Unilateral tolerances-why?

[sendithard]

We just onboarded a new customer. All their prints have unequally disposed surface profiles. And their CAD models are all made at MMC condition. That causes some issues with surface hits on the CMM with tight tolerances. So I'm in the middle of altering their models to what we make the parts at. We are dealing with some goofy .05/.025mm profiles on position and profile, which is basically beyond the capability in my opinion of our CMM. I'm trying to get a Gage RR done at the moment on these ridiculous internal callouts,. Uncertainty is at a minimum of 2 tenths or 5 microns.

GDT is for communication. Can someone explain to me why you would ever desire to basic a print at the MMC with one sided tolerance? What is wrong with the basic at what the part should be made at and a bi-lateral tolerance zone?

The customer just provided a print at Profile .025 U 0 and the tolerance zone is dashes in the direction the part can grow which is opposite the callout. They don't understand the callout nor do our engineers. Run an external profile of .025 U 0 by two random engineers and then run an internal profile of .025 U 0 by them later in the day and see if you get the right answers. No chance. I cannot stand unilateral tolerances, and would enjoy hearing why anyone would use them?

Thanks.

 

[3DDave]

It's a preference, just not your preference.

ASME Y14.5 is for communication, just not to the CMM operator alone. This may make certain calculations for stress and interference easier or trivial. It means the basic profile is exactly equal to one boundary of the tolerance zone.

There are schemes where the nominal value doesn't lie inside the tolerance zone.

There should be no "dashes" used in conjunction with the "U" symbol and, if graphically depicted, it should be a phantom font.

There aren't "internal" and "external" profile tolerances; it's even a bit dicey to call anything an internal feature as every feature is on the outside of the material of the part, but the committee needs to please the crowd rather than explain the sort of rules the computer graphics people use for determining where material is and isn't based on surfaces. The ASME calling them different adds to the confusion you noted.

Perhaps make up a guidebook in advance of accepting new customers that tell them what you will and will not accept on drawings.

 

[mfgenggear]

OP
what type of part, and geometry.
how are the parts machined. or manufactured.
if the parts are quoted with those tolerances
then it has to meet those requirements

 

[mfgenggear]

OP
Also if the CMM does not have the precision required. Then it requires a layout on the granite surface plate.

 

[drawoh]

We just onboarded a new customer. All their prints have unequally disposed surface profiles. And their CAD models are all made at MMC condition. That causes some issues with surface hits on the CMM with tight tolerances. So I'm in the middle of altering their models to what we make the parts at. We are dealing with some goofy .05/.025mm profiles on position and profile, which is basically beyond the capability in my opinion of our CMM. I'm trying to get a Gage RR done at the moment on these ridiculous internal callouts,. Uncertainty is at a minimum of 2 tenths or 5 microns.

Thanks.

Terminology...

	Modelled size	Max	Min
Nominal	⌀40	+0.3	+0.1
Min	⌀40.1	+0.2	0
Median	⌀40.2	+0.1	-0.1
Max	⌀40.1	0	-0.2

I would prefer to do nominal modelling and then apply the tolerances. If people are doing to do 3D printing, or any form of moulding, median modelling is the way to go, as you note. The vendor wants to work off the model.

Chat with your customer. As mechanical designer, I have had these conversations throughout my career, and the desired processes have changed along with the technology. Make it clear to them that a preferred modelling technique will reduce fabrication costs.

 

[3DDave]

(Last edited: Tuesday at 11:22 PM)

We just onboarded a new customer. All their prints have unequally disposed surface profiles. And their CAD models are all made at MMC condition. That causes some issues with surface hits on the CMM with tight tolerances. So I'm in the middle of altering their models to what we make the parts at. We are dealing with some goofy .05/.025mm profiles on position and profile, which is basically beyond the capability in my opinion of our CMM. I'm trying to get a Gage RR done at the moment on these ridiculous internal callouts,. Uncertainty is at a minimum of 2 tenths or 5 microns.

GDT is for communication. Can someone explain to me why you would ever desire to basic a print at the MMC with one sided tolerance? What is wrong with the basic at what the part should be made at and a bi-lateral tolerance zone?

The customer just provided a print at Profile .025 U 0 and the tolerance zone is dashes in the direction the part can grow which is opposite the callout. They don't understand the callout nor do our engineers. Run an external profile of .025 U 0 by two random engineers and then run an internal profile of .025 U 0 by them later in the day and see if you get the right answers. No chance. I cannot stand unilateral tolerances, and would enjoy hearing why anyone would use them?

Thanks.

"their CAD models are all made at MMC condition. That causes some issues with surface hits on the CMM with tight tolerances"

That's a problem between you and your CMM software maker.

"So I'm in the middle of altering their models to what we make the parts at."

They cannot predict problems with your processes.

"We are dealing with some goofy .05/.025mm profiles on position and profile, which is basically beyond the capability in my opinion of our CMM. I'm trying to get a Gage RR done at the moment on these ridiculous internal callouts,. Uncertainty is at a minimum of 2 tenths or 5 microns."

That's another item to put into the handbook for reasons to refuse models and contracts that you give to potential customers before onboarding them.

"why you would ever desire to basic a print at the MMC with one sided tolerance?"

You don't mention any process, so for those that involve removal of material one can program the CNC system to have a very, very small negative offset (into the material) from nominal and thus maximize the chances that any out-of-tolerance conditions can be resolved by removing material by minimizing the risk of accidentally removing too much. If any feature fails then the offset for that feature can be corrected.

Needless to say, I did not see the edited version of the comment. So that means I will entirely quote every single comment you make from now on in my replies. I see that drawoh is already doing that. Consider this the first item that is going into my handbook.

 

[ctopher]

I'm trying to understand why are you inspecting your customer models? Doesn't your customer give you an outline of what they need, then you supply the product? As long as you tolerance the parts to meet their dimensional envelope?

 

[jassco]

Hi, sendithard:

Do your customer prints have a note to indicate you can use its 3D model? If not, then the models mean nothing to you.

Best regards,

Alex

 

[dtimberlake]

"GDT is for communication. Can someone explain to me why you would ever desire to basic a print at the MMC with one sided tolerance? What is wrong with the basic at what the part should be made at and a bi-lateral tolerance zone?"

Can't really speak for "why".
Sometimes I have to dig pretty deep to even be sure of the "what."

But +0/-.0005" is how the OD of Metric ball bearing with bores around 80-120 mm are toleranced in catalogs.
I have no clue what the manufacturing drawings show.

 

[Mech1595]

GDT is for communication. Can someone explain to me why you would ever desire to basic a print at the MMC with one sided tolerance? What is wrong with the basic at what the part should be made at and a bi-lateral tolerance zone?

For functional fixtures/gauges, I'll model critical features at MMC/LMC and specify the limits as needed on the drawing. This simplifies the design process on my end, and is no issue for the fab shop.
These are also for one-off/limited qty components used internally, so I'm not really concerned about a CMM operator setting up a program [edit: for long-term production].

 

[Gr8blu]

When the companies I have worked for use single sided tolerancing, what they really mean is that the "zero" side of the tolerance is the nominal value - and the deviation allowed is zero in that direction. Typical for a series of parts that have to mate with multiple different parts within an assembly. Using the ball bearing example: the ball CANNOT exceed the diameter specified (+0.000) but CAN be a bit undersize (-0.0005). This is because during operation there is thermal growth and if the ball is too large, the design clearance disappears, and the bearing is likely to fail prematurely.

 

[ctopher]

Zero isn't necessarily the nom value. If a dim is for example .150 +.000/-.005, the target value is .150.
The 3D model is .150.
The tolerance range is .145-.150.

 

[Belanger]

Chris, just a small nit-pick... While I agree that the tolerance range is .145 - .150, the target value is not .150 (according to ASME Y14.5). In the standard, paragraph 4.1(q) says "UOS by a drawing/model note or reference to a separate document, the as-designed dimension value does not establish a functional or manufacturing target."

 

[drawoh]

Zero isn't necessarily the nom value. If a dim is for example .150 +.000/-.005, the target value is .150.
The 3D model is .150.
The tolerance range is .145-.150.

By my definition above, zero is the nominal size. For quite a few years now, I order fabricated parts by sending out a PDF of the fabrication drawing and a STEP of the CAD model. There is an understanding that the fabricator will use the STEP file for size reference. This is why your modelling/tolerancing technique must be methodical.

 

[mfgenggear]

Unless otherwise agreed upon. Tolerance is tolerance. If it meets engineering drawing its in spec and acceptable. That is what tolerance is for . For acceptance.

 

[DanStro]

I always ask our purchasers to put a note on the PO to any shops that we send 3d models to that states that the prints are the controlling documents and that is what the final parts will be inspected against. There have been times when the 3d model was the controlling document, normally for 3D printed parts, but our default is the print(s).

This is really the only way I've found to make sure everyone is on the same page as to what to do if there are conflicts between the two. Of course if there are conflicts I'd prefer the shop to just ask but they are usually not too inclined to do that and without some kind of note like this they inevitably pick the wrong one. This also gives the shop a CYA if there is an error on the print that is not on the model.

 

[ghostdigital]

"Can someone explain to me why you would ever desire to basic a print at the MMC with one sided tolerance?"

Old school..

Before CNC's we manufactured stuff with manually operated machines and the strategy for the machine operator (machinist) was to remove just enough material to achieve MMC. The idea was that no more effort should be made as well as the end part would dimensionally move around as the part stress relieved itself on material removal. On in-process inspection there would be material left to be removed should the shifting of geometry occur due to material removal throwing something out of tolerance conformance.

In todays modern manufacturing world machining CNC and other subtractive manufacturing processes require programming and a 3D model at nominal with bilateral tolerances is optimal. Modern manufacturing machinery is not necessarily more accuracy capable then yester year but more consistent which facilitates bilateral tolerances.

Moreover, unilateral tolerances applied to a MMC modeled 3D cad file usually requires extra programming work to offset the cutter compensation to the nominal size to allow a bilateral variation as targeting MMC may require additional manual machining work.

I'll be back to review my post for clarity later...

 

[supergee]

I am trying to reply to the essence of your question, which is WHY people model their parts at MMC. I can't say I completely agree with it, but here are the arguments.

The reason I got from designers that use that approach is simple: to be able to locate interferences. When drawing at nominal value, some feature in the CAD won't be in contact. But in reality, the features could interfere at MMC.

There are interference analysis tools that should help with that, but you can only set a single distance value for the analysis on the software I know. Because of that, the analysis is quite difficult since parts usually have more than 1 tolerance for all features... at least well designed parts do. For simple products, this is not a concern but when dozens or hundreds of parts interact with each other, checking for interferences can be tedious.

The other reason that some have is when parts are design to fit an existing part that was scanned. The scanned surface is the basic shape, and no defects can violate that surface. having unidirectional tolerance zone in this case is the way to go. This is the only situation I am aware of where I would use this.

When you think about it, a lot of features are already drawn at MMC: clearance hole, screws and bolts threads are usually drawn at nominal diameter which happens to be the MMC values. Same goes for keyways and other types of hardware.

My opinion is that I won't use this technique unless I am forced to. This is a relic of the time when drawings were hand drawn. Back in those days, tolerance analysis was: "do the line cross on my drawing". I try to stay clear from solutions that help the draftsperson, because my experience is that those solutions are making someone else's job harder down the line (Example: creating an assembly of a bolt, a nut and two washers to save drawing time, ends up creating countless assemblies in the PDM/PLM software that needs to be managed by IT with no added value)

If Dassault systems, Siemens and Autodesk cared for my opinion, which I doubt, I would make it so we could see parts at MMC, LMC or nominal, with a couple of click.

I hope it is clear. English is not my native tongue.

 

[mfgenggear]

there is a reason there are functional go and no go gages. to make sure it assembles.

 

[Burunduk]

Sometimes unilateral tolerances just "feel" right. The faces of the support bosses in this cover can be fully coplanar with a plane tangent to the weld pad surface or slightly (up to 0.2 mm) below. The requirement is just that they do not protrude above it, from obvious reasons. An alternative could have the bosses designed with a basic offset of 0.1 in the allowed direction, but I guess from some aspects the shown solution might be easier to most of those involved with the part.