Symmetrical Tolerancing 2

[TomFin]

Hello World,
The part shown in the link is a hinge block. It is to be sent out for fabrication. I’d like to dimension the pin hole in such a way that variance occurring to the width of the bar stock will not cause the pin hole to be off center due to the fact the pin hole is dimensioned from one of the two vertical edges. This block is used multiple times in a weldment and both sides are used as positioning surfaces which is why I’d like to convey the importance of the pin hole lying mid-plane rather than just dimensioning off an edge.
Our drawing checker promoted a symmetry callout referencing the mid plane, but symmetry is only appropriate for non-cylindrical features and can be expensive to inspect (Geometrics III). The only dimensioning scheme I’ve come up with is positional tolerance relative to a datum, but then again the hole would still be dimensioned off 1 edge.
Then again it is bar stock which shouldn't have much variation. What do you think?


Failure is a prerequisite of successful design

 

[KENAT]

How about make .563 a 'datum' (asme y14.5M 3.3.2b, this invokes the center line as the datum).

Use positional tolerance on the hole, can't find an example with a hole in the standard but 5.60 is similar idea.

I'm not sure you properly define your end radius/overal length either but my brains aching, we just had lay-offs so someone check what I'm saying.

KENAT, probably the least qualified checker you'll ever meet...

 

[TomFin]

Always sorry to hear about lay-offs. *Fig 5.60 to avoid confusion. The picture provided is just a snippet of the actual drawing. Kenat, you're right in that it should state FULL R.

From Fig 5.60 refers to a center plane and a datum plane of the actual mating envelope. If I were to insert a diameter cylinder into the feature control frame to represent a cylindrical axis, then perhaps the same logic would apply, but to cylindrical tolerance zones. Is this sound logic?



Failure is a prerequisite of successful design

 

[KENAT]

Look at my attatchment, is this in the ball park? I've made some assumptions as I don't have all the info.

It assumes A is a surface the hole is perpendicular to.

I think per 14.5 para 1.8.4 it's R not FULL R.

Anyone want to pick my sketch apart;-)

KENAT, probably the least qualified checker you'll ever meet...

 

[powerhound]

Other than making the 1.000 a basic dimension, I think it looks good.

Powerhound, GDTP T-0419
Production Supervisor
Inventor 2008
Mastercam X2
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[ctopher]

... and the .281 basic.

Chris
SolidWorks 07 4.0/PDMWorks 07
AutoCAD 06
ctopher's home (updated 10-07-07)
ctopher's blog

 

[vc66]

I'm not sure the 1.000 and R should be basic. KENAT said that datum A is the surface perpendicular to the hole. That said, the 1.000 and R are not measure from any datums, are not the basis of any FCF's, and therefore shouldn't be basic.

Is it too early? Or am I right?

V

Mechanical Engineer
"When I am working on a problem, I do not think of beauty, but when I've finished, if the solution is not beautiful, I know it is wrong."

- R. Buckminster Fuller

 

[ewh]

I agree with vcastro66 about not making the 1.000 and the R dimensions basic. KENAT's sketch seems to address the OP well.

 

[ewh]

Oh yeah! Congrats on tipmaster of the week, KENAT! That should look good on your resume

 

[powerhound]

Yup, you're right vcastro. I looked at it too quickly. The bottom edge needs to be datum C and then the 1.000 made basic, that'll fix it. As it is, it's not a complete print.


Powerhound, GDTP T-0419
Production Supervisor
Inventor 2008
Mastercam X2
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[MadMango]

This block is used multiple times in a weldment and both sides are used as positioning surfaces which is why I’d like to convey the importance of the pin hole lying mid-plane rather than just dimensioning off an edge.

Doesn't the width .563 (datum B) need to be basic as well? Seems if both sides are critical, the width must be controlled as well.

"Art without engineering is dreaming; Engineering without art is calculating."

Have you read faq731-376 to make the best use of Eng-Tips Forums?

 

[KENAT]

Thanks ewh though based on the quality of that sketch not sure the tipmaster was deserved! Not sure how the heck I got it either, someone out there must like my ramblings. Maybe I'll post the email up on my cube wall next to my degree cert, but that's another topic;-)

Back on topic...

Refined sketch.

In mine I'd think 1.000 should be basic as the it locates the hole which is controlled by position. I'm sure I made it basic originally but then it must have got deleted or something and I didn't put it back (hey I said I was the least qualified checker you'll ever meet).

I dropped the R.281 as I think giving the overall length and width then "R" is probably better. Otherwise you have to look at locating the R on the hole which seems overkill.

Who said anything about R being basic?

I didn't initially want to assume the bottom edge was a datum because I didn't know all the details but it probably should be.

Anyway, I've made more assumptions, corrected an error and take a look.


KENAT, probably the least qualified checker you'll ever meet...

 

[vc66]

Shouldn't the 1.282 and R also be basic? The 1.282 is dimensioned off of Datum C and the R should be exact. Then you can put a surface profile callout under the R to complete it.

Maybe I'm going a bit overboard.

V

Mechanical Engineer
"When I am working on a problem, I do not think of beauty, but when I've finished, if the solution is not beautiful, I know it is wrong."

- R. Buckminster Fuller

 

[KENAT]

I didn't think a surface profile was probably required for the rad and hence no I dont' think 1.282 or R should be basic.

The designer would have to decide but even I'm thinking it's probably overkill for the application and that yes, you are going overboard;-).

KENAT, probably the least qualified checker you'll ever meet...

 

[TomFin]

MadMango,
I could probably specify the width of the bar stock using a basic dimension, but according to the drawing checker bible I'd have to call out both surfaces comprising the thickness as datums. I'm trying to keep this part as inexpensive as possible. Although now that I brood over this point I'm starting to worry about the consequences of thickness variance.

Kenat,
Congrats on Tip-master of the week! Hope you were able to finalize your roughness call out dilemma. I think you hit the nail or in this case pin on the head with your drawing. By the way is it necessary to specify the front face as a Datum? I'm assuming 'Yes' if I want the hole to be perpendicular to the face.Then again wouldn't we want to reface the oppositte face, the face it sits on as the drill approaches the part.

Failure is a prerequisite of successful design

 

[KENAT]

I just said "It assumes A is a surface the hole is perpendicular to."

You'd have to pick which surface is A based on function.

Someone else may be able to provide better guidance on this.

KENAT, probably the least qualified checker you'll ever meet...

 

[MechEng2005]

I'm not real familiar with GD&T or ANSI standards, but I'll throw my hat in anyway. =) Don't hurt nobody, right?

Could you just reference the hole center in subsequent assemblies and then the width isn't important?

Otherwise, I'd draw the hole off center and put a centerline on the bar and the hole. Then, just dimension the distance from the bar centerline to the hole centerline as 0.000 +/- 0.XXX. Of course, visually the drawing would not show it centered, but the dimension should control, not the visual representation.

On a side note, is the radius on the end of the bar even required? Wouldn't the bar width and the fact that it is shown as 180 degrees indicate that the radius is 1/2 of the bar width without need to dimension the radius? It could still be put in as a reference dimension of course.

-- MechEng2005

 

[ewh]

MechEng2005,
I'm not sure of the modeling procedures at the OP's place of business, but your suggestion would be breaking a primary rule at places I have worked. The part should be modeled at nominal, and that offset hole would never pass checking.
Then again, if solid models aren't used, the rules mqy be different.
"R" or "FULL R" should still be called out for the radius. The fact that it is 1/2 of the width only permits the omission of the actual size.

 

[KENAT]

MechEng2005 ,

Your suggestions probably wouldn't be 'best practice' for CAD as ewh points out and also to some extent from a drawing point of view.

Using the hole as essentially the assembly datum for alignment may have merit, depends on other unknown factors.

On your side note:

In my sketch the dimension of the radius is not needed however "R" to indicate full radius is necessary per ASME Y14.5M-1994. Simply showing 180 degrees isn't adequate, would most people spot the difference between 175 degrees and 180? For certain applications though this could make a difference.

The OP original sketch didn't have an overal length so did need the R.281 although I was wrong in my earlier post and it is fully dimensioned though possibly not in the best wasy.

"It could still be put in as a reference dimension of course." Excessive use of reference dimensions is generally considered bad practice and discouraged by the standard, can't recall the reference.

KENAT, probably the least qualified checker you'll ever meet...

 

[ewh]

Para 1.4(c)
"... No more dimensions than those necessary for complete definition shall be given. The use of reference dimensions on a drawing should be minimized."