must fall within that tolerance zone

Assuming the above (or some or most of it) is correct, would this be the same as measuring the X, Y deviance from the center point of the actual hole to the theoretical position of the hole, both on the plane perpendicular to the hole (or the theoretical plane it should be on)? Then using the 2(SQRT(xdev)^2+(ydev)^2) formula to verify that it is in tolerance (of course top and bottom of the hole to verify the entire axis)?

Hopefully what I'm asking makes sense!

 

[chez311]

That diameter of .006 at that center point is projected through the thickness of the feature (the pad that the hole is in) normal to that same plane (XX degrees from datum A) to create the cylindrical tolerance zone

It might seem like nitpicking, but its an important distinction - while the tolerance zone extends through the thickness of the part to which it is attached (the pad/leg where the hole is) the tolerance zone is located/oriented to the associated DRF. There is no requirement as shown for the hole to be normal to the "pad" through which it extends - only that it be located/oriented to |A|C|D|.