Tolerance, Bilateral vs Limit

# Thread: Tolerance, Bilateral vs Limit

1. Plastic
Join Date
Dec 2017
Country
UNITED STATES
State/Province
Wisconsin
Posts
9
Post Thanks / Like
Likes (Given)
0
0

## Tolerance, Bilateral vs Limit

Hey all! I was impressed with the answers to my last question, so I am back.

Another topic discussed is how to dimension a feature on a part, for example a shaft of nominal diameter 5.000". I am using RC4, so the shaft is to be made with -.0016 to -.0032 as a tolerance. I have up to this point used bilateral dimensioning. I realize the machinist has to do the math on the 5.000" number to get the numbers to manufacture too. If I were to use limit, the numbers on the print would read 4.9984"-4.9680". Again, the machinist would have to do math if wants to hit mean. What do you guys prefer?

Now, to throw in an additional argument. When I model this part in solidworks, I dimension the part to the nominal 5.000". I have read some places will actually put the mean dimension in the model, so in this case 4.9976". The print will then either read a symmetric +/-.0008 or do the limit again. The reason they do this is because we now have the CAM software that will import the model. If the model is made to that mean dimension, the programmer will not have to make any changes.

I do not know any CAM software, how it works or how much work these different cases put on the machinist/programmer. So that is essentially my question, what makes it easier on others? I know if someone is measuring it is easier to see limit dimensions as that is the output on the caliper without any math.

2. Cast Iron
Join Date
Mar 2014
Location
Posts
381
Post Thanks / Like
Likes (Given)
42
234
If you expect them to machine it drom the solid model, draw it the size you want it (the mean). If you expect them to make it from a print you can do it any way you like.

You will run into problems (especially on turned parts) if the same tool is machining a feature that has an equally tight tolerance, only in the other direction.

3. The response is usually pretty good when you ask well written and thought out questions.

Most of the folks I've talked to prefer limit dimensions for ease of use, so I try to give them that when I can. If you know it's going to be programmed and run through a CAM system, you can model it as nominal in Solidworks and then adjust the dimensions to read as limits. Best of both worlds, but takes a few more clicks.

4. Always always always always create the model to perfect form. You can call out the tolerances in the drawing however you want (we prefer symmetric bilateral). The point is some CAM guy is going to, at some point, pull the model in and never look at the drawing. Don't laugh, I've seen it happen.

Drawings and models are a form of communication, your goal is to communicate as clearly as humanly possible. Having someone do extra math is just not good practice.

Seeing 5.000 -0.016/-0.032 drives me up a wall. Yes the dim is 5 nominal. Is the part going to be used nominally? No. Then write the damn thing 4.976 +/-0.008 and be done with it.

5. Stainless
Join Date
Feb 2013
Location
Posts
1,055
Post Thanks / Like
Likes (Given)
1144
683
Originally Posted by Rewt
Always always always always create the model to perfect form. You can call out the tolerances in the drawing however you want (we prefer symmetric bilateral). The point is some CAM guy is going to, at some point, pull the model in and never look at the drawing. Don't laugh, I've seen it happen.

Drawings and models are a form of communication, your goal is to communicate as clearly as humanly possible. Having someone do extra math is just not good practice.

Seeing 5.000 -0.016/-0.032 drives me up a wall. Yes the dim is 5 nominal. Is the part going to be used nominally? No. Then write the damn thing 4.976 +/-0.008 and be done with it.
This. It pisses me off when a model isn't to "perfect" form. It makes extra work for the programmer and/or machinist.

Is there a reason not to do it this way?

6. Why wouldn't it be made to true size? That's just asking for a fuck up...

I
realize the machinist has to do the math on the 5.000" number to get the numbers to manufacture too. If I were to use limit, the numbers on the print would read 4.9984"-4.9680"
That's a hell of a tolerance.

7. Diamond
Join Date
Dec 2008
Country
UNITED STATES
State/Province
New York
Posts
10,235
Post Thanks / Like
Likes (Given)
0
2657
i would never ever trust solid model. i always go off of drawing dimensions and tolerances. parts have to fit together. that is if shaft goes in hole it needs to happen. assembly guy not going to care about theoretical discussions.
.
things out of round (warpage), bores that have taper from tool wear, alot of things can cause problems.
.
worse thing in my experience is solid model with small corner radius or chamfers. if not selected correctly often program is .010" off if hard to see corner radius was .010", i would never trust solid model. i have seen too many small CAD problems become big problems making the part and assembling the part.

8. Originally Posted by AARONT
This. It pisses me off when a model isn't to "perfect" form. It makes extra work for the programmer and/or machinist.

Is there a reason not to do it this way?
We have some tooling made in Italy that completely ignores things like dowel fit. They draw it straight up line to line. Both the dowel and the hole to nominal. Clearance for cutting steels the same way.

I have no idea how they finished the dies.

9. Aluminum
Join Date
Jan 2009
Location
Maine, USA
Posts
203
Post Thanks / Like
Likes (Given)
100
92
I agree with three posts above me. 5.000 (-x, -y) is not a proper tolerance. -0, +x or -x, +0 are appropriate for showing either side of nominal on a drawing. Also, ignoring the incorrect math in your first post, you wouldn't write (upper limit-lower limit), it'd be the opposite.

A fit is a fit and a tolerance is a tolerance. In this case you can't combine them in my opinion.

As far as modelling, I do not know, but it would never seem to be a good idea to model the part as something outside the tolerance of the actual part. Again, fit is fit and tolerance is tolerance.

10. Diamond
Join Date
Dec 2008
Country
UNITED STATES
State/Province
New York
Posts
10,235
Post Thanks / Like
Likes (Given)
0
2657
some will dimension a bore as 3.0000 +.0020/-.0000
.
cause bore needs to be big enough to get the mating part to fit into the bore. so everything dimensioned from that point of view or way of thinking
.
same with setting a indicating bore gage. do you set in middle of tolerance (looking for +/-.0010" or do you set 0.0000 at minimum size so bore gage reads +.0001 to +.0020"

11. I don't care really. But it has to be right.

12. Aluminum
Join Date
Dec 2016
Country
UNITED STATES
State/Province
California
Posts
160
Post Thanks / Like
Likes (Given)
26
44
Always model at nominal! I've seen minus/minus tolerances screwed up more times than limit dimensions.

13. Plastic
Join Date
Dec 2017
Country
UNITED STATES
State/Province
Wisconsin
Posts
9
Post Thanks / Like
Likes (Given)
0
0
Thanks for the replies everyone, and I apologize for typing the incorrect number in there.

JCByrd I thought it was always upper limit, -.0016, and then lower limit, -.0032. That was my interpretation.... and never mind, as I type this I am reading ASME Y14 2.2 direct tolerancing and in that form that I have it typed out in, single line, it should be lower limit than high limit. This is what I really meant to have that look like (as looks in drawing with bilateral):
(blank space)-.0016
5.000
(blank space)-.0032

wasn't letting me use spaces!

Thanks again everyone!

14. Cast Iron
Join Date
Dec 2015
Country
UNITED STATES
State/Province
Illinois
Posts
459
Post Thanks / Like
Likes (Given)
166
259
that looks like a very dangerous way to show the tolerance. Of course there are minuses in front of both tolerance limits but I could see very easily miss reading that as 5.000 +.0016/-.0032.

I am defiantly in the model to nominal camp. I have a group that routinely brings turning me models with with a -.002/-.004 tolerance that is next to a chamfer with a angle call out up to a defined dia. Then the next dimension starts at the top of the chamfer meaning that the solid model is nothing like what they will get will get if I follow the dimensions. So every time I call them down to have them explain what dimensions are actually important and I usually end up not being able to use the solid model for anything.

TLDR: Model doesn't match the dimension which makes me angry and wastes time.

15. Nominal isn't a word we should be using really.

(of a role or status) existing in name only.

I understand what it implies in Manufacturing. But if we're going to have a conversation about how to tolerance a part Nominal makes it even more confusing. Example; one person means Nominal as the exact dimension desired, another person means the whole rounded value. (5, in this case).

IMO, none of it matters. The person looking at the Print needs to read it and understand it. If they fuck up, okay. If the Spendgineer fucks up, that's on them.

R

16. Stainless
Join Date
May 2017
Country
UNITED STATES
State/Province
Minnesota
Posts
1,154
Post Thanks / Like
Likes (Given)
1454
803
I've seen far too many cases where single sided tolerances end up defining impossible geometry, especially when the "nominal" size is outside the tolerance range. Model it at the median and call it 4.9976" +/- .0008", since that's what you really want. The programmer will program to the median, the operator will adjust to the median, the inspector will inspect to the median. Calling it anything else just adds more work for everyone (including redrawing geometry for the programmer) and adds risk of math errors and reading errors, such as the one you made in your original post (5.000" -.0016 to -.0032 is not 4.9984"-4.9680".)

This may not be a big deal if you're just turning and/or grinding a plain shaft, but when it comes to shafts machined as bosses on milled parts and controlled radii and blends between the shaft surface and other features it can be a big deal.

Calling it 15.0000" -10.0016 to -10.0032 is as meaningful to me as 5.0000" -.0016 to -.0032.

17. If I got a drawing that had a double minus or plus dimension I'm going to assume it's a mistake and have the engineer verify it. Then I'd probably have choice words for him/her.

At work we work to models, very few drawings exist.

18. Hot Rolled
Join Date
Feb 2013
Country
UNITED STATES
State/Province
Idaho
Posts
736
Post Thanks / Like
Likes (Given)
161
828
When I was an engineering manager, I passed a rule that everything was modeled at "nominal" dimension and all tolerances were bilateral/ symmetric. As far as I recall, this never caused any issues in the supply chain. I still model everything like that, and I look down upon any print that is toleranced any other way. I think it just shows laziness on the part of the designer/ drafter.

And yes, I am one of those lazy/ ignorant people that rarely look at the print and run everything through a CAM system. Sure, I'll glance at the print and check for weird or extremely tight tolerances. Then I program everything off the model, check key dimensions and ship the part. My customers use me because I build difficult parts extremely quickly, often times overnight. I tell them that the model is the gospel with the print only being used for the tolerances that aren't easily elucidated by the model.

I have a pretty refined system of programming and most errors can be prevented using verify on the CAM system. Programmed correctly, deviations only occur due to loading an incorrect tool or offset, excessive deflection in the part or the tool, parts being loaded incorrectly... I'm over simplifying of course, but I am just pointing out that parts that are correctly modeled to a nominal dimension are much easier to manufacture using today's technology.

19. Stainless
Join Date
Jun 2006
Country
UNITED STATES
State/Province
Alabama
Posts
1,886
Post Thanks / Like
Likes (Given)
1092
739
Originally Posted by G00 Proto
When I was an engineering manager, I passed a rule that everything was modeled at "nominal" dimension and all tolerances were bilateral/ symmetric. As far as I recall, this never caused any issues in the supply chain. I still model everything like that, and I look down upon any print that is toleranced any other way. I think it just shows laziness on the part of the designer/ drafter.

And yes, I am one of those lazy/ ignorant people that rarely look at the print and run everything through a CAM system. Sure, I'll glance at the print and check for weird or extremely tight tolerances. Then I program everything off the model, check key dimensions and ship the part. My customers use me because I build difficult parts extremely quickly, often times overnight. I tell them that the model is the gospel with the print only being used for the tolerances that aren't easily elucidated by the model.

I have a pretty refined system of programming and most errors can be prevented using verify on the CAM system. Programmed correctly, deviations only occur due to loading an incorrect tool or offset, excessive deflection in the part or the tool, parts being loaded incorrectly... I'm over simplifying of course, but I am just pointing out that parts that are correctly modeled to a nominal dimension are much easier to manufacture using today's technology.
That's pretty much how I go about most things that come across my desk

20. Stainless
Join Date
Sep 2010
Location
india
Posts
1,274
Post Thanks / Like
Likes (Given)
73
229
Targeting the mid dimension seems to be the most logical, as it will take care of variations due to random reasons. However, there was an argument some time back that since the tool wears out with time, resulting in increased size, the same tool can be used more often if we target a dimension lying towards the lower size.