Continue to Site

Eng-Tips is the largest engineering community on the Internet

Intelligent Work Forums for Engineering Professionals

  • Congratulations KootK on being selected by the Eng-Tips community for having the most helpful posts in the forums last week. Way to Go!

Using Profile to position a feature?

Status
Not open for further replies.

randy64

Aerospace
Jul 31, 2003
170
Very simple part. A rectangular hole in a rectangular block. Rectangular hole size is dimensioned with basic dim's and has a profile callout pointing to it. Three datums called out - bottom (A) of block and two edges (B & C). Profile is called out to all three datums. There are also basic dim's locating the rectangular hole from the edges (datums B & C).

Local "expert" says this is okay, that we can use profile to locate the rectangular hole. I disagree, argueing that profile is a tolerance of a feature size, not a tolerance of location. Therefore, dim's that locate rectangular hole should become unbasic, or just toleranced dim's - OR - add positional tolerance callout to rectangular hole and keep dim's basic.

Who's right?

Thanks
 
Replies continue below

Recommended for you

Profile can be used to control size, form, orientation, and location (per Y14.5-1944, para 6.5.1). Your expert is right. Figure 6-19 in same spec is probably close to what you're describing.
 
Looks like the profile in this case was used correctly. Profiles do NOT reflect features of size but surfaces and it looks like the surfaces are reflected from datum B & C and, probably, perpendicular to datum A.

One could also have used a positional tolerance if the hole was shown as a feature of size with tolerances with basic dimensions to its centre.

Dave D.
 
SteveMartin, I see in 6.5.1 it says "location", but I've never seen it applied that way.

Figure 6-19 was my suggestion on the way it should be done. It shows positional tolerance. As it is, the only control frames on the drawing in question are the profile for the rectangular hole and profile for the outside edges of the rectangular block. They are each held to different tolerances. I just don't see how that can relate to location. If it can relate to location, what is the tolerance of the basic dim's that locate the rectangular hole?

Not trying to be contrary, just trying to wrap my head around something that seems illogical to me.

Thanks.
 
randy64,

Can the profile tolerance be inspected?

Will a part that conforms to the profile tolerance work?

Will a part not conforming to the profile tolerance not work?

ASME Y14.5M is a language, not a procedure. There usually is more than one way to express your requirement, although there are often subtle differences in the resulting geometry. A profile tolerance explicitly shows an MMC, which probably, is what you need. The geometry shown by a positional tolerance and ±[ ]tolerances on the slot show something a little more complex.

Critter.gif
JHG
 
drawoh, I'm not sure I see what you're saying has to do with my question. My question concerns how the profile callout can be used to locate the rectangular hole within the rectangular block. Since both rectangular shapes have a profile tolerance that means their edges must fall within their respective tolerance "bands" or "zones." What I don't see is how those profile callouts can have anything to do with actually locating one feature (or their tolerance "bands") to another.


???????
 
Sounds like your expert is correct, and that it's a permissable way of handling this.

In fig 6-19 the positional tolerance is effectively a refinement.

It will come down to function if the extra control is needed.

Your idea of combining basic & +- dimensions in your OP sounds incorrect.

KENAT,

Have you reminded yourself of faq731-376 recently, or taken a look at posting policies: What is Engineering anyway: faq1088-1484
 
I agree as well, the situation you have described is valid and legal. As Dave said, profile is not applied to features of size but rather the profile of the feature.

Powerhound, GDTP T-0419
Production Manager
Inventor 2009
Mastercam X3
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II
 
Okay. I guess I'm not being clear. If you look at Fig 6-19, that is pretty much my situation, with the following three important differences: (1) There is no positional tolerance, (2) there is a profile callout to the outline of the block and (3) the profile callout to the interior feature (in my case a rectangular hole) is called out to 3 datums, A, B & C.

Given that, my question is: What is the tolerance (or more specifically, where would I find the tolerance) on the basic dimensions that locate the interior feature (in Fig 6-19 it's the 25 dimension)?

So far a couple of you have said "the expert is correct", but haven't answered my specific questions. I guess I can accept that I'm wrong if someone would explain to me how you can use profile to locate features. No one has done that yet.

Again, not trying to be nasty, but I need and want to know this stuff so I can be able to defend/explain it to my customer and my detailers.

Thanks.
 
The combined basic dimensions (& geometry) define the theoretically perfect form/location/orientation etc. of the surfaces.

The profile tolerance then defines how much the actual surfaces are permited to vary from that.

The point is the surface profile tolerance controls location as well as the other things. The location tolerance is part of the surface profile tolerance.

KENAT,

Have you reminded yourself of faq731-376 recently, or taken a look at posting policies: What is Engineering anyway: faq1088-1484
 
"The location tolerance is part of the surface profile tolerance."

This doesn't answer my question. Specifically, how is the location tolerance discerned from the profile tolerance? Is there a formula to do this? Is a percentage of the profile tolerance used to determine the location?

Here's the way I see it: If you have two features that have profile tolerances called out to them, they are independent of each other. Profile only controls the form of each feature independently. Putting a basic dimension between the two features does not control location via the profile. I think you need another control, like positional tolerance, as shown in Fig 6-19.

I am trying to be open minded on this, but so far nobody has taken the time to fully explain how this would work using only profile tolerancing.

Thanks.

 
Let me try to explain it this way. The basic dimension from a datum edge to one edge of the cutout is what positions your tolerance zone. The actual profile of that cutout edge has to fit inside that tolerance zone. It's kind of futile to determine a positional tolerance from a profile tolerance because they are 2 different things. Position regards the location of a centerplane or axis while profile regards the location of an actual surface.
Look at Fig. 6-26 and disregard the lower portion of the composite FCF. Notice how the tolerance zone is defined as being 0,8mm wide. The tolerance "channel" is 55mm wide from center to center and 40mm high from center to center. The channel is now positioned 20mm from datum B to the center of the left side of the channel and 20mm from datum C to the center of the bottom of the channel. This is how the tolerance zone is located and the edges of the cutout must fall within the tolerance zone at all points. Also remember that the toleance zone is perpendicular to datum A.

Powerhound, GDTP T-0419
Production Manager
Inventor 2009
Mastercam X3
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II
 
powerhound, are you saying that the 8mm tolerance applies to the 20mm locating dimension? And then once that is established, it also applies to the size of the tolerance zone?

Another way to ask: You say "The channel is now positioned 20mm from datum B to the center of the left side of the channel and 20mm from datum C to the center of the bottom of the channel." What is the tolerance on the 20mm dimension?

Also, I'm assuming that the "channel" is actually the tolerance zone and not the size of the feature.

Thanks.
 
Remember that the 20mm dimension is telling you where the tolerance zone is, not the edge of the feature. The edge of the feature has to fall within the tolerance zone. There is no tolerance on the location of the tolerance zone, it is located theoretically perfectly.

The tolerance of the 20mm dimension is comprised of the amount that the edge of the cutout can vary within the 0,8mm tolerance zone. It could effectively be +/-0,4 but to couch it in those terms could lead one to believe that it is a feature of size, which it's not.

Powerhound, GDTP T-0419
Production Manager
Inventor 2009
Mastercam X3
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II
 
randy64,

Here's another way of explaining the upper callout in Fig 6-26 (the surface profile of 0.8 to A, B, and C).

The profile tolerance for the cutout defines a tolerance zone that is 0.8 thick. The inner and outer zone boundaries are each offset by 0.4 from the basic geometry shown on the drawing (the 40 x 55 rectangle with R5 fillets). This zone controls how large or small the cutout can be, as well as its form.

The Datum A reference requires that the zone must have an exact (basic) relationship to Datum A (in this case, the relationship is exactly perpendicular).

The Datum B reference requires that the zone must have an exact (basic) relationship to Datum B (in this case, the middle of the left-hand section of the zone must be exactly 20 mm from Datum B).

The Datum C reference requires that the zone must have an exact (basic) relationship to Datum C (in this case, the middle of the lower section of the zone must be exactly 20 mm from Datum C).

So the cutout must fall within the tolerance zone, and the tolerance zone is at an exact location relative to B and C (two outside edges).

Evan Janeshewski

Axymetrix Quality Engineering Inc.
 
axym, thank you. Your explanation is the first that begins to make sense to me.

If I understand it, this is similar to positional tolerance in the following sense: The basic dim's from the datums locate a perfect point which is the center of the diameter, or cylinder, that the center of the hole must rest in.

Is this correct?

Thanks
 
Forgot to finish my thought.

Using profile to locate uses basic dim's from the datums to locate the perfect (or exact) center of the tolerance zone that the outline of the feature must rest in.

Right?

Thanks again to everyone for their patience.
 
Randy, it sounds like you're having real difficulty understanding the concept of profile tolerance. I suggest you take a look at ASME Y14.5M-1994 section 6.5. If you still are having difficulty maybe talk to your local expert and see if he can explain it or get some training if you can. A text book may help.

There is no tolerance on the 20mm dimension. The 20mm dimension is giving you the theoretically perfect location. The profile tolerance is telling you how far the real surface can vary from that.

KENAT,

Have you reminded yourself of faq731-376 recently, or taken a look at posting policies: What is Engineering anyway: faq1088-1484
 
randy64,

I am looking at Figure 6-19 in ASME Y14.5M-1994.

The profile tolerance on the hole is 1.2mm. The positional tolerance is Ø0.5 at MMC. They are locating a sloppy feature accurately. The profile tolerance on its own, allows a positional error of 0.6mm. The drawing would be equally valid without the positional tolerance, but presumably, the part would be less functional.

I use profile tolerances on my outlines more often than not nowadays. If you apply ±[ ]tolerances, the angle tolerances on your tolerance block apply, and that generally is not accurate enough. ±[ ]tolerances can be safely applied to well defined outlines.

Critter.gif
JHG
 
KENAT, I think I have a pretty good concept of how profile tolerancing works, I've just never seen it applied to locate a feature, and didn't think it could be used that way. I always thought of profile as a completely independent tolerance, kind of like flatness or parallelism. I had always applied it to the outside outline of a part, not as a locating device for an interior feature.

Apparently my thinking was wrong.
 
Status
Not open for further replies.

Part and Inventory Search

Sponsor