×
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

unilateral tolerancing
5

unilateral tolerancing

unilateral tolerancing

(OP)
Friends,

In a meeting today one of our manufacturing engineers stated he was going to call another meeting to state "we should never use unilateral tolerancing".  As a design engineer, I am against forbidding use of unilateral tolerances as I feel it is removing a communication tool for use on our drawings.  He claims we should always model the parts so that the nominal dimension can utilize a bilateral tolerance.  He is saying this because they are using the CAD models to generate CNC programs, and then they have to go back the CNC programs and edit the numbers so that they are in the middle of the allowable tolerance.  I hope that makes sense.

What are your thoughts?

Thanks in advance for your input,

-Mike

RE: unilateral tolerancing

mmolt,

   I systematically model my stuff to nominal size, and I apply tolerances.  Sometimes, these come out +/+ or -/-.  I want to build the model, then think about tolerances.  I want to edit tolerances at the drawing level.  Almost all of our stuff either is machining or sheet metal.
 I like knowing my modeled size, as well as my required dimensions.

   Recently, I sent out for the first time for a rapid prototyped part.  The process as FDM.  As far as I can tell, the fabricator did not look at my drawings.  He used the model.  Some of my dimensions did not work.

   We have a conflict here.  Convenient design and modeling, versus convenient manufacturing setup.  I do not see an issue with the actual manufacturing process, since the model is used to create tooling, or for CNC programming.

   I lean towards modeling to nominal size.  Wiggling model dimensions every time I change a tolerance, sounds like a strategy for making mistakes.  Also, I want the fabricator to look at the tolerances on my drawing and think about what they are doing.

   Our machine shops want us to send them DXF files, and your sheet metal shops want the original SolidWorks drawings and models.  Everything seems to work for me, including profile tolerances with specified boundaries.

   Next time I try rapid prototyping or casting, I will probably model to nominal size.  I do not have a good working relationship to these people yet.

                               JHG

RE: unilateral tolerancing

Normally modelling to nominal (as in mid range of tolerance) size is good practice, however, I'd say there are perhaps exceptions.

Drill sizes for holes is one that comes to mind.  Typically drill tolerances are +.004 -.001 or similar.  Should you model/dimension to the nominal drill size or to the mid range of the actual drill tolerance?   Or should you just forget about modelling/dimensioning to suit standard drills?

Another one is where you have min depths of holes, especially threaded ones and/or ones with danger or breaking through.  Not being able to say "... .250 MIN DO NOT BREAK THROUGH" but instead having to assign a tolerance that prevents breaking through whle not requiring bottom tapping or having to specify if a V drill can be used etc. would add time to design.

Finally MAX on internal raddi is useful, it leaves if up to the machinist (or whoever) to pick the tool size that works best for them.

I have more to say but gotta go now!

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

RE: unilateral tolerancing

From my experience, all models are at 'nominal'. Usually the machine operator will make adjustments within the CAM to meet certain tolerances. For Rapid Prototyping, I would create a configuration specifically for prototyping with adjustments meeting tolerances.
To have 'one' model for everything can create havoc.

Chris
SolidWorks/PDMWorks 08 2.0
AutoCAD 06/08
ctopher's home (updated 10-07-07)

RE: unilateral tolerancing

As usual it takes me a while to write a response so I don’t see others responses when I am ready to post. It is not productive for me to edit the response to the original question because others may be posting during the edit. Sorry if I am reiterating earlier posts!
Paul

I would “as a rule of thumb” model all features at nominal dimensions…not because I think that there are not functional reasons to model features other than nominal (unequal bilateral or unilateral) but because unless the design intent is accurately communicated for the life of the product, people will supplant the intent with their own logic and do what they think makes sense.

Let me give a for instance. I was tolerancing a transmission casting control body with fastener clearance holes that were to remain cored to size and valve cores to be machined with minimum material removal. The advantages of the tolerancing intent was that the fastener clearance holes would not require machining and the valve bores, when machined,  would be less vulnerable to surface porosity. The datum registry was designed so that the primary would locate and orient relative to the major valve core slides and the secondary and tertiary registries (intersecting in the center of the structure to minimize shrink variation) relative to core side of the clearance holes. Suffice it to say there were logical reasons for specifying all the fastener clearance hole cores unequal bilateral 1/3 from LMC to suggest core pin sizes to the casting source since all of their position tolerances minimum at MMC and the valve cores 1/3 from LMC to mitigate the risk of porosity since their position tolerances were liberal, well oriented to the primary, but RFS.

It seemed logical to me, however I ran into smack dab into CAD policy that prohibited specifying things with sizes other than with limit dimensioning. I tried to reason with the authority but failed to convince them of my logic. In the end I realized that unless my intent was communicated consistently and accurately others would likely summarily dismiss the design intentions as misguided and convert the targets equivalently to nominal values.

Let me also say that casting suppliers cannot use a nominal model to cut their tooling they have to account for contour shrink so they will grow the model or remodel to account for their predicted shrink.

Paul   

RE: unilateral tolerancing

2
Please convey my thoughts to the manufacturing engineer who is being short sighted and only concerned with his tasks and not seeing the whole picture.  As you have already stated you are a design eng., so I would say I'm preaching to the choir here but if it gives you ammo for the meeting, here goes.

Whenever you design, you model to the "perfect" size for function, always. Because the only thing that is "perfect" is your CAD model, this is why all features should be at ideal size, location, orientation and form.  Most of course, set out to design to standard sizes that match common shaped material or even standard drill bits.  However, more often than not it just doesn't work out that way.

From the nominal you must now specify what the total allowable deviation is from what those "perfect" nominal are and still allow the product to function in all capacities as intended.  
How does one determine these allowable deviations?  Hint: Tolerance analysis/synthesis

You then create the specification or drawings and sometimes this does not always mean equal bilateral tolerances.  Because as Kenat pointed out for the drilling process empirical data has shown that a drilled hole will more than likely be bigger rather than smaller. That is why most designers know to use the unequal bilateral tolerances on a standard drilled hole feature.

To further clarify this phenomenon.  In the process of performing tolerance analysis there is the introduction of the perceived or actual manufacturing process(s), this introduces noise to the "perfect" design or VARIATION.  

Variation is a product of the mfg process, while tolerence is a product of the features function.  They are not one and the same.  It is always in ones best interest to insure that you know the difference.  That the two are mated accordingly with the functional tolerance range always bigger than the capability of the selected process.  Be sure to consider non-normal distributions (if applicable)and the inevitable mean shift while setting this allowable range.  

Here in lies the problem to what your manufacturing engineer proposes.  Because of the nature of the induced variation it is sometimes unavoidable to make every tolerance equal bilateral.  Knowing that a process has mean shifts and non-normal characteristics, we must adjust or shift our allowable tolerance range around the "perfect" design nominal.

The comments I have just made are basic in nature and do not capture this topic entirely.  There are always exceptions and other scenarios to consider but I hope you and the others get the point.

Some more food for thought to ask this mfg eng is to ask a tool and die/mold maker if they always shoot for nominal.  I would bet 9 out of 10 will tell you they shoot for "steel safe", because as everybody knows, it's easier to take away material than to add.  

Or even better ask if his CNC machining process(s) are all capable of producing a normal symmetrical distribution with no shift!

RE: unilateral tolerancing

Most of the major automotive manufacturers supply models with unilateral tolerances on them. This does show good design intent IMO, however it is also a pain for manufacturing, especially on complex surfaces rather than just a boxed up fabrication. In an ironic way there are pluses and minuses for both ways.

This has been debated on here before with regard to hole sizes, if you have a press fit hole for example do you model it at say 30mm and call it out as a H7 or do you model it at 29.996 (the exact figures may be wrong, just using an example)?

Rapid prototyping only adds to the problem as in files like .stl they are pretty much uneditable, where as the CAD system I use needs you to model to the nominal size to add a H7 limit.

As far as I am aware there is no industry standard and I don’t see this problem going away any time soon I am sure this subject will run on.

RE: unilateral tolerancing

(OP)
Guys,

Your comments have been very helpful, and will definitely help me convey my thoughts IF he ever calls that meeting.  These manufacturing guys always seem to want us to change everything to make their life easier.  I don't mind being flexible in my design work, but damn, there's is a limit.  I told him if he said "we can no longer use unilateral tolerances", it would be like taking away a tool, a hammer for instance.  Pissed him off royally.  For whatever reason, he is taking this very personal, and started dropping arguements like, "well, when I worked at Texas Instruments we had this same problem and they changed to not use unilateral tolerances..."blah blah blah.  Who gives a hoot about TI.

Keep the suggestions coming.

-Mike

RE: unilateral tolerancing

You can have your cake and eat it too.  Model with unilateral tolerances if you like but then go into edit/setup/dimbound and change the dimension form the default "Nominal" to "Middle".  Now your 10+0/-1 dimension will regen to measure 9.5 right where the machinist & rapid prototyper needs it.

RE: unilateral tolerancing

Everybody,

   Let's be clear, or at least, agreed on our terminology.

   Take the case that I have a 1.25" shaft that has an Rc7 fit in a 1.25" hole.

   From the Machinery's Handbook...

Hole 1.250+.0025/-0
Max=1.2525
Median=1.2513
Min=1.250
Nominal=1.250

Shaft 1.250-.003/-.0046
Max=1.247
Median=1.2462
Min=1.2454   
Nominal=1.250"

   I would like to model to the nominal dimension, as shown above.

                         JHG

RE: unilateral tolerancing

Sounds like some people need refresher courses on math and print reading.  Just lazy, nothing else.

RE: unilateral tolerancing

At my present assignment we live with this nominal concept every day. The company standards do not allow unilateral dimensioning for manufacturing and nominal CAD dimensioning reasons.
 It applies to drilled holes too. We use ±.010 on all holes with MMC and let bonus tolerances apply.
 This means we in engineering convert all unilateral dimensions that show up on parts and spec sheets.
 
KENAT, it doesn't apply to thread depths however. Nothing wrong with XX MIN FULL THREAD. MIN or MAX dimensions are also permitted as the design requires.

RE: unilateral tolerancing

P.S. We are not permitted to use limit dimensioning either for the same reasons. On holes, often the ±.010 hole tolerances cry out for projected tolerances, which engineers here don't like to use. As a checker, I am adding circle P's to FCF,s a lot, and converting unilateral and limit dimensions that designers try to use anyway.

RE: unilateral tolerancing

Quote (mmolt):

In a meeting today one of our manufacturing engineers stated he was going to call another meeting to state "we should never use unilateral tolerancing".

Ummm, he does realize that normal drill tolerances and all limits and fits tolerances are either unequal bilateral or unilateral, correct?

That's just laziness at its ugliest.

V

RE: unilateral tolerancing

I don't work at TI, but a rocket company with NASA contracts, and the unilateral ban is a pain on things like
shaft and pin fits, as drawoh mentions. We do use unequal tolerances, however, the nearest good or practical nominal.

RE: unilateral tolerancing

It seems like the rule makers driving the process of design instead of allowing the designers/engineers to do their job.  Just a thought.

As design changes over time, unilateral dims can become unavoidable, particularly with molds parts where tolerances can and will be adjusted based on history.  

Matt Lorono
CAD Engineer/ECN Analyst
Silicon Valley, CA
Lorono's SolidWorks Resources
Co-moderator of Solidworks Yahoo! Group
and Mechnical.Engineering Yahoo! Group

RE: unilateral tolerancing

Quote (xplicator):

Variation is a product of the mfg process, while tolerence is a product of the features function.  They are not one and the same.  It is always in ones best interest to insure that you know the difference.

Amen brother!

I cringe every time some schmuck vendor uses the phrase "...standard manufacturing tolerance..."

It amazes me how many people do not seem to understand the difference between a design tolerance and manufacturing variation.

RE: unilateral tolerancing

"...standard manufacturing tolerance..."

Like .005 and .010.
I see these numbers for 'standard' tolerances everywhere on all types of parts. I have also seen them on parts that if on the low end, the part would disappear!

Chris
SolidWorks/PDMWorks 08 2.0
AutoCAD 06/08
ctopher's home (updated 10-07-07)

RE: unilateral tolerancing

You can't please everyone.  Molders typically start at LMC (steel safe, add plastic).  Machinists do better with MMC.  Go to nominal w/ symmetric tolerance and either of these cases has lost half the working range.

In most cases (especially outsourced parts), the print is the binding legal document to determine if a part was made correctly.  Not the model, not an email from the engineer, not a block of code, not a scrawl in a notebook, but the print!

RTFP!  Everyone, no exceptions.

RE: unilateral tolerancing

To TheTick, I hate to burst your bubble but in my automotive experience "CAD is GOD" as the saying goes.

For example, we receive the CAD (math data) and the GD&T(paper drawing) but the two don't jive. Changes have been made to the math data but often the drawing(s) are far behind. So... in this case the customer says "go by the CAD data".

It appears to me that the fast and furious pace in the auto industry has lead to this state. I'd had always been in your current school of thought until landing in the auto industry.

Just to let you know.  

---SolidWorks 2008 SP3.0---

RE: unilateral tolerancing

Sayings are not the same as standards.  It also has little (nothing?) to do with whether it is appropriate to mandate a single tolerance scheme on a print.

In my automotive experience, nothing got made for a customer until they signed a drawing and a purchase order.  The drawing is what defined the deliverable.  Parts (the real objects shipped in crates on pallets to customers) did not get accepted or rejected based on a CAD model.

In either case, so what.  It's a CAD model with no tolerances.  How are you defining the tolerances?

RE: unilateral tolerancing

The term "Basic size" is used in ISO 286 (metric standard ISO system limits and fits), not "nominal". Symmetrical +/- tolerances are rather exception when using that standard.

RE: unilateral tolerancing

The Tick, I think you are a little behind the times, as BARM states in the automotive industry, or at least body panels and various other pressings the model is the master.

You will get a drawing but it only shows a few basic dimensions, usually holes and slots as well as the clamp areas for inspection and what areas have any specific tolerances other than the general as well as material spec.

They do not attempt in any way to give enough information to manufacture the part, it is purely to the model.

RE: unilateral tolerancing

If you're using the model, with no tolerances, does that mean that the machinist cuts it perfectly, or the part is bad?

Unless you're putting tolerances on the model, it's no good.

Try physically making a perfect part, with no tolerances... see where it gets you.

V

RE: unilateral tolerancing

There is no perfect part, this is why tolerances exist.

Chris
SolidWorks/PDMWorks 08 2.0
AutoCAD 06/08
ctopher's home (updated 10-07-07)

RE: unilateral tolerancing

Apparently I've said something without actually writing it.  An ability I didn't know I had.  This thread, and my posts in it, are about use of tolerances on prints.  I'm not debating the merits of building from CAD models.  Apparently some have lost the ability to read paragraphs along with the ability to read prints.

RE: unilateral tolerancing

I think you will find that anyone who has not taken a vow of silence has the ability of saying something without actually writing it down.

The way parts are toleranced, at least in the automotive industry is exactly as I described it above. However the part is NOT dimensioned, the model is master.

RE: unilateral tolerancing

I guess I still don't understand how one manufactures a part without tolerances...

V

RE: unilateral tolerancing

ajack1

Are the suppliers of the CAD model providing a file with the tolerances embedded into it? I know at least one CAD software can do it because I've seen it but I don't know which one it was. As far as I know the only thing you will be able to get from the CAD model is the nominal dimension without tolerances. Are you saying that the customer only provides drawings with the tolerances that they really care about and they don't really care about the other dimensions?
Whatever the case may be, Fundamental rule 1.4 (a) says that each dimension MUST have a tolerance except for those SPECIFICALLY IDENTIFIED as reference, MIN, MAX, or stock. From the threads, I don't see that the CAD dimensions are specifically identified as anything. Would one be correct in assuming that they are all reference? What if someone assumed all OD's were MAX and all ID's were MIN; or vise-versa? I'm no stranger to the idea of "well it's always worked before so what the problem?" but it only takes one multi-million dollar assumption to change the way everything goes. If a company has been allowing this sort of practice for years then suddenly hundreds or thousands of parts get made that will not work, someone has to pay for it. Who will it be; the company that provided the untoleranced data or the company that agreed to build parts based on untoleranced data? It's a dangerous game, in my opinion.

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

RE: unilateral tolerancing

There are tolerances, usually a general profile and surface tolerance and occasionally hole tolerances, which are normally unilateral but there are not dimensions, they come solely from the model.

As to if they are embedded in the model I do not know but they are readable as prints. We only have a basic version of Catia for reading in data, this is a requirement of most automotive manufacturers.

 This might not comply with any standard and I cannot categorically state that all automotive manufacturers work this way but certainly the likes of Ford, GM, Audi, VW, Honda, Toyota and BMW all do and have done for a good few years.

RE: unilateral tolerancing

Yes, as ajack1 as stated above this has been my experience too.

So what did I do when the math data and the GD&T did not match? I inform the customer and he signs off to it. We still use/need the tolerance from the GD&T but apply it to the size(s) of the CAD model.

In fact, to inspect the part you need the CAD model. The model is used to compare against the actual part produced. Think CMM.

Note, tolerances can come from the original drawings (GD&T) or signed notes and emails.

It this the best method? No but it's our reality in this environment of "Got to have it now!"

Note: There is software out there including SolidWorks in which you can include all your GD&T into a 3D model. The idea of this is to reduce the reliance of 2D drawings. ie: the drawing not up to date with the CAD model.

Hope this helps.


---SolidWorks 2008 SP3.0---

RE: unilateral tolerancing

I also work for supplier to automotive companies.
We are creating the 3D solid models using the mean dimensions (median as drawoh calls it). Only some complex castings (as gearbox cases) are made using the "mathematical data" - the 3D model. The simplified drawing with requirements/tolerances/GD&T for the important features is part of the documentation. Any other parts have fully dimensioned 2D drawings including all tolerances, GD&T etc. The critical part drawings are usually also verified by the OEM's.
We supply the same OEM's as ajack1 mentioned, plus Chrysler.

RE: unilateral tolerancing

As far as using primarily CAD data, as others have posted, it is done.  A few critical dimension on the print along with notes which specify that the CAD data is the MASTER data model and a general profile tolerance note.  When the drawing is signed off, it is the same as signing off on the model.  Unfortunately, in my experience, those that have the authority to approve the drawing don't have the ability to even interogate the model, trusting that it was modeled and checked appropriately.

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

RE: unilateral tolerancing

(OP)
I think we've gotten a bit off topic here.  ...and what I'm reading is that some parts are so complex it doesn't make sense to attempt to create an all encompassing drawing to go with the model.  For instance, one can imagine the complex curves associated with todays automobile exterior sheet metal parts...those are probably nearly impossible to dimension and have the dimensions mean anything to a human.  So, in those cases some assumptions must be made about how good the not so critical features will end up, for other dimensions that are critical, some callouts on a drawing must be made to communicate the allowable deviation from nominal.

Regardless, in my line of work, the drawing IS without a doubt the binding contract with the supplier.  The drawing is what is signed off on and agreed upon...otherwise a supplier could give you almost anything, and you would be responsible for the bill, regardless of whether the part meets the requirements of the design.  The drawing is the DEFINITION of what is required.

Now, back to the unilateral question.  I guess where outlawing unilateral tolerances doesn't make any since is in the case of fits and holes.  In the case of drilling a hole, the standard tolerances are almost always unilateral.
For instance, according to a table in front of me listed as "drilled hole tolerance (under normal shop conditions)" a 1/4" drilled hole should have a +.0063 -.001 unilateral tolerance.  So, if I were to do what the manufacturing engineer wants I would need to model the hole as .25265 and some change instead of exactly .250, so he could have his symmetric tolerance.  To take that further, I don't think there is a standard drill that size, so once again his CNC setup guy would have to make some manual adjustments to his program right?

-Mike

RE: unilateral tolerancing

mmolt: What you are defining i.e. + .0063/-.001 is an unequal, bilateral tolerance, not a unilateral tolerance.
Unilateral is one of the tolerance values is zero.
(ASME Y14.5M-1994 ¶ 2.3.)
 Bilaterals can be equal (±.010) or unequal +.005/-.001, with the primary value being the "target" dimension.
Back to your original arguement (and post)with the manufacturing engineer. Was he insistent on target dimensions with equal ± tolerances, or would he accept a  target value (e.g. drill size) with an unequal tolerance value?
 

RE: unilateral tolerancing

(OP)
Pardon me Ron, you're right, it is indeed bilateral, but nonetheless, the manufacturing engineer still has the same problem with it.  He said he only wants us to use symmetric tolerances, so yes, he is insistant there is a target dim with an equal plus/minus tolerance.

Listen, I don't have a problem TRYING to always use symmetric tolerances, but I'm not going to agree with his demand to never use anything but symmetric tolerances.  Like I mentioned, I feel it would mean throwing away some pretty good communication tools on our drawings.

-Mike

RE: unilateral tolerancing

That pretty much seems to sum it up Mike. It does seem strange to me that you can produce a car body part or an airplane wing in this way but a ¼” drill hole becomes a problem.

The shafts and holes standards go back to the days of pencils and paper I can see no good reason to change them, especially if all that matters is what is “drawn” on a 2D print.

I must say I have never seen a .250 drilled holes dimensioned as .25265 +/- .00365 that just seems to cause confusion for no good reason.

RE: unilateral tolerancing

Carrying a dimension to 5 decimal places means that you have to have inspection equipment capable of measuring to 6.  Is your manufacturing engineer and quality department prepared to do that?

RE: unilateral tolerancing

(OP)
Well, I would never put that many places on the drawing, more or less it was for completeness.  Regardless, .253 +/- .004 is still pretty ugly in my opinion.  I just think our manufacturing engineer is picking the wrong battle, and didn't think it through.  Our meeting is tomorrow, and we'll be debating it in front of management, and ultimately, they'll make their decision.

-Mike

RE: unilateral tolerancing

mmolt,

So basically your manufacturing guy wants all features in the models at mid tolerance range with symmetric bilateral tolerance applied.  This is so that he can plug it straight into his CAD to CAM/CNC convertor program without having to do any manufacturing Engineering.

Does he realize that in many cases this may mean either tightening tolerances and/or requiring more timely inspection (for instance changing a threaded hole from ".25 Min Full Thread Do Not Break Thru to something like .250 +- .005 plus some kind of note or convention to deal with the pilot hole not breaking thru)?

While automation is generally a good thing as it reduces labour/speeds things up etc I have concerns that sometimes it means people put less thought into things and that hence the design, or in this case process, isn't optimized to the same extent.  Maybe the speed with which the CAM program can be made compensates in this case, I don't know, but generally I have concerns.

It's a small step from not wanting to massage the automatically produced from the model CAM/CNC program to match drawing tolerances to completely ignoring the tolerances and just trying to produce the part dead nuts and hope for the best.  This seems to be what a lot of our suppliers do, and we often find parts out of tolerance.

I had more to say when I first read this post but lose track now.

On the slightly off topic but realated issue of Model Based Definition (which implicitly the manufacturing guy is going toward) you need to control your models very carefully, especially if you're going to outsource the manufacturing.  You need to make sure the model being made to doesn't get changed (intentionally or accidentally) between the initial ECO release (or equivalent) and when the CNC program is made from it.

Based on your description of your situation if not already done I suggest making it clear somehow that the models are for reference only and the drawing is the controlling document.

Good luck in your meeting.

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

RE: unilateral tolerancing

ASME Y14.41 does allow the models to be the driving document, if it is implemented.  However, even on ASME Y14.41, tolerances must be clearly stated.  Often, the nominal is not a the center of the tolerance range.  This is particular true of molded parts, which can vary over time, and from tool to tool.  It's my opinion that it's really not a good engineering practice to disallow non-symmetric tolerances.

Matt Lorono
CAD Engineer/ECN Analyst
Silicon Valley, CA
Lorono's SolidWorks Resources
Co-moderator of Solidworks Yahoo! Group
and Mechnical.Engineering Yahoo! Group

RE: unilateral tolerancing

(OP)
To put a cap on this from my perspective, the meeting with management to discuss this issue went well.  In the end everyone agreed we would try to use symmetric tolerances if at all possible and only if the design requirements can be met in doing so.  That said, I was pleased in that it was agreed it is good to have non-symmetric tolerances at times, and that they should not be "outlawed".

-Mike

RE: unilateral tolerancing

(OP)
Thanks Matt! I truly appreciate your and everyone elses comments and help.

-Mike

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