Technical drawing: reference dimensions

  • Thread starter FranzS
  • Start date
  • Tags
    Reference
  • #1
FranzS
74
23
TL;DR Summary
How to properly indicate dimensions on a 2D technical drawing?
Hi PF,

as in the company I work in we're updating all 2D technical drawings (production drawings) because of a software change, I'm now having some doubts about how to indicate dimensions correctly. By the way I'm not in charge of that job, I'm just discussing the possible options with the technical office in order to improve the current state of things.

So, until now, we have always indicated redundant dimensions (reference/auxiliary dimensions) without parentheses "( )". Actually, "my" guys from the technical office don't seem to have made up their minds about which really are the main dimensions and which are the reference/auxiliary ones... go figure. No issues in production though, just a bad old habit.
Now I'm suggesting to finally and formally decide which are the main dimensions and to use parentheses "( )" to indicate the redundant/reference/auxiliary dimensions (as in the sample drawing below).

IMG_20250121_204733.jpg


Moreover, my concern is about formally respecting all tolerances. For instance, let's suppose that in the above drawing the dimensions are subject to a general tolerance of ##\pm 0.5## (whatever the units) and that the rightmost dimension "20" is not between parentheses.
In that case, I argued with my colleagues that the drawing is not technically correct because of the redundant dimensions and that the resulting tolerance on dimension "60" won't be clear (actually, you could think the same for each dimension).
They replied that they want to go on with their old method of redundant dimensions without parentheses and that, according to them, their way of indicating dimensions implies that, in this specific example, each single dimension will have to be within the general tolerance.
Now, their explanation actually makes sense to me as there's some kind of logic behind it (and it can indeed be applied to our machined parts without any issue) but I'm a bit skeptical about the conventionality / technical validity of such approach. I also think that their reasoning is equivalent to having a narrower tolerance on the three dimensions 20 / 20 / 20 (hope it makes sense).
Could you please advise me? Thanks guys.
 
Last edited:
Engineering news on Phys.org
  • #2
Machinists should read the drawing and understand exactly what is important about the part without anyone explaining it to them.

In your drawing (with the parenthesis), I understand that the total length is critical, the width of the middle part is critical, and the positioning of the middle part is also critical with respect to the left side.

Without the parenthesis, all widths are equally important, including the total width. Positioning is less critical as nobody cares whether you start from the left or the right side for measurements.

There are many other ways of dimensioning this drawing. You could have a dimension of 40 for the end of the middle step instead of the middle step width, which would emphasize the importance of the location rather than the width of each step.

There are no wrong ways of dimensioning; it is about telling the machinists how the part will be used ... without explicitly telling them. This may help them choose the better tools and processes to do the job.
 
  • Like
  • Informative
Likes Astronuc, russ_watters, gmax137 and 4 others
  • #3
Could the new drawings simply mimic the dimensions shown in the old drawings?

You are correct about the propagation of accumulation of manufacturing errors: you can't expect 60+/-0.5 in the example case.

The normal practice is to provide no dimension where chain errors will naturally accumulate for not being a critical section of the part.

A simple solution to propagation of errors in your example is to use a datum and chain-dimensioning.

overview-of-dimensioning-in-part-design-1593524412.jpg


Dimensional precision is expensive and time-consuming, and should be avoided where unnecessary.

Please, see:
https://www.thefabricator.com/thefa...ances-to-ensure-usable-fabricated-metal-parts

https://www.gdandtbasics.com/asme-y14-5-gdt-standard/

https://www.thefabricator.com/thefa...ensioning-and-its-role-in-drafting-and-design

:cool:
 
  • Like
  • Informative
Likes FranzS, gmax137, phinds and 1 other person
  • #4
Thanks for your replies.
Lnewqban said:
You are correct about the propagation of accumulation of manufacturing errors: you can't expect 60+/-0.5 in the example case.

The normal practice is to provide no dimension where chain errors will naturally accumulate for not being a critical section of the part.
I'm not really saying that the error should accumulate on overall dimension 60. In my (uneducated) opinion, the drawing is simply inconsistent and ultimately wrong, whereas my colleagues again point out that all dimensions (60 included) must be machined within the general tolerance (and that is "explicitly implicit", so to speak).

Let me rephrase the whole thing from a different perspective: if we were to send such a drawing (with redundant dimensions and no parentheses) to an external supplier that would produce the parts for us, what would he do?
  • Would he reject the drawing or ask us for clarifications?
  • Would he produce the parts without asking anything, as he would automatically embrace my colleagues' point of view?
  • Other?
 
Last edited:
  • #5
FranzS said:
Let me rephrase the whole thing from a different perspective: if we were to send such a drawing (with redundant dimensions and no parentheses) to an external supplier that would produce the parts for us, what would he do?
The real question you have to ask yourself is: what is important to you?

With your drawing, the external supplier has to make 3 measurements to verify that the part conforms to the drawing. With the other drawing, it needs to make 4 measurements.

First, each measurement is an additional constraint that can lead to scrapping or correcting a part, i.e., the more there are, the higher may be the cost of manufacturing.

Second, each measurement takes time to make, i.e., the more there are, the higher will be the cost of manufacturing.

It might be trivial for a single piece, but not so if you have to produce a large quantity.

But even if you only make one part, it is always good to develop good habits and understand what message you want to convey with your drawing each time. Then you do it without thinking when you really need it.
 
Last edited:
  • Like
Likes Lnewqban
  • #6
jack action said:
The real question you have to ask yourself is: what is important to you?

With your drawing, the external supplier has to make 3 measurements to verify that the part conforms to the drawing. With the other drawing, it needs to make 4 measurements.

First, each measurement is an additional constraint that can lead to scrapping or correcting a part, i.e., the more there are, the higher may be the cost of manufacturing.

Second, each measurement takes time to make, i.e., the more there are, the higher will be the cost of manufacturing.

It might be trivial for a single piece, but not so if you have to produce a large quantity.

But even if you only make one part, it is always good to develop good habits and understand what message you want to convey with your drawing each time. Then you do it without thinking when you really need it.
Thanks for your answer, but I'm not focusing on how to improve the parts / production / quality control, etc. That's already well established at an operational level.
Mine is merely a question about the drawing formality / consistency on its own.
 
  • #7
FranzS said:
Thanks for your answer, but I'm not focusing on how to improve the parts / production / quality control, etc. That's already well established at an operational level.
Mine is merely a question about the drawing formality / consistency on its own.
The point is that having 4 dimensions instead of 3 has a meaning. One is not better than the other.

The part that complies with the drawing with 4 dimensions will always comply with the drawing with 3 dimensions because it is the same thing with tighter constraints.

That is the same thing as if you change the general tolerance from ##\pm 0.5## to ##\pm 0.1## on the same drawing. Your colleagues would tell you that the drawing with the ##\pm 0.1## tolerance would also respect the one with the ##\pm 0.5## tolerance, so "It's the same thing." But why would you do that if ##\pm 0.5## is enough? Why put that tighter constraint on the machinist? Sure, it is easier for the designer who doesn't have to second-guess if the parts will fit or not. Then again, why not go all the way to ##\pm 0.01##?

On your drawing, if one dimension would have to be set as a reference, I would imagine it would be the total length (60). But what do I know? I don't know what this part is for. Maybe it needs to fit inside another part with a critical tolerance.

So it is not about respecting some convention, it is about what is expected from the part.
 
  • Like
Likes Astronuc, FranzS and Lnewqban
  • #8
FranzS said:
Let me rephrase the whole thing from a different perspective: if we were to send such a drawing (with redundant dimensions and no parentheses) to an external supplier that would produce the parts for us, what would he do?
  • Would he reject the drawing or ask us for clarifications?
  • Would he produce the parts without asking anything, as he would automatically embrace my colleagues' point of view?
  • Other?
Well that's a question to ask the machinists, no? I think the PF (engineer's POV) answers have been on point. If you want to know what the machinists will do, ask them. E.g.,
https://practicalmachinist.com/forum/categories/general.38/

Take your time to carefully formulate your question, they can be a surly and sarcastic crowd over there.
 
  • Like
Likes erobz and FranzS
  • #9
FranzS said:
I'm not really saying that the error should accumulate on overall dimension 60. In my (uneducated) opinion, the drawing is simply inconsistent and ultimately wrong, whereas my colleagues again point out that all dimensions (60 included) must be machined within the general tolerance (and that is "explicitly implicit", so to speak).
But machining natural errors, for excess or defect, must accumulate somewhere.

I believe that your colleagues make a mistake assuming that all dimensions (60 included) can be machined within the general tolerance.

Coincidentally, it is achievable in the example drawing.
It becomes evident that it is impossible if the part has more than three steps.

FranzS said:
Let me rephrase the whole thing from a different perspective: if we were to send such a drawing (with redundant dimensions and no parentheses) to an external supplier that would produce the parts for us, what would he do?
He would try to reproduce this specific drawing because he knows the part is possible to achieve.

He would ask for clarifications in cases that he knows that the designer should have left him some margin for errors in at least one left-over or sacrificial or non-critical dimension, which is not to be considered or measured by quality control.

The last two attached drawings show what would happen if your colleagues design, draft and order a 4-step part for which they specify that all dimensions (total length of 60+/-0.5 included) should be machined within the general tolerance of +/-0.5.
Something must yield.
Machined part 1.jpg

Machined part 2.jpg

Machined part 3.jpg

Machined part 4.jpg

Machined part 5.jpg
 
  • Like
Likes gmax137 and FranzS
  • #10
This is why we spend so much on certain government organizations. Standards are developed so that we can replicate a part to the exact functional dimensions. This eliminates a bunch of chaos. Without going into too much detail on this particular part the standard ANSI Y14.5M standard should apply in the USA, ISO may be different but suspect ISO and USA ANSI and JIS, etc..pretty much comply.


A Reference Dimension is a dimension given to any features that are just for reference – or visualization purposes. These are called out on a drawing using parenthesis (i.e., 5.125). It also could be a dimension that is described on another drawing or elsewhere.
Either way, the dimension does not get inspected.

ARB_20250125_135706.jpg
 
Last edited by a moderator:
  • Like
Likes Astronuc and FranzS
  • #11
FranzS said:
TL;DR Summary: How to properly indicate dimensions on a 2D technical drawing?

Now, their explanation actually makes sense to me as there's some kind of logic behind it (and it can indeed be applied to our machined parts without any issue) but I'm a bit skeptical about the conventionality / technical validity of such approach.
Do all drawings have a reference to ANSI Y14.5? It is my experience from reviewing drawings over that past 35+. years, that engineering drawings (not sketches) have a reference to the ANSI Standard. The dimensions and tolerances are set according to the significance of a dimension that affects 'fit, form or function'. There should be some engineering analysis somewhere that evaluates the appropriateness of a dimension or feature with regard to performance in the intended service and environment. Such an analysis would look at fit-up (interference), stress concentration, temperature (thermal conductivity), vibration, fatigue life (affected by stress concentration), vibration, . . . , and even corrosion.

The American National Standards Institute (ANSI) is a private, non-profit organization that administers and coordinates the U.S. voluntary standards and conformity assessment system. Founded in 1918, the Institute works in close collaboration with stakeholders from industry and government to identify and develop standards- and conformance-based solutions to national and global priorities.
https://www.ansi.org/about/introduction
https://www.ansi.org/about/history

While I am not a member of ANSI, I have used their products. I am a member of ASTM, in which I contribute to selected national (in some cases international) consensus standards.
 
  • Informative
  • Like
Likes Tom.G, Lnewqban and berkeman
  • #12
Astronuc said:
Do all drawings have a reference to ANSI Y14.5? It is my experience from reviewing drawings over that past 35+. years, that engineering drawings (not sketches) have a reference to the ANSI Standard. The dimensions and tolerances are set according to the significance of a dimension that affects 'fit, form or function'. There should be some engineering analysis somewhere that evaluates the appropriateness of a dimension or feature with regard to performance in the intended service and environment. Such an analysis would look at fit-up (interference), stress concentration, temperature (thermal conductivity), vibration, fatigue life (affected by stress concentration), vibration, . . . , and even corrosion.


https://www.ansi.org/about/introduction
https://www.ansi.org/about/history

While I am not a member of ANSI, I have used their products. I am a member of ASTM, in which I contribute to selected national (in some cases international) consensus standards.
Thanks for your answer. As Europeans, we look at EN / ISO standards, but either way we have no reference to any standards in our drawings.
 
  • Like
Likes Astronuc
  • #13
Sometimes the standard references are 'hidden' in a coversheet or internal procedure or internal drawing spec. Not saying that's the case here but it happens.
 
Back
Top