Bidirectional Positional Tolerance

[jimbod20]

I think I have the correct subject line. Reference the attached hand sketch.

I have a casting with primary, secondary and tertiary datums E, F and G respectively. E is a surface defined by 3 datum targets. F is the secondary datum defined by 2 datum targets. G is the tertiary datum defined by one datum target. The location of the .250 inch diameter hole (datum B) is defined via basic dimensions from E, F and G. Size and position of .250 diameter hole is as shown on attached sketch.

My question;

I can allow hole B to move in one direction more than the other from datum point G. Position to E and F must be as shown on attached sketch. Can someone explain to me how I define position of B relative to G a different amount/magnitude in two directions?

 

[jimbod20]

Attachment provided.

 

[powerhound]

Figure 5-41 in the 1994 standard should get you what you want. I'm assuming you are working to the 1994 ASME standard. Your current callout, while not really illegal, is probably not the clearest way to do this with a single hole.

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

 

[jimbod20]

Hi Powerhound,

Do you know if i can define a tolerance zone as shown in attached sketch? I use figure 5-41 in 1994 standard in attempt to illustrate.

I also clarify previous sketch.

For example, I can allow .250 machined diameter B to move more in one direction relative to Datum G (next higher level assembly will fit) I still need position of .015 for diameter B to E and F via additional single segment FCF.

 

[jimbod20]

Additional attachment.

 

[pmarc]

jimbod20,
Is there any particular reason that true position of the hole can't be modified to make positional tolerance zone symmetrical relative to that true position?

Y14.5 standard does not offer any support on such method of positional tolerancing.

 

[jimbod20]

Pmarc,

The issue is as follows.

My machine shop has a machine fixture which sets up the casting on E, F, G. The machinist then indicates the location of a round cast boss at the top of the casting ~ 7 inches above surface E. An 'offset' is established based upon the indicated location of the cast boss vs theoretically exact location to ensure the cast boss has uniform wall thickness around a machined diameter within the boss (visual to customer). The offset is indicated/established and slightly different for each part. Diameter B is installed with the offset and moves in one direction relative to G. The offset is always away from G. Functionally this is ok. Diameter B is a mount lug and the offset simply gives me a little more clearance at the next assembly level. I have established a limit for magnitude and direction of 'offset'. I do need position of .015 with respect to E, F. I suspect my description is sufficient. I'm looking for a way to put what I just described on the drawing.

 

[fsincox]

I think what you have done is fine and technically legal, if that is what you truely want. based on what you say in your last statement I question that is really what you want anyway. You are describing a machining framework location that also imposes an offset to accomodate a "casting datum" location, are you not?
Frank

 

[jimbod20]

I did not provide adequate explanation;

I setup the machine and casting drawings to establish function and interface with the next assembly. The casting allows profile of .060 relative to cast datum structure E, F, G. Position of B with respect to E,F,G (ie .030) is based upon tolerance stack of profile to cast datum structure and machine to cast datum structure. I illustrate cast datum structure and machine datum B on my attached sketch. FYI, primary machined datum axis is B-C. C is located with respect to B.

Design intent is as shown on my sketch.

The real castings are produced and we find the need to establish a machine offset based upon the location of cast boss ~7 inches above surface E. We want uniform wall thickness around the machined boss (aesthetic want). The offset is in one axis in one direction. Functionally the offset is ok for my needs. Magnitude and direction of offset is such that I simply end up with a little more clearance at the next assembly.

Now to my original message thread. Is there a way for me to define what I describe on the drawing.
- I need position of B with respect to E and F of .015.
- I need position of B with respect to G of .030 in one direction. I can allow greater position tolerance of B with respect to G in the other direction.

I do see unequally disposed profile tolerance zone in ASME Y14.5-2009.

 

[vouty]

Hi ,
Your case seems exactly what is in ASME y14.5-2009, page 141 and I think I agree with your proposition if I well understood (see my attached sketch).
Depending of the culture, the size, the structure of your company I'll use Multiple Single-Segment Feature Control Frames or not.
There are several reasons for that :
1/ In the shop, very good professionals must be comfortable with interpretation of the geometrical dimensioning and tolerancing . Multiple Single-Segment Feature Control Frames is a sophisticated way to explain geometrical requirements but not always the easier/faster way to communicate depending on the context of application and the frequency of utilization
2/ Using a combination of geometrical tolerances is allowed and easy to interpret for anybody (see attached file).
3/ Tools used during inspection have to be considered (CMM , Gage-fixtures, non CMM and no Gage-fixtures .... ?)
So I'd make my decision with these parameters, to have a balance between a clear geometrical tolerancing and good communication
All depends of the structure of your company, the training , habits and the potential questions of your partners.
Same time I'll avoid using only a rectangular tolerancing which doesn't provide information for inspection setup(possibility of several different setup giving different results).
Hope this helps'

 

[CheckerHater]

If I understood you correctly, your actual position is a compromise between theoretical position wrt [E|F|G] datum framework and hole being centered wrt cast boss.
So, why don’t you put your money where your mouth is and make your boss a datum?
You specify how much the hole position may vary to [E|F|G] in one tolerance frame, and how much position tolerance is allowed to boss-derived datum in another tolerance frame.
Tolerances in both tolerance frames will have to be met together
Resulting tolerance zone will look somewhat like the enclosed picture. (You specified diametric tolerance zones in your example, but similar arrangement can be made with rectangular ones)

 

[jimbod20]

I will try my explanation again. I provide a more detailed sketch to facilitate discussion.

The cast datum structure is E, F, G (primary-secondary-tertiary). Machine Datum structure is axis B-C, diameter D and surface A (primary-secondary-tertiary). I think you can see location of surface A.

I 'stacked' design intent as follows;

1. Cast profile to cast datums
2. Machine datums to cast datums
3. Machine features to machine datums.

Design intent is per the attached sketch.

The castings are setup in a fixture that replicates the cast datum structure (E, F and G). Manufacturing and inspection find that if they machine the bore of the cast boss in accordance with basic dimensions at the top of the casting (adjacent to .3776 diameter datum d) the cast wall is no longer uniform around the machined boss. This is ok per design intent. I stacked to provide adequate wall thickness. Manufacturing wants visually appealing parts. My customer does have general workmanship inspect criteria.

Manufacturing finds they can 'indicate' the location of the cast boss and establish an offset relative to the perfect location. The offset provides a uniform cast wall around the machined bore of the cast boss. The castings are setup in the machine fixture, the cast boss is indicated and an offset is established for each part. The offset is relative to datum G in one direction only. The offset axis and the offset direction is identified in the attached sketch. The machine datum structure (B-C and D) moves with the offset. Functionally this is ok. B-C, D and A are the mount interface locations at the next assembly.

Inspection finds datum B does not meet position to G (the outcome was accepted when the offset was established). I have inspection submit results to me via MRB and I approve for use. Disposition is the parts are functionally acceptable and the offset simply provides a bit more clearance at next/customer assembly level.

I might be asking a dumb question;

Is there a way I can change my drawing to allow offset of B to G in one direction more than the other? I use ASME Y14.5M-1994 standard.

 

[vouty]

Hi ,
Do you mean to have a larger tolerance in offset direction ?
If yes , and if allowed, you ca change the tolerance value of your first segment for B (e.g. : .030 -> .040), and you basic move of half the difference).
Do you have this possibility ?
An appropriated note on a drawing can help to traceability of modifications and to get the approbation by partners


(ASME Y14.5-1994 p 107-108)

 

[CheckerHater]

1. Is the round boss on top of your part somehow related to any of your datums/features/whatever named A, B, C, D, E, F, G?
Is this relationship shown anywhere on your drawing?
2. Is the round hole inside of the round boss on top of your part somehow related to any of your datums/features/whatever named A, B, C, D, E, F, G?
Is this relationship shown anywhere on your drawing?
Is this the hole that has to be centered to the boss for functional/aesthetic reasons?
3. Do you need your B to be able to move in relationship to G in order to adjust position of the round hole inside of the round boss, or is it part of some other functional requirement?

 

[fsincox]

CH,
I believe I am seeing this the same way you are, I see many problems now with castings were they they want to machine the part complete from one set-up but the casting tolerances will not accomodate.
Frank

 

[jimbod20]

Hello,

The round boss at the top of the part provides transfer tube interface at the next assembly level. Transfer tube is a functional interface. Holes B, C, D and surface A establish physical mount interface at next assembly. The machined boss at the top of the part is related to machine datums B-C, D and A via basic dimensions to machine boss with position control of .015 to B-C, D, A.

The machined hole within the cast boss at the top of the part is centered via manufacturing/machine shop process.

I would like to allow B to move more in one direction than the other relative to G.

 

[CheckerHater]

The machined hole within the cast boss at the top of the part is centered via manufacturing/machine shop process.

Is "The machined hole within the cast boss at the top of the part" centered via GD&T? I don't see it on your drawing.
Which boss are you talking about, square or round?

 

[jimbod20]

I modify the sketch. See attached.

Round boss at the top of the part. Location is via basic dimensions x.xxx. Size is .8135 with .015 position to B-C, D, A.

 

[CheckerHater]

OK, when you adjust your setup to center the hole to the boss, does the hole stay within tolerance wrt datums, or does it go completely off-charts?

Right now I am a bit confused by your description: it looks like you carefully position the part to the datums and then just move it as you please and drill the hole. Maybe you just specify that hole has to be centered to the boss and that’s it?

Also, I am sorry for not responding quickly. I am posting from work when I can.

 

[jimbod20]

The .8135 diameter hole, B-C and D all move with the 'offset'. When we inspect the fully machined housing we only find B out of position with respect to datum G. B is not out of position with respect to E or F. C position to B is good. D position to B-C, E and F is good.

I could only center .8135 boss within cast diameter.

I prefer for .8135 diameter hole, B, C, and D to all move via offset. B, C, D physical mount holes. .8135 a fluid interface at next assembly.