GDT for round parts 3

[cooblacrouse]

My company manufactures predominantly hollow round parts. I am fairly new to the field and have been seeing inconsistencies in historical drawings when it comes to geometric dimensioning and tolerancing. The only answers I seem to get in house is to copy what was done on previous drawings. As I have studied on my own I have yet to find an example of an ID feature called out, using concentricity or runnout, in reference to and OD datum. Does anyone have any input or resources I can use? Examples I find in text books seem to be exclusively done on shafts, OD to OD.

Thank you,

Bob

 

[drawoh]

Cooblacrouse,

If you want more information on datum targets, and you don't have a good drafting textbook, check out a website for a foundry. Datum points are a problem with castings.

Your problem is that you have a round outside form that you are trying to use as a datum. The form is not accurate enough to work properly as a datum. You need a new datum, and you have two choices...

1.] Fabricate features in the part that will work as datums in subsequent processes. As noted previously, this is a worst case solution, but sometimes, you have to do it.

2.] Arbitrarily pick three spots on your OD, and designate these as datum targets. You must provide dimensions to the points so that their location is unambiguous.

Either way, everyone measures from the same reference point.

Once you have established datums, true position is easily measured with a height vernier, if your tolerances are not too tight.

JHG

 

[diamondjim]

Bob,
I agree with you in that either the od or id
which ever was used to center the bearing should
be the datum and very accurate. With small parts
any pressure distorts the true circle unless you
are clamping only axially. I also agree that
concentricity is a pain and only should be used
if thin parts that will conform to their mating
part which would have enough thickness or wall section
to keep it round. Rings are not like fabricated or
molded parts. You have to understand the machining
operations and control them to achieve your intent.
I often wonder why taper is not used more often for
mating parts. You could be a little off radially and
the part could be assembled with only a little axial
displacement. You have to know the runout of your
machines. We have grinding machines for large part
that grind very flat but radially runout .003 inches
so to control concentricity and not runout the parts
would have to me centered or matched on the table with
some indicator mark i.e. the zero positon or whatever
will allow them to go back the the table so the high
spots are concentric. Going from table to table you
have to know where the tables high spot or greatest
eccentricity is if concentricity is your goal and
center accordingly. What a pain but a reality.

 

[Viktor]

"I agree with you in that either the od or id
which ever was used to center the bearing should
be the datum and very accurate." - this is incorrect statement! The axis not the surface is the datum.

"I often wonder why taper is not used more often for
mating parts." - because to measure any taper is much more difficult - at least two-three measurements are needed. Moreover, stadards micrometers and/or calipers cannot be used particularly for ID. Look at the common design and production practice of standard tapes (Morse, Brown & Sharps, Jarno, ASMT etc. ) – the increase production and inspection time as well as the cost of special gauges illuminate all apparent advantages of using them for general mating surfaces.

Viktor

http://viktorastakhov.tripod.com

 

[testy]

Viktor

How do you measure the axis of a hole when it exists in theory only?

 

[drawoh]

diamondjim,

The ID is not useable as a datum because it will be removed by a subsequent manufacturing process. If you need the gear to be located accurately to other features, your datum must be available througout the manufacturing process.

JHG

 

[jackboot]

I am just starting to integrate the ASME Y14.5 into our drawings - those requiring several critical dimensions.

Here is an example of a simple part that I have had a real headache with.

Hollow Cylinder:
Length 4.000 +/-0.0025
ID 3.505 +/-0.0005
OD 4.064 +/-0.0005

Here is what I need as a finished product: The OD and the ID must be concentric with one another as close as possible. Currently, we measure the "wall thickness" at 4 locations on each end of the part. We like to see that the "wall thickness" readings do not vary more than 0.0003 from each other at one location and from each end as well.

However, I end up with a long mental discussion with myself on how to best to Geo-tolerance this-and honestly, if my inspection logic is truly sound. I hope this isn't too confusing.

Question:
Would my datum be the axis of the part?
Wouldn't the datum on the OD or the ID be better- since this could be easily inspected?
How would this be called out in order for the drawing to make sense and allow for manufacturing as well as inspection?

jackboot

 

[drawoh]

Jackboot,

If you use either the OD or the ID as your datum, the datum is effectively on the axis.

The axis itself is not a physical entity, and its definition is ambiguous until you dictate which features define it. Off the top of my head, I can see six ways to define the centre axis, several of which will cause different results when you inspect the part.

Let's assume that the ends of your tube are not important, and that your requirement is to locate the OD and the ID to each other.

Question: Which feature can I jig to easily?

Let's assume for the moment that it is the OD.

I define my Datum A as the OD. I define the ID as concentric to Datum A.

Consider what happens if you do not apply a concentricity specification. The two diameters have tolerance zones that measure .0005" on the radius. These control concentricity. Each diameter can move .0005" off the theoretical centre, leaving you with maximum measured centering error of .001".

Let's try an alternate approach, where the end conditions do matter. At assembly time, we will push the tube up against a perpendicular surface, where it will locate to a raised, accurate button.

My Datum A will be the flat mounting surface at the mounting end. My Datum B will be the ID. I will apply a positional tolerance to the OD with respect to datums A and B.

In this scenario, Datum B is the circle where the ID intersects the end face defined as Datum A. There can be no concept of concentricity. The positional tolerance on the OD controls the location WRT the bottom of ID, and the perpendicularity WRT the end face.

The ID's perpendicularity is controlled by the diameter tolerance.

JHG

 

[drawoh]

Jackboot,

Correction.

I just reread the standard more carefully. The perpendicularity of the ID in my example above is controlled by the angular tolerance note on your drawing. ASME Y14.5M-1994 refers to this as an "implied 90 degree angle".

My understanding is that ISO assumes that you have a perfect 90 degree angle, and that your dimension tolerance controls the maximum angle. I would strongly prefer this.

If you want the ID to be concentric to the OD in my second example above, you would have to apply a perpendicularity specification from Datum A.

It all depends on your requirements.

Aren't you all sick of hearing this?

JHG

 

[Viktor]

Question:
Would my datum be the axis of the part?

The part does not have its own axis. Rather we should speak about the axes of ID and OD.

Wouldn't the datum on the OD or the ID be better- since this could be easily inspected?
It depends on the method of inspection. If you use a high precision collet to hold OD and thus to locate its axis and then check ID then the axis of OD is your datum. If you prefer to put the part on a precision measuring arbor having zero clearance and the check OD – then you better select the axis of ID as the datum. If you use a CMM then it doe not matter. However the measuring sequences and zero setting would depend on what you have selected as the datum. The same can be said about manufacturing sequence.


How would this be called out in order for the drawing to make sense and allow for manufacturing as well as inspection?

According to you choice of the datum (see above) you set the datum designation on your drawing.

For round parts the perpendicularity of its faces does not make sense – I would advise you to use runout which is actually measured.

I also disagree with the statement that “Each diameter can move .0005" off the theoretical centre, leaving you with maximum measured centering error of .001".” – it is not so.
Viktor

http://viktorastakhov.tripod.com