×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Symmetrical Tolerancing
2

Symmetrical Tolerancing

Symmetrical Tolerancing

(OP)
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

RE: Symmetrical Tolerancing

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...

RE: Symmetrical Tolerancing

(OP)
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

RE: Symmetrical Tolerancing

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 apartwinky smile

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

RE: Symmetrical Tolerancing

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

RE: Symmetrical Tolerancing

... and the .281 basic.

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

RE: Symmetrical Tolerancing

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

RE: Symmetrical Tolerancing

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

RE: Symmetrical Tolerancing

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

RE: Symmetrical Tolerancing

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

RE: Symmetrical Tolerancing

Quote (TomFin):

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: Eng-Tips.com Forum Policies to make the best use of Eng-Tips Forums?

RE: Symmetrical Tolerancing

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 topicwinky smile

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...

RE: Symmetrical Tolerancing

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

RE: Symmetrical Tolerancing

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 overboardwinky smile.

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

RE: Symmetrical Tolerancing

(OP)
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

RE: Symmetrical Tolerancing

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...

RE: Symmetrical Tolerancing

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

RE: Symmetrical Tolerancing

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.

RE: Symmetrical Tolerancing

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...

RE: Symmetrical Tolerancing

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."

RE: Symmetrical Tolerancing

I believe the locus for the hole should be a rectangle rather than diametric. If that is the case there is no need for the 1.000 to be a basic dimension.  Nor is there a need for datum feature C.

Has it been determined that Y14.5 is applied to the drawing in question?

RE: Symmetrical Tolerancing

Correct me if I am wrong but I don't think you actually need the 1.282 dimension.
You have already specified the width of the part and that controls the size of the radius (hence the "R" callout) and if the hole is concentric to the radius (which I infer from there not being a second centermark) then an additional height dimension is redundant.

David

RE: Symmetrical Tolerancing

...nor would a feature control frame be legal to use, nor would there be any need to use GD&T at all or reference anything like the ASME standard. That would effectively be converting the whole thing to coordinate dimensioning which in itself has so many disadvantages that that was the reason that GD&T was developed in the first place.
  The person that posted the OP is the one doing the drawing so I would imagine he is trying to conform to the ASME standard if he's asking us about it.

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

RE: Symmetrical Tolerancing

The above is in reference to ringmans post, not aardvarkdw's

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

RE: Symmetrical Tolerancing

(OP)
Powerhound, you're right. I am trying to veer away from coordinate dimensioning and implemement GD&T for the sake of assembly.

Failure is a prerequisite of successful design

RE: Symmetrical Tolerancing

Ringman, why square?  The location is to the radius as well as width so I think circular makes sense.  The Ops main concern was on centering the hole wrt the width.  What you’re proposing would lose this, in fact you don’t even address it.

That said a square zone could be achieved by dropping the diameter symbol from the FCF while still having the benefit of centering the hole wrt the width.

The OP & I traded quotes from 14.5 so I think it’s reasonable to assume it applies.  However, just to be sure TomFin do you invoke ASME Y14.5M-1994?

aardvarkdw, did you not see the other thread on coaxiality?winky smile  You cannot infer coaxiality/concentricity just because the radius is shown coaxial to the hole.  That is why the height is given.  Now if you want to use a geometric control of the radius to relate it to the hole you could lose the height but this seems over the top  for the application.  

However, this is based on my best guess of function as I don’t’ have all the information.

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

RE: Symmetrical Tolerancing

(OP)
Yes I am invoke ASME Y14.5M-1994 as I referred to it as the bible in a previous post.

Failure is a prerequisite of successful design

RE: Symmetrical Tolerancing

Well, if the hole is to be located symmetrically wrt the width, the result would be a zone with the width allowed extending the length of the part.  The 1.00 dimension with the tolerances provided would likewise result in a zone bounded by 2 planes the width allowed.  The resultant zone for the location of the hole then would be a rectangular, if not square zone rather than diametric. Diametric zones work well for round fastener holes when they are a part of a patterm of holes.   

RE: Symmetrical Tolerancing

Actually diametric tolerance zones work well in all cases for which they are applicable. If you can think of a single instance where a square tolerance zone works better than a cylindrical one, please explain it to me.

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

RE: Symmetrical Tolerancing

Ringman,

I suppose you could just use positional on the width and use coordinate for the length but this doesn't seem like good practice.  Also I think a circular zone is probably appropriate in this case.

Powerhound

I had a case recently where square was better than round.  Basically a case of intersecting holes.  A screw came down one and had to 'clamp' a round shaft in the other as I recal.  I could actually use a larger 'square' zone than I could 'round' zone.  Make sense?

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

RE: Symmetrical Tolerancing

IF you would liook at the fig 5.21 in the Std., and at the pattern of holes in the lower left portion of the part.  The composiite tolerancing has a diametric zone specified for both the pattern locating tolerance zone and the Feature locating tolerance zone.  I believe if you will explore the possibilities on an enlarged drawing, you will find that the rectangular zone would provide not only a '(bonus)' tolerance but would also allow a more precise method of determining the min. edge distance for the hole pattern.  

This would approximate what was used years back  when the pattern was allowed to be located by plus and minus dimensions.  My personal opinion is that something was lost in the updating of the std.

RE: Symmetrical Tolerancing

ringman, is this in response to Powerhound 'cause you've lost me as it applies to the OP?

Because of the impact of 'wall thickness' in the portion of the hole sat in the radius, I think based on the information to hand that a diametric zone is appropriate.

If the function dictates otherwise then the designer should consider this but from what information he gives I think diametric makes sense.

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

RE: Symmetrical Tolerancing

I'm starting a new thread on square tolerance zones.

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

RE: Symmetrical Tolerancing

Powerhound,

Good idea! It will work for rivet holes too.

RE: Symmetrical Tolerancing

Going back and rereading the OP, the piece is used in a weldment.  On that basis, it is unlikely that interchangeability is a consideration in any manner.  Hence it wsould seem overkill to get carried away with much if any positional tolerancing.  Comments?

RE: Symmetrical Tolerancing

(OP)
Ringman,

   You appear well-versed in the standard and thankyou for chiming in. But in response to

Quote (Ringman):


"the piece is used in a weldment.  On that basis, it is unlikely that interchangeability is a consideration in any manner.  Hence it wsould seem overkill to get carried away with much if any positional tolerancing.  Comments?"

    Yes this block and it's mating block are used in separate weldments call them A&B,that must align for the hinge pin. As a matter of fact interchangeability is a consideration, for the block is ambidextrous. With our mfg production rack containing ~30 weldments each of type A & B, an assembler with a random pick of an A and of a B must be able to tap the pin through both mating blocks without too big of a hammer :) Unless I've missed the boat on what you define interchangeability as, then I believe it isn't overkill to use positional tolerancing for this case.

Failure is a prerequisite of successful design

RE: Symmetrical Tolerancing

Tom Fin,

Again, if I am reading this correctly, the matter of alignment or interchangeability would be handled at the next assembly level of the drawing.  Not on the single hole of the detail part.

RE: Symmetrical Tolerancing

I would find out how these parts are fixtured in the weldment to determine what the datums need to be.  Does it hold the part in space by the sides of the part, or does a pin slip in the hole for alignment?  Is there slop in the fixture, or is everything tight?  I'm starting to see where Ringman is coming from, there is no need to increase the cost of this part by applying unnecessary GD&T requirements if the fixture does it's job correctly.

Having said that, it does sound more and more like the width of the part and the location of the "hinge pin" hole is critical in your part.  I'm thinking perhaps a parallelism control between the indexing faces and tight tolerances on the hole position should be applied (Basic dim on the width and Positional location of the hole).  The diameter of your hole may also require some additional care to allow for misalignment, distortion during welding, pin insertion, etc.  How far apart is the second block?

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

Have you read FAQ731-376: Eng-Tips.com Forum Policies to make the best use of Eng-Tips Forums?

RE: Symmetrical Tolerancing

Mad Mango,

Thanks.  I believe that this thread illustrates the necessity for having more than just the detail part to make a determination as to the best scheme for dimensioning.
There is an example in the 1988 Standard which I believe supports that.   

RE: Symmetrical Tolerancing

Agree one can't be definite without having all the information.  I thought I'd made this pretty clear by stating that I'd made assumptions.

That said, I really don't see what the problem is using positional for the hole.  It seems appropriate.  The value of the tolerances/hole size need to be carefully considered but fundamentally using a position control would seem reasonable.

This is what I was trying to show the OP.  The main point was finding a way to center the hole wrt the width.  I believe the scheme I proposed does this.

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

RE: Symmetrical Tolerancing

(OP)
Kenat,

  That was the original intent of the post and I will implement that scheme.

MadMango,
   The second block has .060" separation. I've checked the welding fixture and as I expected the fixture does it's job best when the hole positioned as close to the center as possible.  

Once again, thank you all for your admonition.

Tom

Failure is a prerequisite of successful design

RE: Symmetrical Tolerancing

TomFin,

Can you provide a sketch showing the weldment configuration for this part?  That would go a long ways in the solution.

RE: Symmetrical Tolerancing

TomFin

If the fixture used the holes for locating the part, that should take care of the alignment problem.  Is that not a possibility?

RE: Symmetrical Tolerancing

TomFin sorry this all seemed to get out of proporation.  I think you and I are on the same wavelength and I hope it helped.  My last few posts aren't directed at anything you've said/asked.

Quote:

ASME Y14.5M-1994

2.1.1.1 Positional Tolerance Method.  Preferably, tolerances on dimensions that locate features of size are specified by the positional tolerance method described in Section 5.  In certain cases, such as locating irregular-shaped feature, the profile Tolerancing method described in section 6 may be used.

I believe this justifies using positional on the hole.  I've previously explained why I suggested diametric tol zone.

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

RE: Symmetrical Tolerancing

(OP)
Ringman,

   The fixture uses either the left side or the right side of the hinge block, depending on which of the 6 locations it is welded to. The fixture does not use the hinge pin holes for fixing the hinge block into position.
   It uses: 1. The bottom Face, 2. The LH or RH face, and 3. The Front Face. The fixture does have a feature to align the block via the hinge pin hole as secondary alignment assurance.
   I agree that if the hinge pin hole was used as a primary alignment feature this increase overall ease of assembly alignment. The only issue I see if the pin hole is used as primary alignment is that off center pin holes, or thickness variance will cause gaps between the mating surfaces of the hinge block and the tube it is welded to. Waning the gap at the fixture would only delay alignment issues at assembly.
  I think the root cause solution would be to control the symmetry of the pin hole as well as the width of the block and employ the pin hole as a primary alignment feature at welding.
   

Failure is a prerequisite of successful design

RE: Symmetrical Tolerancing

TomFin,

What is the function of the hidden lines in your original sketch.  Are they somehow associated with the alignment.

RE: Symmetrical Tolerancing

(OP)
Ringman,
  That was just a pependicular hole for a spring pin to keep the hinge pin from sliding out the back end. So, no it is not associated with the alignment.

Tom

Failure is a prerequisite of successful design

RE: Symmetrical Tolerancing

If having the hole in the center is ultra critical, I would either use ground bar stock.  That way you can dimension it either way.  If it is only semi-critical, you could specify a tolerance range on the bar stock width.  If this is a weldment I hope you specify accurate secure fixturing for making the welds otherwise the distortion will kill your alignment.  Depending on the rest of the geometry, you might ensure alignment by specifying that a tooling hinge pin be inserted prior to welding.  You will still need to fixture it tightly during the weld, but the tooling pin will guaarantee alignment.

Ed

RE: Symmetrical Tolerancing

PLEASE SEE ATTACHMENT. The .563 is a datum feature of size
meaning the mid plane is datum B of what the actual size of nom .563 feature is machined. Hence .316 dia is located about datum B midplane within postional tol specified. Of note datums A and C include.

ray Doyle

Ray Doyle
SolidWorks 99-07

RE: Symmetrical Tolerancing

I'm not sure that your .281 rad is properly defined.  You don't explicitly define the center point of it.  This was part of why I gave overal length and just 'R'.

Also, I don't believe CL is usually used any more.

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

RE: Symmetrical Tolerancing

I agree with KENAT.  Specifying the actual radius size is unnecessary in this situation.
Using "CL" in that matter is like wearing a belt and suspenders.  The line font defines that it is a centerline.  The only time I specify "CL" is when identifying an axis or other specific feature (i.e. CL DATUM X).
Otherwise, makes sense to me!

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources