BEST METHOD FOR SMALL, TIGHT TOLERANCE, HOLES

[YCENG]

I need to make two .0275" holes in a .120" thick plate, with a hole diameter and centerline tolerance of +/- .00005", or better.

I was thinking of making the plate of either carbide or 440C 54-56RC.

Is jig grinding the best method for making these holes?

Is one material better than the other for the tolerances I'm trying to get?

Thanks for any input you can give me.

 

[MikeHalloran]

I'm guessing.. plunge EDM, and lap in a jig borer.
I wouldn't expect a great yield to those tolerances.



Mike Halloran
Pembroke Pines, FL, USA

 

[mfgenggear]

Yceng

+/- .00005 is approx. .00014 true position.
I believe .0005 true position is more possible.
.0001 max hole tolerance is possible but tough.
to my experience this would be a best effort basis.
Carbide requires diamond coated tools.
440C SS is tough to keep flat during heat treat so surface grind & lap will be required.
rough EDM the hole if done after heat treat ,Jig grind then lap the hole,
maybe some one else, knows of a process that can hold this tight of tolerance.

do you really need it that close?
what is this for?

MfgEngGear

 

[unclesyd]

Though your diameter is large by our small hole (.0150") standards we our holes made by EDM in hardened material or drilled in unheat treated material. We didn't use much 440 material due to stability problems. Our primary MOC was one of PH SS worked in the aged condition. Our process was drill or EDM ream and then broach. We could hold your centerline tolerances on the PH material. What type of edge do you need on the holes as we required discernible radius at 100X.
We actually made most of our tooling but at times we did use tooling from Najet.

http://www.najet.com/tooling/newDefault.htm

 

[Troy2601]

I suggest the same as above, in my opinion you will want to use a hardend steel and first use EDM and then lap them in jig borer

 

[is2634]

We have done similar applications using wire edm and jig grinding.

Both materials can be processed in either fashion without much difference in cost.

In our application, we would counterbore the hole to reduce the effective length of the critical dimension for jig grind. The jig grinding process gets very difficult when this size hole is longer than 3 diameters. If you need the full length, I would recommend wire edm using a recent top of the line model.

Regarding size tolerance, your ±.00005 inch can be achieved with either process given some type of in-process sizing feedback. We use gage pins in .0001" increments in-process for offset adjustments (with high end CMM for off-line final inspection). Watch out for issues with form and orientation controls such as roundness, cylindricity and perpendicularity.

Regarding position tolerance, much will depend on the quality of the datum you are measuring from. If possible create the datum and feature in the same operation. Even when we do this our true position (ANSI Y14.5) results are near .0002", but occasionally we are less than .0001".

Measurement uncertainty of this tyype of hole will be quite large. A CMM will not be able to scan the entire hole depth, so you will have to use a partial scan or resort to vision and backlighting.

is2634