Projected Tolerance

[mart0528]

I need some help on projected tolerance. I haven't taken a GD&T class yet, so this mught be a basic question. I have a CT-50 taper shank shrink fit tool holder. The shank of the holder is datum A. As of now the company tolerances the bore to the shank as .0002" concentric to A. I need to have a projected tolerance of .0002" to datum A, 4 inches from the nose of the holder. What is the best way to acomplis this? Secondly, after researching my question, is concentricity the proper tolerance for the bore for this or is runout a better idea? Thanks.

 

[drawoh]

mart0528,

This sounds like more of a design question than a drafting question. What is being located by this thing?

I tend to use position tolerances on stuff like this, but it all depends.

Could you show us a drawing?

JHG

 

[KENAT]

If it's for interchangeability then probably position.

If it's for alignment etc then runout/total runout would be worth looking for.

I've come to realise that concentricity is pretty limited in its applications so you're right to question.

A picture paints a thousand words per drawoh...

 

[mart0528]

I know what I want, and it's designed. I just don't know how to express it using the proper drafting standards. What I want to express is basically shrinking a 'perfectly straight' pin into the holder and measure the runout or concentricity 4 inches from the nose and keep a tolerance of .0002". Is position the proper way to do this and do I need more datums for position?

How do I insert a sketch here? I can't seem to figure it out.

 

[mart0528]

Figured it out.

http://www.mooload.com/new/file.php?file=files/180706/1153234637/ct50.doc

 

[MechNorth]

Hello Mart,

First, thanks for clarifying that you haven't taken any GD&T courses yet...has anyone at your company? Not meant as sarcasm, but rather as concern. These parts are quite pricey (at least from the purchaser's perspective) and they are by necessity quite precise.

I have a couple of concerns; first, there are no controls shown for the conical taper surface which generates Datum-A. I worked with conical tapers in the .0002" diametral size tolerance range for about 10 years, and for the last few of those, I was working on the best way to GD&T them. Second, most people aren't aware that a conical taper actually generates three datum planes; two mutually perpedicular at the axis of the cone, and the third at the apex of the cone which is typically a projected point in space and therefore a useless generator of a datum plane. The issue there is that the surfaces perpendicular to the axis are then located wrt the apex of the cone...not a good idea. Better to put a note with -A- callout that restricts it to "GENERATES 2 DATUM PLANES THROUGH AXIS ONLY", and then designate the back face of the flange as the secondary datum feature -B-. The conical surface should have a Surface Profile control tying it to Datum -A-, and the Secondary datum feature should reference it back to Datum -A-.

As for your Projected tolerance zone, you did the feature control frame correctly. Kenat's comment above is correct; Concentricity has very limited use, and there is considerable talk about removing it and symmetry from the next version of the standard. Use Total Runout instead, with a tolerance tighter than the size tolerance, otherwise it is redundant by Rule #1.

One final suggestion, get some GD&T training for your engineeering & manufacturing personnel. There are a number of highly-reputable trainers around that do in-house and seminar-style training all over the USA, Canada, and into Europe. My preferences are Tec-Ease (

http://www.tec-ease.com)

and iigdt (

http://www.iigdt.com).

Tec-Ease in particular is very helpful with their unlimited after-training support; they trained and mentored me through my GDTP-S certification.

Good luck!
Jim


Jim Sykes, P.Eng, GDTP-S
Profile Services
CAD-Documentation-GD&T-Product Development

 

[ringman]

MechNorth,

Your take on the conical datum is interesting. How do you define the datum. I believe that the axis alone does NOT ESTABLISH the 2 mutually perpendicular planes, but that they are established only when a tiertiary datum is required and applied.

I cannot recall seeing the interpretation of a datum point at the apex.

I was not able to access the link to mooload, can you help me on that please?

Thanks

 

[MechNorth]

Hi Ringman,

Y14.5M-1994, Section 4.4.2 Parts With Cylindrical Datum Features; "A cylindrical datum feature is always associated with two theoretical planes intersecting at right angles on the datum axis. The datum of a cylindrical surface is the axis of the true geometric counterpart of the datum feature..., and simulated by the axis of a cylinder in the processing equipment. This axis serves as the origin of measurement from which other features of the aprt are located." See also Fig. 4-5.

The standard outlines basic fundamentals or principles, but unfortunately doesn't provide much guidance on some of the more challenging real-world situations that we all encounter. Instead, they expect us to make logical extensions and correlations of the principles to new situations. A conical surface used as a Datum Feature is one of these situations.

By extension, the surface of a cone has an axis which is the datum (the result of an infinite number of center points of opposed points around the cross-sections along the length of the cone). Similarly, by extension the axis of the cone generates two mutually perpendicular datum planes which are the origin of measurements in 2 directions away from the axis of the cone.

The next part is the real challenge, and I came to understand it as the result of discussion and debates with several of the people who actually write the standard. Whereas the cylindrical surface is always parallel (or equidistant if you prefer) to the axis of the cylinder, the surface of a cone converges at the cone's apex. This point is effectively a limit or origin of the axis, and therefore the origin of measurement along the axis (the axis is, as always, theoretical and extends infinitely in both directions beyond the apex). Added to this, measurements originate at datum planes. By combining the two, the apex of a conical surface therefore generates a datum plane which is mutually perpendicular to the two datum planes generated by the datum axis. Furthermore, this third datum plane (not tertiary, but third) is the origin for measurements along the axis.

It's a lot to take in, and not easily understood. For that reason, many senior GD&T experts will go to extreme lengths to avoid using a cone as a datum feature; some people add non-functional features such as cylindrical and planar surfaces to bypass the situation.

If the link isn't even launching your internet browser, try copying the address it into your browser. If it's launching the browser but not going beyond that, you may need to accept Mooload.com's cookie. Once you get into the site, under the bolded DOWNLOAD LINK is a hyperlink "Click Here To Download". If there's still no luck, post again.

Hope I've been able to help.

Jim

Jim Sykes, P.Eng, GDTP-S
Profile Services
CAD-Documentation-GD&T-Product Development

http://www.profileservices.ca