Criticism on gauge drawing 1

[prdave00]

I'd appreciate some constructive criticism on the attached drawing of an in-process gauge (or maybe this fits the definition of a checking fixture). Criticisms regarding both clarity (or lack thereof) and manufacturability (assuming the gauge tolerance has been appropriately assigned) would both be equally well received.

The gauge will be threaded into a hole (probably to a specified torque) and then a CMM algorithm will be used to verify the gauge is in the appropriate spot by probing the domed ends and locations long the shafts above and below the external threads.

I fear the drawing in its current state is ambiguous (especially application of surface profiles without datum references), may be difficult to inspect, and the tolerances too tight.

References to sections of ASME Y14.43 that bolster the criticism would be much appreciated.

 

[KENAT]

Well I'm not sure I'm really hitting some of the things you're most concerned about but a few comments with reference to the standard.

I'd be tempted to give the overall length rather than the theoretical center of the spherical radii based on 1.8.4.

I'm not sure you've got your spherical radii called out correctly, it's almost double dimensioning as it's already controlled by the pin ID. Also the symbol should be 'SR' not just 'R' 1.8.2.5. You might even want it to be a controlled radius, which I guess would be SCR but I'm not 100% sure.

Hope it helps but it's early and my brains not up to speed yet.

Posting guidelines faq731-376

http://eng-tips.com/market.cfm?

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​

 

[ewh]

I agree with KENAT that there is a double dimension situation. I would make one of the SRs a datum, reference the other back to that one and extend both profile tolerances along the cylindrical surfaces.
I'm sure others will have more/better suggestions.

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[prdave00]

KENAT & ewh:

Thanks for the initial feedback and I'll give the suggested datum reference some more thought. If I change the dome callouts to FULL SR & remove the surface profile tolerance does the diameter tolerance of the shaft take over to control size & therefore form based on the envelope principal?

I had a problem with the profile tolerance for the domed features since the profile isn't constrained to any datums and would essentially float if I were to use something like an overlay. Am I incorrect in interpreting this?

I'm trying to clean this drawing up before I send it out to gauge companies for quote. With the drawing as is we have received multiple no quotes. I think mostly due to the tolerances but having an ambiguous drawing probably didn't help.

 

[flash3780]

Establishing radii as datums can be... tricky. Perhaps datum target points would be most appropriate. ASME Y14.8 also has some good examples of setting up vee-block datum targets, which may be useful. I would establish two datums to cover my bases in the axial and radial directions. A double vee-block setup with one datum target fixed (A) and the other moving (B) would work. Of course, the vee-blocks will contact the spherical radii.

It should be much easier to define your part once you have proper datums established. The article below discusses how to establish up datum target points on page 2 (although I think you want a double-vee-block for your situation).

http://www.mechsigma.com/newsletters/2004_05_Newsletter.pdf

Am I correct in the understanding that this is a double-start thread, since the lead is 2x the pitch? Most screw threads are single start. Usually the lead is the pitch multiplied by the number of starts, so the relationship seems odd in this case. Perhaps it's due to the taper... I don't work with tapered threads much.

Regardless of the GD&T, you'll need to go to a gagemaker to get this part made; most shops won't have the capabilities.

Good luck.

 

[MikeHalloran]

The dimensioning of the ball ends makes the OAL tolerance effectively +/-.003", which may not be the desired effect. If the part were much larger and fatter, I'd use tooling balls pressed into the ends, so they could be shimmed or lapped into exact position by the gagemaker. As drawn, he's got exactly one chance to get it right, and there are too many features to control at once to do that.

If you could make the upper shank fatter, and make the upper sphere a pressed-in tooling ball (I don't know how small they come), the gagemaker might be able to make the remainder of the part in one setup and then press in a ball to get the OAL where you want it.

Otherwise, it's an impossible part. The only way you could make it worse is to include a slot or other radial feature and demand that the thread be 'clocked' in relation to it.

The .3769 dimension is from a theoretical center of a sphere to a theoretical apex of ... what? It's not abundantly clear that it's to the apex of the thread's minor conical surface, if indeed that's what intended.
It's certainly not an easy thing to measure in any case. More usual gagemaking practice would include a dimension to a circular gage line at a defined diameter (i.e. a precise sharp-edged hole in a carbide ring) that would seat on the thread's minor conical surface somewhere below the thread per se, where you now have a notch formed by the smaller cylinder's od and the conical surface at the lower end of the threaded area, which is itself located by the .962 dimension, though that's not abundantly clear either.



Mike Halloran
Pembroke Pines, FL, USA

 

[prdave00]

[blue]flash3780[/blue]: Thanks for the detailed response and introduction to MechSigma as what looks to be a pretty good reference for practical application of GD&T. I was actually surprised how deficient this drawing was in terms of a datum structure - none of the features are related. Yes, it is a double start thread, but some dimensions were disassociated in the drawing giving incorrect numbers, s/b .0197 pitch and .0394 lead.

[blue]Mike[/blue]: I love the idea of using a tooling ball at the ends (instead of machined in features) and will see if I can make something like this work. I'm not sure how (or even if) one could determine the virtual sharp based on the minor diameter (or major for that matter) of the thread. Could you humor me with a sketch of what you described regarding using a circular gauge line?

 

[MikeHalloran]

See the bottom illustration on this page:

http://www.riten.com/technical-support/faq.html#1

Centers often have a physical scratch or mark or discontinuity at their gage line, but it's not necessary. You just give a basic diameter, and an axial location to that diameter. That and an angle locates a taper unequivocally.

You are of course free to make your thread's major surface basic, which may simplify manufacturing and measurement.





Mike Halloran
Pembroke Pines, FL, USA

 

[ak762]

The gauge will be threaded into a hole (probably to a specified torque)

I am not sure but may be add gauge plane to your design