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Repeated Basic dimensions
2

Repeated Basic dimensions

Repeated Basic dimensions

(OP)
If a basic dimension is repeated in separate views of a drawing, does this pose a problem for interpretation in any way or violate the standard?  The dimension of course applying to the same feature in both views.

The drawing of course being prepared 'In compliance with ASME Y14.5M-1994.'  

I looked could find no conclusive statements.

Thanks

RE: Repeated Basic dimensions

Normally it will not be a problem, if the dim is to the same points in every view. I don't like to do this. I dim basic once, then ref the dim in other views if needed. There is usually no question if done this way.

Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 06/08
ctopher's home (updated Jul 02, 2008)

RE: Repeated Basic dimensions

I agree with ctopher. I don't think it's stated not to, but I definitely use only one "true" callout per drawing. Whether basic or not, if repeated, I use a reference dimension in the "inconsequential" view.

V

RE: Repeated Basic dimensions

to all:
ctopher and vc66 have it right. if you repeat the same dimension to the same feature in separate views, the feature is double dimensioned.

say in 6 months, the dimension changes, and a new employee gets to make the change. suppose he doesn't know about the 2nd dimension, and the drawing gets released? which dimension is the correct one?

i HATE using reference dimensions! they can (and have been) dangerous, especially when the 'main' one has changed and the (ref) hasn't.

regards..

teddykaye

RE: Repeated Basic dimensions

(OP)
In my situation, Pro Engineer is used for modelling and the dimensions are associated so that should tend to negate confusion from changes in the future.

I had thought that I had seen 'somewhere' by a GD and T GURU that it was allowable.  Anyone recall such?

RE: Repeated Basic dimensions

That's assuming, of course, that the new employee knows enough about Pro/E to use associated dimensions, and not just create them in the drawing. Believe me, I know from experience.

By somewhere, do you mean on Eng-Tips?

V

RE: Repeated Basic dimensions

(OP)
vc66,

Not necessarily there, don't rem where.

RE: Repeated Basic dimensions

ringman,

   Showing the same dimension in two places is bad practise.  Showing one of the dimensions as a reference dimension would be the prefered way.

   If you are using 3D CAD such as ProE or SolidWorks, both of your dimensions will be updated by any changes.  I prefer to apply FCFs somewhere close to the basic dimension.  If there are two basic dimensions, I can convert one of them to ±, or I can apply an FCF to each one and make them disagree.

   How about it is bad practise, but not has bad as it used to be.  :)

                       JHG

RE: Repeated Basic dimensions

Ringman, out of interest, why are you considering repeating the dimension?

I was in a similar quandry a while back but then thought it thru and made the second dimension reference.

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

RE: Repeated Basic dimensions

(OP)
Kenat

You would have to see the drawing to appreciate or understand the logic.  A radius in indicated in a very small view then additionally in a detail where the holes are positionally toleranced.  It rather seemed to make the definition more clear.  And that should be the object of the drawing in the first place.   

RE: Repeated Basic dimensions

So you're repeating it in the detail view?  I'd lean towards reference dim if any but like you say, I'd have to see the drawing.

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

RE: Repeated Basic dimensions

Interesting discussion.
 I value the opinions of those above, but I find it hard to share their opinion.

I have assumed the position,(because some GD&T guy once taught it to me) that since a basic dimension carries no tolerance, if it is repeated as basic (say in another view on another sheet for clarity) that this NOT the same as a repeated "hard" dimensional callout, i.e. double dimensioning.
The primary reason being that one cannot get the tolerance there, but must go to the FCF for the tolerance.

 There is validity however to the thought that the basic dimension could be revised in one place, and missed in the other.
Still it bothers me (and I'm not sure why) that a Basic dimension would be shown in parentheses somewhere else on the document. Perhaps because I would go looking for a toleranced hard callout somewhere else.

I have seen drawings in the past where an attempt was made to avoid this confusion by placing parentheses around the basic box of the dimension. This REALLY bothers me.

Is this an old checker set in his ways, who should get over it, or do I have a valid argument?

Does anyone care to opine on this one?
 

RE: Repeated Basic dimensions

I was taught in GD&T class that adding parentheses to a basic dim was OK. It indicates the dim is basic, but is referenced somewhere else on the dwg.

Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 06/08
ctopher's home (updated Jul 02, 2008)

RE: Repeated Basic dimensions

checkerron..
no parentheses should ever be put around a basic dimension box to make it (ref.) just put the value itself in parentheses.

ringman..
if the dimension is important enough, to avoid any question, why not show it in the detail view only? that way, it's both clear AND concise. (and you don't end up with a (ref) dimension.)

ctopher..
"a reference dimension is usually shown without a tolerance" is what i learned in gd&t class. a basic dim's tolerance is found in the fcf.

teddykaye

RE: Repeated Basic dimensions

CheckerRon,

   In 3D CAD like SolidWorks or ProE, the two basic dimensions are looking at the same feature of a 3D model. If the model changes, both dimensions update.

   Okay, so far, as long as your are on 3D parametric CAD.

   On the one view with the basic dimension, I apply an FCF showing a profile tolerance of 0.4mm.  I do not apply an FCF on the other view.

   Six months later, someone updates the drawing, changing the other basic dimension into a bilateral tolerance of +0.1/0mm.  The nominal values, controlled by the model, are still the same, but the tolerances are different.

   In a strict, technical sense, the reviser should have searched the drawing to find out how the feature was controlled, but not everyone is this careful.  Maybe they were trying to fix the apparent lack of an FCF!

   A reference dimension shows the dimension, and indicates that the feature is controlled elsewhere on the drawing.

                             JHG

RE: Repeated Basic dimensions

tk369,
If a dimension shows parenthesis, it is reference. It does not mean there is not a tolerance associated with it. It simply means the dimension is stated somewhere else on the drawing that does have a tolerance associated with it.
If I saw a dwg that had a lone dim on it with (), it would mean nothing to me.
If a basic dim had parenthesis around it, I would think the same...I would look for that dim somewhere on the dwg and for its associated tolerances.

Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 06/08
ctopher's home (updated Jul 02, 2008)

RE: Repeated Basic dimensions

"a reference dimension is usually shown without a tolerance" is what i learned in gd&t class. a basic dim's tolerance is found in the fcf.

A reference dimension is always shown without tolerances. A basic dimension is exact, and has no tolerance, as it defines perfect geometry.  Tolerances are for features (either size or location), features are located from datums by basic dimensions.

My cad software lets me create reference basic dimensions, but I don't trust it to be right, and have only been forced to use such a critter once (and cringed even so)...but nobody has questioned it, and that particular drawing has gone overseas and back.  Have not seen the subject of referenced basic dim's. discussed by the spec, nor by any authoritative guru (i.e. somebody not posting in this forum).  

I will point out, again, that repeating a basic dimension may be over-dimensioning, but since basic dimensions ARE EXACT, there will be no difference between parts made with multiple basic dimensions, or parts made with a single basic dimension, locating the same feature (provided there isn't a conflict in the value of the dimensions).  To be certain that people know what you mean, perhaps adding "REF." adjacent to the basic dim. block, instead of the parentheses, would make it clearer.  You could even say "REF., see Sheet 1" or similar.

RE: Repeated Basic dimensions

Repeating the same dimension in two different views is not double dimensioning as I understand it.  Double dimensioning results in being able to locate a feature using more than one series of dimensions, resulting in more (different) dimensions than required to define the part and differing tolerance accumulations locating the feature.  This introduces ambiguity.  The situation presented by the OP is different, as it is not ambiguous but a question of repeating a dimension already present.
Again (please don't turn into the angle thread), this is open to interpretation of the standards fundamental rules.
Para (how do we make that symbol?) 1.4(c) "Each necessary dimension of an end product shall be shown.  No more dimensions than those necessary for complete definition shall be given."
Based on that, I think the dimension in question should be reference, regardless of its being basic or +/-.  the repeated dimension IS NOT required to define the part.  As long as only the dimensions required are present, there is no ambiguity, and the fabricator knows that each of those dimensions are required.  Repeating a dimension introduces ambiguity, as he must now determine if that dimension has been accounted for already or if it is only present in this location.  Simple to do, but unnecessary, and adds to the drawings complexity.
As to wether a basic dimension can be reference, I don't think it really matters as long as the dimension is clearly reference.   

Believe it if you need it or leave it if you dare. - Robert Hunter
 

RE: Repeated Basic dimensions

ewh,
I agree.

Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 06/08
ctopher's home (updated Jul 02, 2008)

RE: Repeated Basic dimensions

I'm glad that others believe parentheses around a basic box is an ugly kludge.

I don't feel a whole lot better about putting the word "REF" next to a basic dimension box. That's a kludge too.
 I do prefer putting "REF, SH1,Z3G" next to a repeated basic dimension rather than turning the basic dimension into parenthetical dimension alone.

Thanks, btrueblood for that thought.

We too use Pro/E Wildfire, and expect it to automatically change any repeated basic dimensions (as long as they are associative), but the point is well taken that Murphy's law will prevail, and someone will mess it up.

 As a checker, I should know that better than most.
 

RE: Repeated Basic dimensions

Paranthesis round a basic, yeah that doesn,t even sound good let alone look it.  If it's a reference dim what does it matter that it's reference of a basic dimm or a +-.

ewh, that's pretty much my thinking.  I just couldn't be bothered to type a bunch out given how that other thread went.

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

RE: Repeated Basic dimensions

Had me worried, too.  This seems to be a much calmer thread though, so far...

Believe it if you need it or leave it if you dare. - Robert Hunter
 

RE: Repeated Basic dimensions

I'll think of something...I can't have you guys being too calm.

Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 06/08
ctopher's home (updated Jul 02, 2008)

RE: Repeated Basic dimensions

I would keep the box off of the "reference" dimension, and just add parentheses around it. It's debatable, but I feel like a reference basic dimension is somewhat of an oxymoron.

V

RE: Repeated Basic dimensions

If we are going into personal preferences, I have to agree with leaving the box off.  It does seem like a kinda ugly kluge having a basic dimension being reference.

Believe it if you need it or leave it if you dare. - Robert Hunter
 

RE: Repeated Basic dimensions

Ergh, dunno, ewh.  If you are referencing a basic dimension, leave it basic, otherwise somebody is gonna get confused-er?  My approach is to always try and annotate my kludges, like I said.

...

When the ASME committee gets around to this one, I hope they tell us whether the () go inside or outside the box.  Or maybe we'll have a box with bulging ends?

...

Now, if you reference a basic dimension, and there are now two basic dimensions for the same feature on the same drawing, should you state "2X" on the original basic dimension, to indicate that you've referenced it, and how many times you did so?

RE: Repeated Basic dimensions

That's sadistic, btruebloodbugeyed

Believe it if you need it or leave it if you dare. - Robert Hunter
 

RE: Repeated Basic dimensions

2X has nothing to do how many times the dimension is referenced on a dwg. But, most people these days building the assembly wouldn't notice the difference anyway.

Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 06/08
ctopher's home (updated Jul 02, 2008)

RE: Repeated Basic dimensions

btrueblood,

   A box around a dimension is part of the tolerance specification as per ASME Y14.5M-1994.  If the dimension is for reference, probably, it should not show any tolerances, therefore there should be no box.

   A revision could involve removing the box.  Don't force a drafter to search the drawing for reference dimensions with basic dimension boxes.

                       JHG

RE: Repeated Basic dimensions

(OP)
I am not convinced at this time that repeating Basic dimensions on a PRO-E generated drawing would result in any sort of problem, nor strictly violate Y14.5M.

However at this time the problem is, at least temporarily, resolved.  I would like to thank all who have contributed opinions.  

I was rather hoping that a GURU, past or present committee person, might respond, but so it goes.

Thanks again
Ringman

RE: Repeated Basic dimensions

Unfortunately, if it is not spelled out in a standard somewhere, questions like these boil down to opinion.  Even the gurus can have differing opinions.

Believe it if you need it or leave it if you dare. - Robert Hunter
 

RE: Repeated Basic dimensions

While I've never seen it used, making a basic dimension ref. by placing parens around it in an auxiliary view seems perfectly sensible to me.

However, having said that, I don't see the need to make any dimension in an auxiliary view a reference just because the same dimension is shown elsewhere.

It is not double-dimensioning because it does not introduce ambiguity.  It is the same information, presumably the aux view is needed to clearly show something that may be too cluttered etc. on the main view.

It does not violate "Each necessary dimension of an end product shall be shown.  No more dimensions than those necessary for complete definition shall be given."  You are not providing more dimensions than necessary, you are making it easier to view the some of the necessary ones.

As noted above, it may cause problems if it is changed in one place, and not the other, but if everything is fully parametric/associated that can't (shouldn't) happen.

So while it may be a drawing/configuration control problem, I don't see it as a violation of drafting standards.

RE: Repeated Basic dimensions

Depends again on interpretation.  Using that logic, you can have two or more of the same dimension on a drawing, regardless of tolerancing method.  After all, they're the "same dimension".
Two of the same dimension is one more than required to completely define the part.

Believe it if you need it or leave it if you dare. - Robert Hunter
 

RE: Repeated Basic dimensions

(OP)
Yes BUT,.... the tolerance is not associative is it?  I am not a Pro E expert.

The tolerancing could result in a problem with double dimensioning.

RE: Repeated Basic dimensions

Neither am I.  I meant that it makes no difference if it is a basic dimension or a +/- dimension that is duplicated.  The tolerancing would remain the same, just repeated.  This is beside the point I was trying to make, which is that any duplicate dimensions are not required to define the part, and therefore should be reference.

Believe it if you need it or leave it if you dare. - Robert Hunter
 

RE: Repeated Basic dimensions

ewh,

I think we are debating a subtle point of semantics - which is something I love to do...

In my view "double dimensioning" is the locating of a feature from two independent data.  This introduces ambiguity, and must not be done.

"Duplicate" or "repeated" dimensioning is showing the exact same thing in two or more places.  There is no ambiguity introduced.

If a feature is shown on both a main an auxiliary view nobody gets excited about "OMG, that feature is shown twice, whatever shall I do?"  Rather it's "Oh, that was nice of the drafter, he has given me this auxiliary view at an expanded scale so that I can see what is going on here without a microscope".

Why should dimensions be any different?

 

RE: Repeated Basic dimensions

MintJulep,
We are in total agreement regarding double dimensioning.  As for repeating, I think that it would be even more helpful if the repeated dimension were reference, thus the reader would know that the feature is located elsewhere, and this is just a "reminder".
As for semantics... it can get very frustrating sometimes, but I think it is good mental exercise, and I tend to learn from such debates.

Believe it if you need it or leave it if you dare. - Robert Hunter
 

RE: Repeated Basic dimensions

ringman,

   I do not know about ProE either.  In SolidWorks, the tolerances can be associative, depending on how you constructed the model and applied the dimension.  Whether it stays that way or not depends on who revises the drawing, and whether or not they checked the model out as well.

   How much confidence do you have in all your co-workers?

                         JHG

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