What's new
What's new

Asymmetric tolerancing

The real Leigh

Diamond
Joined
Nov 23, 2005
Location
Maryland
I just ran across a very good example of where asymmetric tolerancing is appropriate.

This is a press-fit threaded standoff:
Standoff.png


Note the tolerance on the mounting hole, into which the standoff is pressed.

The diameter of the hole affects the performance of the part. If the hole is nominal, the part will be retained more securely and have greater resistance to torque.

Increasing the mounting hole diameter by .0015" and specifying the tolerance as ±0.0015" would not achieve the same results.

- Leigh
 
Leigh

I would assume most explicit asymmetric tolerances are warranted at some point ....
But the question still remains that you - the machinist - will adhere to what number?
Would it be likely that the operator will have a .147-.149, .166-.168 and a .213-.215 go/no-go pin at the machine? Right outta the gate your Low Limit is not observed as far as design intent.
Actually, in my shop running these in production would have a .148-.149, .167-.168 and a .214-.215 pair. Whichever falls out of range will be re-checked with the LL or HL gage and the offset adjusted immediately.

OH, and another note. The inspection sheet would show .147-.150, .166-.169 and .213-.216 limits.

So I am quite confidently saying that:

Increasing the mounting hole diameter by .0015" and specifying the tolerance as ±0.0015"

would in fact be identical at the end of the day.
 
A concencious machinist with good measuring equipment would attempt to hit and hit nominal much closer than .003. Thus the asymmetrical tolerance will cause a better end result.

My guess is this will effectively reduce the size of the hole as most machinists impose a +/_ .0005 tolerance on them self.
 
My guess is this will effectively reduce the size of the hole as most machinists impose a +/_ .0005 tolerance on them self.

Yup, that's correct.
You reduce your tolerance limit for the purpose of reducing scrap and rework.
If you put that +/-.0005 in the middle of your tolerance band, you can have low or high part without the need for scrap or rework.
If that band starts at nominal ( in this case LL ), any and all of the below LL parts are in need of rework, or in the opposite case where +0/-.003 is the spec, all your OHL parts are scrap.
Hence, most of us hacks don't put it there.
 
A concencious machinist with good measuring equipment would attempt to hit and hit nominal much closer than .003. Thus the asymmetrical tolerance will cause a better end result.

My guess is this will effectively reduce the size of the hole as most machinists impose a +/_ .0005 tolerance on them self.
if everyone is machining to +/- 0.0005 all the time you are costing your employer or yourself serious dough. You should use the tolerances, on new parts they are there for a reason, and if they need to not be there the dumb engineer needs to tighten them up.

This is coming from an engineer. Tolerances should = dolar signs to anyone, and the smaler they get the more expensive the part should be. If you aren't mindful of this you should be.
 
IMO, the window is the window. How you specify the limits doesn't mean a thing. You get parts that are within the window, you pay for 'em. You get parts outside the window, you don't. Though some people do, it would be foolish to expect your parts to have a statistical distribution centered in the window; that would depend on how the job was approached. It's also foolish to think the machinist will try to keep the parts near one of the limits just because they'll perform better.
 
I would have thought that the pressing operation of the insert into the sheet metal would probably contribute most to any misalignment between the insert and the hole in the plate rather than the small tolerance on the hole. If the press tooling is correctly made then the metal around the hole will be displaced reasonably equally into the insert undercut & serrated form. The insert does need to held square to the plate.
These type of inserts are not meant to provide precision tapped holes when pressed into a plate.They are mostly used to provide tapped holes in thin plate for non-critical bolt/screw applications with relatively large clearance holes in the mounted part.
 
I would have thought that the pressing operation of the insert into the sheet metal would probably contribute most to any misalignment between the insert and the hole in the plate rather than the small tolerance on the hole. If the press tooling is correctly made then the metal around the hole will be displaced reasonably equally into the insert undercut & serrated form. The insert does need to held square to the plate.
These type of inserts are not meant to provide precision tapped holes when pressed into a plate.They are mostly used to provide tapped holes in thin plate for non-critical bolt/screw applications with relatively large clearance holes in the mounted part.

No-where (at least I can find) does the O.P. say anything
about POSITIONAL tolerances. Which, best I read from above, is what
your writing about.

Please clarify.
 
Sometimes I will use asymmetric tolerances about a nominal. For example, a 5/8 inch shaft might be .625 +0/-.002 for example. At a quick glance you know it's a 5/8 shaft, closer look gives you the limits.

As a general rule I prefer to specify limits directly. Above example would be .625/.623.

My last choice would be .624 +/- .001.
 
I've always thought of callouts like +.000 -.005 as unilateral tolerances (tolerance all in one direction). Asymmetrical tolerances would be something like +.005 -.002

No matter what they were called, I always programmed to the middle.
 
I think that the nuance of using asymmetric (OR unilateral) tolerancing is best appreciated when the activity of parts being designed and built is kept within a given organization, building its own product line. Within that group that has a common goal, benefit may be seen as parts are produced that are closer to the "ideal" design characteristics. Once those parts are requested from an outside shop, where the only real operational characteristics are "make the parts to print, get paid for the parts" and deliver to schedule, the tolerancing will be used as required, without a sense of strivng to make the ideal part.
 
No-where (at least I can find) does the O.P. say anything
about POSITIONAL tolerances. Which, best I read from above, is what
your writing about.

Please clarify.
The point I was trying to make that was that in the OP example , it doesn't really matter if the tolerance is symetrical or not as the assembly process is the most important factor in this case.
It used to be common practice to specify asymetric ( unilateral) tolerances with the Maximum Metal Condition (MMC) size specified 1st. Thus a 1" hole would have been specified as Ø 1.000" -0.000 , + 0.003. This gave the machinist an MMC target and if he went under this slightly then the tolerance allowed metal to be removed up to the complete tolerance bandwidth limit . A shaft would have been specified as say Ø 0.998" +0.000, - 003.
This method of tolerancing was supposed to have reduced scrap rates as the machinists concentrated on the MMC limits rather than some point between the tolerance limits.
 
Why would you increase the hole diameter for a symmetrical tolerance? Wouldn't decreasing the nominal by 0.0015" get you what you wanted?
For the purpose of the part originally presented, it's desirable to have the mounting hole as small as possible.

This directly controls the amount of material that's swaged into the base of the standoff when inserted, and thus the strength of the overall mounting structure.

Larger holes will work, but with lower retentive force, and greater possibility of failure when the fastener is torqued.

- Leigh
 
No right answer one way or the other, short of limitations within a company's own standard.

Personally, as someone who checks a lot of designs, I want to see the "fit" reflected in the tolerancing. If it doesn't jive, then it's simply more leg work for me.

The manufacturer is going to aim for the mean to keep Cpk high either way.
 
When dealing with unilateral tolerances, which I saw a fair number of, I would take as the desired size the low limit (for -.000 +.001, for example).
I guess it depends on your atitude-are you making it right, or acceptable.
 
I recently had this discussion with a 30 year CNC machinist, who felt that nominal was actually the mean. :rolleyes5:

Ø1.003 +.0005/ -.0000

Nominal is 1.003

The mean is 1.00325

As a prototype, onesey twosey, toolmaker type, I mostly shoot for the nominal number side of the tolerance. I think the design intent warrants that.
 
You guys are scaring me.

Asymmetric tolerances are most typically used to mimic machining operations- i.e. to allow the shop to use std tools and tooling, while recognizing the real world variation that occurs. Best example is a drilling operation. It's possible that a 1/4" drill could be undersize (or result in an undersized hole due to the temperature of the drill or parent material). So it's wise to offer a minus tolerance. We also know that as drills wear they drill larger holes. So you may see a callout that looks like .250 +.0080/-.003. In this instance, engineering is telling manufacturing to use a 1/4" drill bit, while recognzing the historical range of sizes it produces.

Case 2- Structurally we can often live with more metal, but for weight reasons we'd rather not have it. So we're willing to accept a flange thickness that varies from .09-.15, but what we want is .100. If we program to the center of the range, we just increased the weight of our product. In the hole case, we increased the slop in every joint by shooting for the center of the tolerance band.

Engineers frequently screw up their tolerancing as they have become increasingly divorced from manufacturing. My advice is to ask engineering if you aren't sure. Don't reinterpret engineering. Lacking all other information, please program/tool to nominal.
 








 
Back
Top