Verification of Profile of Surface tolerance

[brandnew1]

This is probably a simple question, i believe the standard (1994) explains it but i just wanted to verify with others who are more knowledgeable than me.

The attached pdf shows a part in which a 'profile of surface' of .020 to Datums A & B is called out, with all dimensions boxed in as Basic.

My question deals with the 1.825 diameter in which actual measurement is .0106 undersized (1.8144).

According to Y14.5-1994 section 6.5 Profile Control:"...the true profile may be defined by basic radii, basic angular dimensions, basic coordinate dimensions, basic size dimensions..." i looked at figure 6-17 which calls the diameters to be within the .025.

So in the case of the attached pdf, will this tolerance be a +/-.010, thus the measurement falls out of tolerance?

In the CMM program, the profile of surface has a +/-.010 due to form and location callout, but the actual profile measures to roughly -.006, according to the CMM it appears to still pass even though its below the .010 mark.

Can someone shed some light on this for me?! Thank you for your time and help

 

[pmarc]

I am not sure I get your point corrrect, but the fact that the size of diameter is 1.8144 does not automatically mean that the surface of this feature is outside of profile tolerance zone. Keep in mind that by the definition profile of surface tolerance is not verifying size of a feature, it is checking whether the feature surface lies within tolerance zone which is defined by size basic dimension.

 

[brandnew1]

i'm just trying to understand if the undersized diameter is acceptable or not...Normally when it comes to basic dimensions i'll see something like a feature control frame that will give me acceptable tolerances to a feature.

In this case, all the dimensions, diameters and angles are all boxed in (Basic) but there is no mention of tolerances or anything of the sort except for the profile of a surface callout to .020 of Datum A & B with the "all around" symbol pointing to this callout.

i believe a surface of profile in this case is bilateral thus needing to be within the .020 all around the part. i'm uncertain however if this means that the tolerance for this diameter is 1.825 +/-.010 but profile says it is good.

So is this diameter acceptable?

 

[pmarc]

What I meant to say was that you have to check whether the surface of feature is within the profile tolerance zone - and this is what CMM should do. By measuring the diameter value only you are not able to tell this.
1.8144 itself can't provide you information that you are inside or outside of the tolerance zone for profile callout because by nature it is not checking location of actual profile of a part.

 

[pmarc]

By the way, if you imagine a circle of basic dia. 1.825 and profile callout 0.020 applied to it, the smallest actual circle you can get is 1.805 and the biggest is 1.845. So 1.8144 is well inside that.

 

[KENAT]

Profile controls location & form & size. However, that doesn't necessarily mean you can just add up the size deviation and location deviation - though that will give you a crude approximation if you do it right allowing for the pseudo 'MMC' effect.

Posting guidelines faq731-376

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

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

 

[brandnew1]

Thanks PMARC for your help...so from what i understand, as long as this portion of the part measures within the given profile tolerance than the part should be ok even if the diameter is .0105 below the basic diameter. =)

 

[pmarc]

That's right - profile deviation is all that you have to look at in this case.

 

[MechNorth]

To reinforce what PMarc has said;
A surface profile is a boundary control; as long as the feature is within that boundary, that's all you care about. In this case, your boundary is centered on the datum-B axis. So, you set up the workpiece using datum simulators for datum-A and datum-B, then master your indicator at .9125" from the axis of the simulator. As you rotate the part about the datum axis simulator and move the indicator over the cylindrical surface, as long as your indicator doesn't move more than +/- .01" then you're ok. The CMM just does this all behind the scenes which makes it more confusing.

Jim Sykes, P.Eng, GDTP-S
Profile Services

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com