unilateral tolerancing 5

[mmolt]

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

 

[drawoh]

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

 

[KENAT]

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...

 

[ctopher]

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)

 

[PaulJackson]

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

 

[Xplicator]

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!

 

[ajack1]

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.

 

[mmolt]

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

 

[dgallup]

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.

 

[drawoh]

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

 

[TheTick]

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

 

[CheckerRon]

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.

 

[CheckerRon]

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.

 

[vc66]

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

 

[CheckerRon]

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.

 

[fcsuper]

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

 

[MintJulep]

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.

 

[ctopher]

"...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)

 

[fcsuper]

Chris,

Yup, especially on small radius callouts.



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

 

[TheTick]

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.