Gauge callout on drawing 2

[Paitch]

I have a drawing with GAUGE attached to two dimensions.
Have not seen this callout before and am unsure what it means. The attached sketch is representative of the drawing. If you can shed some light, I'd appreciate it.

 

[KENAT]

I think it's an old/non standard way of saying the 2.900 is essentially basic, so only subject to 'Gauge Tolerances' at inspection.

KENAT,

Have you reminded yourself of faq731-376 recently, or taken a look at posting policies:

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

What is Engineering anyway: faq1088-1484

 

[SDETERS]

We do this a lot on our drawings. How I see this drawing is at this diameter the dimension .400+/-.002 must be met. It is a good way of dimensioning a cone on a drawing. We usually make out GAUGE dimension basic. The gauge dimension does not have tolerance. I am interested on how others do this same type of dimensioning.

 

[cadman1964]

We get this alot here. Basically it's a point on the surface to gage to. The 20deg and .400 are subject to tolerance. Typically the 2.900 would be basic.

This method is lot easier to measure with hard gaging during production. We would build a ring with ID at 2.900 dia and a OD of aprox 1" bigger than your OD of the part. Then we would indicate off the surface of the ring to the top of the part. This is lot easier than trying to measure to Thero sharp point.

Solid Edge V20

 

[drawoh]

SDETERS,

I would use a profile tolerance and basic dimensions. Your profile tolerance would be approximately .004". Perhaps I would use .003".

The tolerance does not only apply at Ø2.900[×].400.

JHG

 

[MikeHalloran]

The 2.900 is not a feature of the part at all, so you _can't_ inspect it. It's a feature of the gage, which is implied BASIC, that's used to inspect the .400 dimension.



Mike Halloran
Pembroke Pines, FL, USA

 

[Paitch]

Thanks all. So it seems the .400 and 2.900 values are somewhat arbitrary and the .400 is just what 2.900 yields when trigged out. Have I got it? See attached.

 

[KENAT]

Essentially, the combination of angle & point on the line give you the slope of the surface.

Rather than giving you the start or end point they've given you a point somwhere in between defined by a diameter and a height. The diameter is 'perfect' with the tolerance put on the height.

Often things are dimensioned like this because the nominal mating point is on the 'gauge' line.

KENAT,

Have you reminded yourself of faq731-376 recently, or taken a look at posting policies:

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

What is Engineering anyway: faq1088-1484

 

[cadman1964]

Paitch, that's how we would measure the part per my previous post. Just remember the gage dia should be basic.

Often things are dimensioned like this because the nominal mating point is on the 'Gage' line.

More often than not in my industry it's dimensioned like this for ease of hard gaging at the press

Solid Edge V20

 

[dgallup]

A gage diameter & length with an angle is one of the recommended ways to tolerance conical surfaces. As others have said, the gage diameter should be basic (enclosed in a box). It has no tolerance. We normally have a note symbol attached to the .400+/-.002 dimension and a title block note saying something like "MEASURE DIMENSION AT GAGE [BASIC] DIMENSION SHOWN." We do it that way because we frequently had multiple tapers on one part.

 

[Paitch]

Our customer has requested that we verify the .400 +/- .002 at FA on the CMM then hard gauge for production.