Positional Tolerance 2

[Seco1]

We have a discrepancy between options about the positional tolerance of a drilled hole in a cast part. I would appreciate anothers opinion. The drawing calls out the following tolerance (as closely as I can imitate the actual call outs, I wish I could attach a drawing):

4 HOLES (diameter symbol)9.0 +-0.2
(control frame)|(position symbol)|(diameter symbol)0.3|A|B|E (end of control frame)
CHAMFER (diameter)10.2 +-0.2 * 45

The horizontal and vertical linear dimensions (for one hole for example) are marked as 29 (horizontal from center) and 50.23 (vertical from center). There is no specific tolerance called out on these dimensions. The title block also has a note about unspecified tolerance on linear dimensions equal +-.2.

What linear tolerances apply to this 9mm hole?

Thanks in advance,

Steve

 

[ewh]

What good is a positional tolerance on a +/- located feature? The positional dimensioning should somehow relate back to your datums, and should be basic.

 

[Heckler]

The locating dimensions must be basic. You can calculate what the linear tolerances would be if you were not using the true position callout....remember the square inscribed in the circle

Best Regards,

Heckler
Sr. Mechanical Engineer
SW2005 SP 5.0 & Pro/E 2001
Dell Precision 370
P4 3.6 GHz, 1GB RAM
XP Pro SP2.0
NVIDIA Quadro FX 1400
o
_`\(,_
(_)/ (_)

Never argue with an idiot. They'll bring you down to their level and beat you with experience every time.

 

[Seco1]

I'm sorry I did not make myself clear ... these are not my drawings or can I change them in any way. I'm simply trying to interpret what is already there. I'm just not sure how to. Well, I'm pretty sure I get what the drawing is getting at, but them someone says your wrong, doubts creep in and you post on message boards . The main discrepency is the linear tolerancing of the hole position. Is it a priority issue (.3 in the control block or .2 in the title block)?

 

[ewh]

You could play it safe and ASSUME the locating dimensions are basic, or you could assume that the geometric control is in error. I would play it safe and consider the dimensions basic (provided they do link back to the referred datums).

 

[Heckler]

Since the True Position is taken at RFS (regardless of feature size) you get no bonus tolerance from the feature tolerance. The title block tolerances should only apply is no other tolerances are specified. Their should be a note somewhere in the title block that states "Unless Otherwise Specified"

Have you had any formal training in the area of GD&T?

 

[kbro151]

I actually don't think this one is that confusing. Before the days of CAD, a lot of effort went into ensuring that drawings were as simple as possible, with the minimum of data required. It took a long time to add dimensions, notes, callouts, etc. I know times have changed, and it is now quite easy to overdimension or put notes in everywhere. If I had a drawing like Seco1, I would assume:

1) title block doesn't apply whenever someone goes to the trouble of specifying a tolerance, and

2) no one 'accidentally' adds a positinoal tolerance callout.

I know, never say never, but this would be my starting point.

Things that supoprt it are heckler's points about rfs and the usual notes in a tolerance block that qualify when the block is applied, and the fact that the positional callout is tighter than the tolerance block.

 

[Seco1]

Thank you for your replies. Personally, no I wouldn't say I have formal training in GD&T, but many years of practical experience. In a nutshell, we are a manufacturing plant and I disagree with the customers interpretation of the tolerancing on this old drawing. I too have been assuming basic location tolerancing. Of course the customer is always right, but if I could show the purchasing agent (who does know anything about GD&T) something concrete it would make my life considerably less complicated. I spent sometime checking ASME today, but have not yet found anything. I was hoping to be able to craft (or find one) a simple explanation of standards, not that they necessarily have to follow standards.

 

[ctopher]

Is the chamfer dia suppose to be part of the FCF?
I would make it a separate callout.

Chris
Systems Analyst, I.S.
SolidWorks 06 4.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 10-27-06)

 

[KENAT]

Sounds like they just forgot to put the box around the basic dimension. I'd treat the 29 and 50.23 as basic.

 

[Heckler]

I told you an explaination, according to you original post it's true position regardless of feature size of DIA 0.3 mm.....so in practical terms regardless of what size the feature comes in between 8.8 - 9.2 mm it's location must be within a 0.3 mm diameter tolerance zone. This translates into +/- 0.21 mm linear tolerance if you do the math....remember the diameter with the inscribed square I was talking about earlier...... the diagonal of the square is 0.3mm so the leg is Cos 45 = leg/0.3 = 0.21

Best Regards,

Heckler
Sr. Mechanical Engineer
SW2005 SP 5.0 & Pro/E 2001
Dell Precision 370
P4 3.6 GHz, 1GB RAM
XP Pro SP2.0
NVIDIA Quadro FX 1400
o
_`\(,_
(_)/ (_)

Never argue with an idiot. They'll bring you down to their level and beat you with experience every time.

 

[ewh]

kbro151,
If you are drawing to ASME Y14.5, nothing has changed in regard to simple drawings. It is still standard practice to include the minimum number of dimensions needed to make the part. A good drawing is a concise drawing. Be it a board drawing or a CAD drawing, this still applies.

 

[ewh]

Seco1,
If the purchasing agent knows something about GD&T, just showing him the situation should be enough without having to provide concrete evidence for your position.

 

[kbro151]

Seco1, Machinery's Handbook has a table in the inspection section that is simple enough for even a purchasing agent to understand. It clearly says position callouts use basic dimensions and RFS is implied unless MMC or LMC is stated.

ewh, of course drawings should still be simple and concise. My point was that it is incredibly easy these days to overdo it. It takes 10 seconds to add a dimension. It used to take a few minutes, more if you had removed the drawing from your desk. In the time it now takes to dimension and add callouts, you used to have plenty of time to consider the necessity of a note, callout, or dimension. That time and incentive to think was built in. Now, it isn't. Usd to be learning to draft took a big time investment. Now the time to produce working drawings is much, much shorter. This is one reason why, in my experience at least, we have a lot of drawings being dranked out for production by a bunch of folks with a less than perfect understanding of drawing, never mind GD&T.

 

[ewh]

Which is why I miss good drawing checkers...

 

[kbro151]

lol....

are you saying that you still have checkers? Never mind good ones...

I have to badger ppl to check my drawings around here.

 

[ewh]

Checker is one of the hats that I wear around here. Problem is that I create many of the drawings, and it is hard to get someone to check my drawings as critically as I do theirs.

 

[danap2005]

From ASME Y14.5M-1994

4 HOLES (diameter symbol)9.0 +-0.2
(control frame)|(position symbol)|(diameter symbol)0.3|A|B|E (end of control frame)

The center of the hole (9.0) has to be inside a circle of 0.3 where the center of that circle is located at 29 (horizontal from center) and 50.23 (vertical from center) - This assumes the 29 & 50.23 are BASIC(read as "theoretically exact, ideal, nominal"), there should be a note somewhere that states UNTOLERANCED DIMENSIONS LOCATING TRUE POSITION ARE BASIC.

If you want to use plus minus dimensions you would divide the tolerance by 2 and multiply by 0.707: (0.3/2)* 0.707 = 0.11 so the tolerance is now +/-0.11

Doing this would not violate the customer specification of being within 0.15 of the BASIC or nominal hole location.

 

[ringman]

Does the drawing make reference to Y14.5 as being applicable? Do you have any insight as to the mating condition of the holes?
These are some factors tneed to be taken into account when specifing the tolerances for the holes. with that being said.......

If Y14.5 is referenced.the 0.3 in the callout will be the diametric tolerance.

 

[Seco1]

Thanks again, this is great help. The drawing does not reference any standard, but it was originally from a source in europe. If the date is accurate it is from '92. There are no notes about basic tolerancing, only the note about unspecified tolerances. If I had to guess, this drawing may have been converted at some point in the past, maybe from hand drawn to digital or from one company to another because of a buyout. That's just a guess though based on several inaccuracies.