True position callout with non datum axis basic dimensions (using OGP measurmind software)

[Langless28]

I am trying to figure out how to setup this TP callout using an optical CMM (OGP). I would be able to do it if both basic dimensions were on datum axis but the basic dimensions for the TP callout is on Y and a straight line basic dimension.

I guess the question can pertain to using the software more than anything.

I have attached a small screen capture of the print which should show you what I mean.

 

[M4C7]

Apologies in advance if this is not what you're asking for, but since the feature is located by basic dimensions, you should be able to calculate the basic X dimension using trig without affecting the actual tolerance value, as shown in the (hopefully) attached image.

If not, then I think I'm completely out of my depth and hopefully someone else here can help you out.

 

[Langless28]

Yes that was my gut feeling of just trig-ing out the X basic, since they are "true" numbers it should not affect the tolerance. Thank you for the sanity check. This means i AM measuring right which also means that there is problems with these parts.

That brings me to my next question, the design intent of this part is that the straight line dimension is what really drives the functionality of this part; because it's pivoting from the right side hole. As long as the straight line dimension is good/close, the part should function as intended. The issue is that radius nub feature is very far out in Y (which functionally does not affect the part) but is throwing off the TP callout (I am getting variances as much as .030" TP).

I am wondering if we can come up with a new dimension scheme that address the straight line dimension, is a little slack for the Y dimension, and still verifies the diameter of the nub feature.

Maybe put a +/- on the straight line dimension, and keep the +/- on the diameter callout.

 

[M4C7]

I think in that case your best bet might be to use bidirectional positional tolerancing (Section 5.9 in Y14.5-1994). This should allow a tighter control on the 3.958 dimension while allowing a looser control on the angle/orientation relative to the DRF. See attached Fig 5-42 for an example. You can also reference 5-41 for using rectangular as opposed to polar coordinates (though polar coordinates seem like a better fit for your case).

Also, I believe you might need to use a basic angle in place of the .122 dimension if you chose to use this method.

 

[tbuelna]

Langless28-

Can you provide a screen grab that also shows datums A & C. I understand that you are considering a drawing revision to modify the way the position of the .099 dia feature is controlled. But when performing a dimensional inspection you must base your measurements from the datum reference frame defined on the drawing. In the sketch provided the .099 dia feature shows two basic dimensions (.122 & 3.958) relative to datum B, but there is still not enough information shown to determine the precise relationship between the feature and datum B.

Another consideration is that in your example datum B is defined as the primary datum in the positional tolerance for the .099 dia feature, which is a bit unusual for this type of situation. If you refer to the ASME Y14.5 bidirectional positional tolerance example provided by M4C7, you'll note that the primary datum listed (datum A) is the surface the hole feature axes are normal to.

 

[Langless28]

A is the face that is facing us in the picture, c is the top surface of the part as seen in the picture. C is the surface this nub feature is physically connected to

 

[tbuelna]

OK, then it would be a good idea to first apply a positional tolerance from A & C to the hole defined as datum B, using surface A as your primary datum. And then use the bidirectional positional tolerance approach provided by M4C7. This should make it much easier to set up a datum reference frame on your CMM for dimensionally validating this feature.

 

[3DDave]

Since B is referenced RFS, only one more reference is required to fix the datum reference frame. If "A" is nominally perpendicular to "B", then it has no direct effect and could be dropped. The lack of a second basic dimension to locate target "C1" makes it difficult to be sure where C1 is relative to the feature that refers to it.

 

[tbuelna]

As shown there is insufficient definition of the datums used in the positional tolerance for the feature in question. Given that there is a point partially defined for the tertiary C1 datum target, I would expect to see a complete system of datum targets defined for the associated planes, such as three datum target points for the primary A plane, and two datum target points for the secondary B plane. The existence of datum target point C1 would seem to imply the part is machined from a casting or forging. The machined hole indicated as datum B would then use a positional tolerance referenced to the datum target planes.

 

[powerhound]

tbuelna,

Dave has a good point. Since B is Cylindrical, primary, and RFS, it already arrests 4 degrees of freedom. A single point as tertiary is all that is required to sufficiently constrain this part for the feature specified. No need for all the extras. Another point is that the nub does not appear to be a feature of size and thus should probably be located with profile.

John Acosta, GDTP S-0731
Engineering Technician
Inventor 2013
Mastercam X6
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[tbuelna]

powerhound-

I would disagree on these points: If it is implied that surface A is the primary datum for B, then surface A should also be the primary datum for the cylindrical "nub" feature position tolerance.

Also since the positional tolerance for the nub cylinder is defined at MMC, there are implications with regards to its feature size.

Interesting discussion.

 

[3DDave]

If the primary surface for orienting the part is "B", and the location and orientation of the numb is relative to it, then that should be the primary reference for the nub. Going back to A means adding the orientation variation that B has relative to A. The small allowances for tolerance suggests that limiting tolerance stack is a high priority.

 

[powerhound]

tbuelna,

That's not a good assumption to make. If datum surface A is just hanging out in space while assembled, there needn't be any reference to it. As it is, reference to A adds absolutely nothing and really needs to be removed from the feature control frame.

John Acosta, GDTP S-0731
Engineering Technician
Inventor 2013
Mastercam X6
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[tbuelna]

powerhound-

The question asked in the OP was related to how to interpret the positional tolerance shown for the .099 dia feature when setting up the part in their CMM. Design intent is never considered when inspecting a component. The positional location of the nub feature must be inspected based on its relation to the datum features listed in the tolerance block. While the screen grab did not include the part of the drawing where the definition of datums A & C were provided, as you pointed out the positional tolerance for the nub feature seems to give conflicting requirements by including A as a secondary datum.

The person performing the dimensional inspection of the part must comply with the requirements as shown on the drawing. If the drawing requirements are conflicting, incomplete or ambiguous, the inspector should request guidance from engineering. But the inspector should avoid making up their own interpretation of any unusual or unclear GD&T situations like the example provided. Engineering drawings should be looked at as a set of QA requirements that the finished component must conform to, rather than being a set of instructions for manufacturing to follow when producing the component. If the tolerance for a feature requires inspection based on certain datum surfaces under certain material conditions, then that's what the inspector must use to validate the feature. Design intent should not be considered by QA.

To be frank, using the machined hole cylinder surface at RFS as the primary datum while also using cast/forged datum target point features (A & C), makes inspecting the machined nub feature more difficult than it needs to be. While I appreciate the design intent of doing this, it also means that each part must first have this hole surface probed relative to a cast/forged surface A (which may not be accessible to the CMM probe) just to properly inspect the nub feature using the CMM. Since this part seems to be made from a forging or casting, it would be best to use the tolerancing approach typically used for these components. The machining and casting/forging drawings should use a common system of coordinated datum target points that the initial machining operations are based on. And after a fully constrained set of datum features are machined on the casting/forging, they will serve as the basis for all subsequent machined features. With these accurate machined datum features in place, an inspection fixture based on these surfaces can be used with the CMM to speed up the inspection process.

 

[3DDave]

B is not defined relative to A, or anything else, in the diagram.

 

[M4C7]

As it is, reference to A adds absolutely nothing and really needs to be removed from the feature control frame.

I'm not hugely familiar with using datum targets, but I did have a question about this statement. If datum target C is calling out a line, then I agree with what you've said above. However, if it is instead calling out a point (impossible to tell from the available view) would you not need to reference datum A to fully constrain the part?

Thanks.

 

[powerhound]

tbuelna,

Thanks for the lecture on how to inspect a part. I figured as long as you were making suggestions on how to alternatively set up the datum reference frame that I could do the same. Guess I was wrong.

M4C7,

A part does not necessarily have to be fully contrained to be sufficiently constrained. Think of a tube. If you specify the OD as a datum feature and then relate the ID to it, that's all you need. You don't have to arrest rotation around the datum axis nor do you have to arrest translation along the axis.

On the other hand, if datum A were primary, then you would have to use two other features in order to constrain it enough to make repeatable measurements.

John Acosta, GDTP S-0731
Engineering Technician
Inventor 2013
Mastercam X6
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[Langless28]

I appreciate all the responses. This part is actually an injection molded part. The issue with this part is it has been manufactured since the 90's and I am the first one to question this feature for being out of tolerance. My initial assumptions (based on DOE's) about the feature being out were hard to back up until I was successfully able to measure the feature. This proved the part to be out of tolerance. My goal now is to revise the drawing to allow the out of tolerance parts to pass incoming inspection. Functionally, they work correctly as the straight line dimension holds true, and its more cost effective to update the print to allow the drifts in Y as opposed to retooling the mold.

As this part was first drawn in the early 90's, i would assume the datum scheme was designed for measurement on an optical comparator where you would restrain the part with a fixture containing a gauge pin for datum B, with the nub feature orientating downwards towards the the floor, up against a simulated datum A plane (holds the part parallel with the comaprator). I would then think datum target C would be to hold the part rotationally about B? Datum C, as territory would only need the 1 point to fully restrain the part.

Currently, i place the part on the surface of the CMM on the opposite face to datum A. I then edge find an arbitrary intersection of the part to define my XY and start the automated program. The program uses a laser to define Datum A and align my XY plane to it. It then grabs points for Datum B and the nub feature respectively. Measuring this way, i cannot see why i would need the datum C, unless i hear back that i would need to use the touch probe to properly grab datum B and then would require me physically restraining the part to accommodate touch probe forces.

 

[3DDave]

I would probably make the nub into datum C and then profile the rest relative to B-C.

I think the goal should be to revise the drawing to describe useable parts and reject ones that won't work. What method is in place to determine how to make that determination and whether a particular tolerancing scheme will serve to adequately separate the two cases?

 

[tbuelna]

Langless28-

It would have allowed for a more meaningful discussion if you could have provided the entire drawing rather than just a snippet of it. It seems like all the participants have a pretty good understanding of GD&T practice, but since you were unable to provide the complete drawing there is quite a bit of debate on how to interpret your example.

In your last post you mentioned this is an injection molded (plastic?) part. Based on the tight tolerances shown for some of the features, I would assume this drawing describes finish machining operations performed on the molded part. If so, this brings up another important consideration when creating your datum references. With molded/cast/forged parts you must account for any draft or variation of the as-molded surfaces when setting up the part for the initial machining operations. Typically there is a system of datum target points (A1/A2/A3, B1/B2,C1) shown on the machining drawing that establish 3 orthogonal datum planes that the initial machining dimensions/tolerances are based on. Once there are sufficient machined features to establish an independent datum reference frame, the original system based on datum target points is no longer needed. Since with your machined component you mostly care about the relationship between machined features, you should base your arrangement of dimensions/tolerances to be inspected on machined datum features, as suggested by 3DDave.

You might also take a look at ASME Y14.8.