True Position of a hole to a face & Profile Question

[J Taylor]

Question 1 - True Position

(M6 Thread) - True Position diameter 0.25 to datum P (datum P is a boss face)
Is this another way of asking for the Perpendicularity of a hole to a face?
In this case the Perpendicularity of an M6 Thread to its accomplying boss face.

Question 2 - Profile of a face

2 Boss faces on the same height - Profile 0.3 to ABC
Underneath - Profile 0.1
Underneath - 2 SURFACES

I have taken this as Profile 0.3 for each boss face back to ABC
Then Profile 0.1 from one boss to the other.

I have attached a drawing, but cannot see in the preview.

Thanks

 

[3DDave]

Question 1: For single hole under Y14.5, the common interpretation is that substituting position for perpendicularity is not a valid use. The angle is required to be basic for the upper segment with the position tolerance to be valid.

I don't understand why there is a requirement to be perpendicular to the local surface. If that is a requirement they should have specified a spot-face that is perpendicular to the hole. The manufacturing problem is that the hole can be acceptably located to the three datum features, and the flat surface can have an acceptable profile to the three datum features, but the hole is rejected for the perpendicularity requirement.

This means that the surface orientation is controlled by the hole location and that requirement is not explicit on the drawing. For manufacturing the machinist needs to fit all three geometric tolerances at the same time to find a solution that is more limited than the defined tolerances.

This problem mostly goes away if the typical variations for the particular machining process are far smaller than the allowable tolerances. If the machining variations are close to the tolerances, then there's a large chance of a high rejection rate. How much of a problem this might be depends on how large the various features are and what the variations are.

Question 2: It seems like you have a correct interpretation.

 

[Burunduk]

If it is just one M6 thread, then the Ø0.25 tolerance with ref. to P should have been replaced by perpendicularity, because in this case, there is no location control aspect to it.

However, there are 2 boss faces. Doesn't the second one has a similar threaded hole in it?
If there were also two M6 holes treated as a pattern (by a specification such as "2X M6-6H"), then the Ø0.25 tolerance with ref. to P (while P is 2 coplanar surfaces) would make sense, as it would control the threaded holes for their mutual location as well as perpendicularity to a datum established from the two boss faces.

You are correct about the second question. The 0.3 profile tolerance controls the location and orientation of the two faces relative to datum ref. frame established by datum references A, B(M), C(M). The 0.1 profile tolerance controls the form and coplanarity of these surfaces.