Tolerance on implied 90 angles.

[PeterStock]

I have a question that is derived from a drawing I recently checked. There were two values in the title block for angles, one of +/-2 degrees if the angle was stated as a whole number and one of +/- .5 degrees if the angle showed a decimal. My question is which applies in the case of an implied 90 degree angle?

My thought is that if I was making the part I would assume +/- .5 degress, but if I was inspecting the part, I would use the +/- 2 degrees as my accept/fail criteria. I am thinking that the 2 degrees would be what it would be rulled as in court (if it came to that).

What do you think?

Peter Stockhausen
Senior Design Analyst (Checker)
Infotech Aerospace Services

http://www.infotechpr.net

 

[Belanger]

I agree. It all depends on whether I'm the manufacturer or the customer!

Y14.5 says in paragraph 1.4.i that we are to assume a 90º angle. That sounds like a whole number to me, so I too would go with the ± 2º. But this is a lesson to all the kids out there to be extra careful with "assumed" things.


John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems

 

[dgallup]

That's one of the reasons we only put one linear and one angular default tolerance in our title blocks. Nobody has to guess. In the OP's case, I would interpret it to be +/-2 degrees.

 

[ctopher]

I don't like to imply any dim. If it's an implied 90 angle, show it as ref.

Chris
SolidWorks 10 SP4.0
ctopher's home
SolidWorks Legion

 

[Belanger]

But Chris, that would be too tedious. Label <b>every</b> 90º angle? That means a simple engineering drawing of a rectangular part would require at least 12 callouts for 90º (4 in each view, if the 3 traditional orthographic views are given.)

I think the clarification needs to be in the general tolerance, not in the decades-old practice of 90º implied angles.

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems

 

[Belanger]

Sorry -- forget to preview my post. One of these days I'll learn how to format in bold!

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems

 

[drawoh]

...

Y14.5 says in paragraph 1.4.i that we are to assume a 90º angle. That sounds like a whole number to me, so I too would go with the ± 2º. But this is a lesson to all the kids out there to be extra careful with "assumed" things.

It is a good idea to use GD&T profile tolerances systematically to control the outlines of your parts. It might be a surprise to people to find out just how inaccurate a tolerance of ±1[&deg;] is linearly.

I asked a while ago (thread1103-261904) about holes dimensioned from edges controlled by the angle tolerances on the tolerance block. We did not really agree on anything except that outlines defined by linear ± dimensions are not a good idea.

JHG

 

[ctopher]

Belanger,
Sorry should have been more clear. I'm not suggesting to label every angle, just the ones that there may be questions about. If you think an angle is implied, but not sure about it, just dim it and make it reference.

Chris
SolidWorks 10 SP4.0
ctopher's home
SolidWorks Legion

 

[powerhound]

I think the more likely scenario is that the person that created the drawing either doesn't know about the implied 90 rule or didn't think about the conflict his that his tolerancing scheme would create with it. Sticking with strict legalism, the drawing is open to more than one interpretation and violates fundamental rule 1.4(d) and is illegal. You should get with engineering and have them resolve it. On the other hand, sometimes you just have to get on with production so if +\- 2 deg will work anyway, I wouldn't bother doing a thing.

Powerhound, GDTP T-0419
Engineering Technician
Inventor 2010
Mastercam X4
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[dgallup]

Why on earth would someone create a 90 degree reference dimension? Since it is a reference dimension, it has no tolerance and does not need to be checked. Talk about the department of redundancies department!

 

[PeterStock]

Thanks all, you have confirmed my thinking. If in reviewing a drawing from this group, I find a implied 90 that needs to be held tighter, I will have them add the 90.0 degree dimension.

Peter Stockhausen
Senior Design Analyst (Checker)
Infotech Aerospace Services

http://www.infotechpr.net

 

[MintJulep]

I'm confused.

You're checking the drawing. So isn't your job to point out errors and ambiguities to the designer so they can be corrected?

You've found an ambiguity. Point it out to the designer.

 

[drawoh]

PeterStock,

Rather than adding a 90.0[&deg;] dimension to your drawing, just add a perpendicularity or profile specification.

The reason I usually apply profile tolerances around my outlines is that angle tolerances are sloppy when applied over long distances. If you have an edge 100mm long, a 2[&deg;] error moves the top by 3.49mm. If you reduce the error to 0.5[&deg;], your error drops to 0.87mm. This may still not be tolerable. If your holes are dimensioned from the angled edge, they will be out of position by 0.87mm, and that almost certainly is not tolerable.

Option 1 is to apply a more accurate angle tolerance, of say 0.05[&deg;] for an error of 0.09mm. Your fabricator will charge you an arm and a leg for that one.

Option 2 is to apply GD&T specifications to control the outline. A profile tolerance of 1mm allows ±0.5mm of wobble along the edge, making it equivalent to a ±0.3[&deg;] tolerance, but it will not be as expensive. This is precisely the situation where GD&T works.

JHG

 

[PeterStock]

MintJulip:
The ambiquity is not with the design, it is with the drawing format. This belongs to our customer and is not up to us to change. For the drawing I was working on, I did the dimensioning scheme, the ambiguity did not apply, controls were added that made the default angular tolerance unneeded.

Drawoh;
In fact on this drawing I did use profile and will as needed on others. But for some features, the angular tolerance may be more appropriate. I was just making the point that I would not be leaving any features that are implied 90 degrees that do need the tighter tolerance, refering to the looser tolerance by default. Profile will probably be one I use the most.



Peter Stockhausen
Senior Design Analyst (Checker)
Infotech Aerospace Services

http://www.infotechpr.net

 

[KENAT]

Peter, if the problem is with the format, which you can't change, then add a drawing note clarifying which tol applies for implied tolerances.

Posting guidelines faq731-376

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

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

 

[PeterStock]

That would also be an option when needed.

Peter Stockhausen
Senior Design Analyst (Checker)
Infotech Aerospace Services

http://www.infotechpr.net

 

[fcsuper]

I agree with KENET and others. The confusion comes from the fact that there are more than one tolerance applied to angles. I've not seen any scenario where this is helpful. Have one generic tolerance and then add tighter tolerances where needed is my first suggestion. If you are stuck with the multiple tolerance levels, then somewhere on the drawing you'll need a statement about which is applied to the implied 90.

Matt Lorono
Lorono's SolidWorks Resources & SolidWorks Legion

http://groups.yahoo.com/group/solidworks & http://twitter.com/fcsuper

 

[Belanger]

I still don't see why we can't just look to para. 1.4.i and say that the 90º is a whole number. That's what is says in black and white; there's no decimal point given in that paragraph's mention of the 90º.

I'm not advocating this practice, but in a GD&T "courtroom" I would say that the OP's scenario is covered. (But I guess that the question coming up is evidence that it should be more clear.)

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems

 

[drawoh]

I still don't see why we can't just look to para. 1.4.i and say that the 90º is a whole number. That's what is says in black and white; there's no decimal point given in that paragraph's mention of the 90º.

...

I think we have largely agreed on this.

"The part I have delivered to you is within 2[&deg;], therefore it conforms. Gimme my money!"

You know what happens next.

JHG

 

[fcsuper]

Belanger,

It is because the standard doesn't say it. The standard is in use in any non-standard way, then that non-standard use needs to be spelled out just the same an any other requirement not listed in the standard.

Matt Lorono
Lorono's SolidWorks Resources & SolidWorks Legion

http://groups.yahoo.com/group/solidworks & http://twitter.com/fcsuper