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!

*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

Any Rules on Implied Symmetry?

Any Rules on Implied Symmetry?

Any Rules on Implied Symmetry?


This has been bothering me for a while.

Please see the attached .pdf for reference.

I come across a lot of old drawings at work that use a simple dimensioning style that takes advantage of symmetry. I also see this style used in many catalogs.

I like this style because it gives the views a clean look (also fewer dimensions) and ensures that mating parts will match concentrically (which I sometimes require).

However, I have not seen any mention of this dimensioning style in drafting textbooks or ASME Y14.5M-1994 (I only have the old version). Are there any rules about this? Is it considered good or poor practice?

If it is legal, how much off-center can the feature be (say the two holes in my example)? How do you tolerance this sort of thing?

If it is not legal, how do I dimension parts that I want to be concentric? For example, we order a lot of flame cut plates and they come in oversized most of the time. If I dimension a part from the corner, the bolt pattern will be way off-center. This could result in a sloppy appearance (material hanging off two sides on a mated joint).

I've seen others dimension to centerlines, but that seems to be illegal.

"NOTE: The following shall not be used as a dimension line: a center line,..." - ASME Y14.5M-1994

I am really looking forward to your responses.

This will solve a lot of debates at work!

Thank you.

RE: Any Rules on Implied Symmetry?

As shown, your example is not legal.  You've already noticed the crux of the problem in your question of 'how much off-center can the feature be'.

Take a look at section 2.7.3 of ASME Y14.5M-1994 as to why you can't simplistically do it.

Now, if you are using GD&T, specifically position and profile, then you can dimension in your 'implied symmetry' style - see figure 5-4 and some of the related text.

Essentially if you use say width of a feature as a datum feature, then you can then 'imply' centering of other features on that feature.

Posting guidelines FAQ731-376: Eng-Tips.com Forum Policies http://eng-tips.com/market.cfm? (probably not aimed specifically at you)
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?

RE: Any Rules on Implied Symmetry?


You can however do so if the ISO 2768 Standards are applied. The tolerances "unless otherwise specified" will depend upon what class you specify H,K,L for geometric relationships and f,m,c,v  "fine, medium, coarse, very coarse" for dimensions and these classes have tabular tolerance values according to the value of the dimension. Datum features need not be specified either... but are rather determined for presedence by the longest features.

Much of the rest of the world operates as so.

Not defending, not recommending, just informing.


RE: Any Rules on Implied Symmetry?

Another good question is "What is the center?".  Features could be symmetrical about the center of one key feature but not another.

Another reason why datum symbols never belong on centermarks!

RE: Any Rules on Implied Symmetry?


   Symmetric dimensioning is good practise when combined with datums and GD&T as per ASME Y14.5. If this this is an old drawing with ± tolerance controlled by notes on the tolerance block, your drawing is ambiguous.   


RE: Any Rules on Implied Symmetry?


Thank you for the excellent lead.

I have always (past 5 yrs) worked for companies that design custom equipment (usually one-offs). I'm not sure how we get away with it, but we seem to have very primitive drafting standards. We mostly stick to direct tolerancing (bilateral & limits); with the occasional flatness, parallelism, etc. notes. I get the impression that GDT would make our production manager blow a gasket. I think people get nervous when they see the symbols (I know I do) and assume the part is going to cost a fortune.

In any event, I need to get onboard with this GDT stuff, even if it's only for my own knowledge. Right now, I'm clearly not up to speed because I am not quite following what you are saying.

I see the examples that you are talking about (for others - see attached .pdf). The examples seem to always use holes. I semi-understand basic dimensioning, true positioning, etc. with holes, but what do I do with that centered cutout in my part? It has a rectangular profile.

Also, in Fig. 5-4, what tells me that the 4-hole pattern is centered on the part? That is really confusing me.

It's OK if I don't fully understand right now (the general idea will do); I plan to save this conversation and revisit the details later; after I hit the books on GDT.


Thank you for the info. Now I really feel overwhelmed! I will put this on file for further investigation.

TheTick & drawoh

Good points.

Thank you all!

RE: Any Rules on Implied Symmetry?

Last attachment (Fig. 5-3) isn't working for me.

RE: Any Rules on Implied Symmetry?


  I don't think your example is correct. You seem to show a flatness spec on a feature of size but I don't think you can do that with 94. I know you can with 09 in the same way you apply straightness to a FOS. Was your example actually to illustrate what you can do with ISO?

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

RE: Any Rules on Implied Symmetry?


Was your example actually to illustrate what you can do with ISO?

No powerhound, I wasn't illustrating the ISO 2768... all you need for that is the the necessary views, nominal sizes, and tolerance class declaration.

I did make a mistake though (I always see them just after I press submit post), the four fastener hole sizes should have been 8 +/- 0.3.

You are correct... if this was drafted in accordance with ASME 94 the flatness note would be incorrect. I was perfectly comfortable controlling the median plane of a feature like this with a feature size straightness (RFS) callout... then the 2009 standard excluded the 94's extension of the control to median planes ( but rather expanded the control of flatness to include median planes ( so I guess from now on according to ASME... form controls applied to "noncylindrical features of size" is the responsibility of flatness.

The only reason I offered the alternative was show how different functional datum features can alter the implied details. How about this one - the bolt clearance holes establish the coordinate X0,Y0 reference and stop rotation.

RE: Any Rules on Implied Symmetry?


Two questions:
1. Your first sketch shows pattern of 4 holes as tertiary datum. Don't you think this is DOF overconstraining?
2. Second one specifies pattern of 4 holes as secondary datum at RMB (using 2009 wording). Wouldn't be better to apply MMB on this pattern, especially that you assume the holes are for clearance? IMO this would help to establish really nice origin for measurement of tolerances that are referenced to A, B DRF.   

RE: Any Rules on Implied Symmetry?


Your first sketch shows pattern of 4 holes as tertiary datum. Don't you think this is DOF overconstraining?

No, not if these holes (as a pattern) are functionally stopping rotation in the assembly. If [B] mates with a pilot diameter in the assembly it can only stop translation not rotation.


Second one specifies pattern of 4 holes as secondary datum at RMB (using 2009 wording). Wouldn't be better to apply MMB on this pattern, especially that you assume the holes are for clearance?

Sometimes yes, sometimes no! It depends on function. I always tell designers that you don't apply "variable feature tolerance allowances or variable DRF mobility allowances to feature controls if the ideal function is diminished or worsened by the increase in permissible deviation.  Critical feature relationships are typically verified for their assembled location, orientation, clearance, or interference of where both constant and variable tolerances for size, form, location, are considered. You don't have to apply the variable allowances to the designs just because the geometric tolerance is applied to a feature of size... or the datum feature is a feature of size.

In the second example (since the clearances holes functionally establish the location and rotation of the spacer/gasket/whatever) I reduced tolerance and clearance of the holes to minimize the ID's translation and outer profiles rotation so that the part maintains maximum perimeter contact with the mating part surfaces and minimum risk of overlap on the mating part's toleranced boundaries. If I had added MMC modifiers to my datum feature pattern I would have had to add it to my stack calculations and possibly reduce my size tolerances to maintain the same predicted critical relationship results.

This whole justification is factitious and conjured to demonstrate the process I use in selecting whether or not to apply variable tolerance or variable datum reference mobility allowances. I will admit that I sometimes recommend their use for reasons other than function:
•    To enable attribute gauging (most label it functional gauging) when it is best the best alternative to poor choices for the gauge strategy.
•    When policies demand that critical characteristics are gauged 100% and there isn't an alternative way to perform 100% non-contact automated inspection.
•    Other reasons that I can't think of just now.

I don't have any problem with attribute gages being used when the modifiers are applied functionally. In that case I would agree that they are functional gages. They are however of no good use for process control... but that is another story.


RE: Any Rules on Implied Symmetry?

curiousmechanical, did you ever get it worked out?

In 5.4 as I understand it, it's centered because firstly it's shown centered, and then the FCF references the datums which are effectively the center planes make it clear what it is centered on.

There are some that argue you need the centering dimensions, it's come up on here before and I'm not sure if anyone changed their opinion even after lots of discussion.


Posting guidelines FAQ731-376: Eng-Tips.com Forum Policies http://eng-tips.com/market.cfm? (probably not aimed specifically at you)
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?

RE: Any Rules on Implied Symmetry?

My colleagues at work would agree with you, Kenat. The profile callout seems more straightforward to me. Maybe position works better for CMM operators. I need to study this more.

RE: Any Rules on Implied Symmetry?


I prefer to use profile when controlling part feature contours that have been functionally designed to have uniform tolerance and enable simultaneous feature contour processing methods i.e. blanking, casting, and molding... no mater whether they may be labeled features of size. When refinement operations are added that can independently control size location, orientation, or form... then I would add an appropriate additional control.


RE: Any Rules on Implied Symmetry?

Hi Guys,

Sorry for the delay! I thought this thread lost its steam.  I'm glad to see that it's back.

Thank you all for the additional feedback.


Unfortunately, I have not had the time to hit the books on GDT, so my understanding is still limited (my time has been completely consumed by Mathcad). Although, thanks to your post, I think I now get the gist of it.

Please see the attached. I would be curious to see the correct way to dimension example: 1 (which uses my current cheap and dirty method). Example: 2 is my poor attempt.

Also, if you have the time, I have two general questions for you experienced GDT guys.


Since graduation I have been in the world of custom machinery (first at a machine shop and now an OEM). So far, I don't see many people use GDT and I suspect the ones who sometimes do don't use it correctly. So my question is, of the engineers who do make drawings, what percentage of them do you think use GDT? I am trying to get a view out of my small world. I am also trying to find out if this is something I NEED to know. I am under the impression that this stuff is for industries with high-volume production (i.e. automobiles, consumer goods, military, etc.). Is that the type of environment that most engineers work in?


At my company the engineers make the drawings. However, I have heard that at larger companies, designers make the drawings. So, who needs to know the details of GDT; engineers, designers, or both?

Thanks guys!

RE: Any Rules on Implied Symmetry?

Without knowing the function of the part, I'd say 'keep it simple'. See the attached drawing.

Hopefully, the next generation entering the workplace won't even know plus/minus. Plus/minus is ambiguous. GD&T is concise. If 'plus/minus' works for you, the short-term gain might be sufficient and a reasonable position to take. But we live in an increasingly complex society and, where it is headed, GD&T is absolutely, unequivocally mandatory  if this high-level of technology is to be sustained.

RE: Any Rules on Implied Symmetry?

It's gonna come back to the functional intent of the design.

If it needs to be 'centered' on the the part, then you really have to use GD&T, I can't think of a robust way to even try and do it with +-.  Even if you dimension to a Centerline, you have to locate that centerline from an edge and you're back to square one.

Your Example 1 is incomplete, you only give the size not the relative location, there is no information on how centered the (assumed) cut out is.  

Your example 2 is not much better, you still haven't set up centering datums.  You've picked the edges as datums, not the 'width' of the part.

You really need more help that it's easy to give in this type of situation.  Without knowing function etc. I'm hesitant to say too much but if I wanted a cutout centered on a physical part, I might do it something like the linked.  I haven't attempted to exactly match your tolerances and assume there's a block tol or similar somewhere.


If it's ok for it to be located from one corner, then Ptruitt's will kind of work, though it's not clear which corner is which on the physical part which can cause problems.  It probably wouldn't be my first choice on how to approach it though.

Q1.  I'm in fairly low volume work but we use GD&T as it allows us to actually capture functional intent while keeping tolerances as loose as possible.  Not everyone is very good at it though, and I doubt some of our vendors really understand it - we've actually used GD&T on parts so we could better capture the function while actually relaxing tolerances and yet they came back with a higher price!  Some shops seem to increase the price based on how many FCF they see - probably because a lot of designers only use GD&T for 'tight tolerances' or 'where it really matters' etc. which is a never ending circle of confusion and lost opportunities.

Q2.  We only have one 'Designer' left and he gets given tasks pretty much the same way as 'Engineers'.  It was similar at my last place.  An Engineer not doing his own drafting doesn't need to be expert in GD&T, however, if applicable he should know enough to be sure the Drafter captured the design intent/requirements properly.

Posting guidelines FAQ731-376: Eng-Tips.com Forum Policies http://eng-tips.com/market.cfm? (probably not aimed specifically at you)
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?

RE: Any Rules on Implied Symmetry?

Thanks for the feedback guys.

Based on your comments, I will keep GDT on my to-do-list. It may not be required at my current company, but it does seem more common than I thought. I have a long career ahead of me and I don't want to become prematurely obsolete.

As for my example, it was just something I whipped up for discussion (no real function). I was just trying to say that what I usually do is example: 1 (I understand this is bad practice). Example: 2 was just my best guess at the proper way.


You are correct; I am not yet capable of having an educated discussion on this matter. However, I will hold onto you example and one day I hope to understand it (just a matter of making the time).

Here is the basic gist of where I am coming from:

Most of the parts we make start from a flame cut plate. The tolerances on the profiles of these plates need to be pretty loose (+/- 1/16"). Most of the time, I don't really care about outside dimensions of the part. However, I want things to bolt up on center. Some of these plates come in pretty oversized (ex. + 1/4"). I have dimensioned parts from a corner and the hole pattern (or cutout) comes out looking clearly off-center. Even worse, when you bolt two pieces together, the edges don't line up and it just looks sloppy (touching on two edges and a gap/overhang on the other two). It seems like when I do the symmetric tolerancing (the cheap and dirty style), the machinist will indicate to the center of the piece and makes that his (0, 0). The parts come out how I wanted, but in the back of my mind, I feel like a looser because I know that my dimensioning practice is bad. When I ask around the office, it seems like most people solve this dilemma by giving a reference dimension to the centerline (which I think looks just as bad). I am happy to find out that GDT is the only correct answer. Now I just need to learn it!

RE: Any Rules on Implied Symmetry?

So, while it's something I tend to avoid because some of the implications can be a bit complex/confusing, if the pattern of holes is your real functional datum,  then it may be that the pattern should be your datum.

ASME Y14.5M-1994 Section 4.5.8 and figure 4-22 goes over this, but for anything more than a 2 hole pattern it can get confusing so I rarely use it, especially when you use the MMC of the pattern in subsequent call outs.

Instead I may choose one of the holes as my secondary datum, and another hole as my tertiary, more like figure 4-8.  It doesn't quite as closely follow true function but may be close enough.

Posting guidelines FAQ731-376: Eng-Tips.com Forum Policies http://eng-tips.com/market.cfm? (probably not aimed specifically at you)
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?

RE: Any Rules on Implied Symmetry?


Thank you for that additional info!

I really appreciate your help.

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! Already a Member? Login


Solutions Brief - Protecting and Rescuing On-Ground Personnel
Keeping our warfighters safe and delivering them a competitive advantage is a key goal of departments of defense around the world. It’s a goal shared by embedded computing manufacturers like Abaco: we never forget who we serve.This case study describes how a major international contractor integrated an Abaco single board computer at the heart of its CAS/CSAR solution. Download Now
Datasheet - Top Enhancements Creo 7.0
PTC's Creo 7.0 has breakthrough innovations in the areas of generative design, real-time simulation, multibody design, additive manufacturing, and more! With Creo 7.0, you will be able to design the most innovative products faster than ever before, keeping you on the cutting edge of product design and ahead of your competition. Download Now

Close Box

Join Eng-Tips® Today!

Join your peers on the Internet's largest technical engineering professional community.
It's easy to join and it's free.

Here's Why Members Love Eng-Tips Forums:

Register now while it's still free!

Already a member? Close this window and log in.

Join Us             Close