+/+ tolerances? 1

[MikeHalloran]

Bearing seat dimension is nominally 4.7244" diameter. The model is constructed that way. Now I'm tolerancing the drawing.

I want to show limit dimensions as 4.7251/4.7245.

SW was having none of it. When I put a negative value in the (-) deviation, SW seemed to take the absolute value. Sorry, I'm used to another package that interprets a negative value for a minus deviation to mean plus.

I was able to force what I want by giving SW an override primary value of 4.7245 (which it insisted on displaying as 4.725 within its dialog box), and specifying deviations of -0/+.0006.

Is there a better way to get SW to deal with press fits?



Mike Halloran
Pembroke Pines, FL, USA

 

[CorBlimeyLimey]

Try typing a + in the - field.

 

[TheTick]

Where, oh where, is such a tolerance permissible within ASME Y14.5M (or ISO or DIN or anywhere)?

 

[Eltron]

I'm not able to duplicate your results. Where are you typing the information about your limit tolerance?

Dan

http://www.eltronresearch.com

 

[engAlright]

I am also curious as to how this +/+ dim works...how can you have a nominal dim that falls outside of the tolerance range?

 

[ctopher]

In this case, it isn't nominal. It's the dim the part is designed for with a +/1 tol.
If it were nominal, it would be 4.7248 +/- .0003.

Chris
SolidWorks 07 4.0/PDMWorks 07
AutoCAD 06
ctopher's home (updated 04-21-07)

 

[MikeHalloran]

Thanks, CBL. That worked just fine.





Mike Halloran
Pembroke Pines, FL, USA

 

[MikeHalloran]

The part is a shaft that's carried by a ball bearing with a 120mm bore. The shaft has to be a little oversize to press into the bearing race.





Mike Halloran
Pembroke Pines, FL, USA

 

[CorBlimeyLimey]

"Is there a better way to get SW to deal with press fits?"
Check out the options in the Tolerance / Precison section of the Dimension Manager. It has selections for the type of fit required along with the corresponding alpha-numeric designations.

IMO, the Override option should never ever be used. In fact, SW should never have made that an option.

 

[Eltron]

That's sort of what I was suggesting to Mike's OP, CBL. The Dimension Manager should be able to get you where you need to go.

Dan

http://www.eltronresearch.com

 

[MikeHalloran]

CBL, I removed the override and read up on the Dimension Property Manager.


Thanks again.



Mike Halloran
Pembroke Pines, FL, USA

 

[crjones]

Could you be talking about "Fits and Limits"? It's in the dimension manager, called fit, fit with tolerance, or fit with tolerance only. In life it's called ANSI B4.1 and can be found in "Machinery's Handbook." It will allow a double positve or double negative tolerance. It is useful in examining the fits of multiple components on a common shaft.

 

[fcsuper]

I use CBL's method a lot. It is useful on molded parts where the desired results of the mold don't made the model. Simply using a plus in both +/- fields gives you exactly what you are asking for. Just do the math to make sure you are printing the numbers you desire. There wouldn't be anything against ASME to do this since the drawing is the specification in those cases.

The other option is to use the override, as also mentioned. I use this method more commonly these days, but it wasn't available on older versions of SW.


Matt
CAD Engineer/ECN Analyst
Silicon Valley, CA
sw.fcsuper.com
Co-moderator of Solidworks Yahoo! Group

 

[CorBlimeyLimey]

The other option is to use the override .... I use this method more commonly these days

Shame on you!

 

[drawoh]

TheTick,

Where, oh where, is such a tolerance permissible within ASME Y14.5M (or ISO or DIN or anywhere)?

+/+ tolerances are not explicitly shown in ASME Y14.5M-1994, but they are not explicitly banned either. In ISO406, Figures_12 and_13 show +/+ and -/- dimensions. Strictly speaking, the diagrams show assembled components with nominal dimensions and tolerances slopping the same way.

ISO406 is sort of more permissive about this.

Sometimes it is useful to show the actual modeled CAD dimension in addition to the permitted variation. Think about the machine shop that asks for a DXF of your fabrication drawing so that they can program their CAM machine.

JHG

 

[TheTick]

Personally, I would still never allow this on a part drawing.

 

[MikeHalloran]

I personally don't care for +/+ tolerances on a drawing, either. That's why I used limits for that dimension. The person reading the drawing will never know that the nominal lies outside the limits.

Which still leaves the problem of using DXFs. Too bad that their native world, architecture, doesn't use tolerances, so they're not in the standard.




Mike Halloran
Pembroke Pines, FL, USA

 

[handleman]

Please tell me that I misunderstand you. You would not allow "oversize" or "undersize" tolerances on a drawing? It's used all the time in machine design. Nearly all the ISO shaft/hole tolerances are over or under the nominal on both sides of the tolerance. Are you saying that you would dimension (and model!) an 18mm g6 toleranced shaft as 17.9885±0.0115 rather than 18 -0.006/-0.017? What's the point? So that your machinist doesn't have to do a little math?

 

[TheTick]

I've learned the hard way not to count on others' math skills or knowledge of standards, especially outside vendors.

The limit dimension seems to be the lesser of two evils. I would still model to actual size. I've had mold makers build right off the model without even looking at prints, only to find that molds were not "steel safe" as a result.

Ask for what you want, on the drawing and in the model.

 

[MikeHalloran]

I'd model at the nominal, and in the case of +/+ or -/- tolerances give limit dimensions... because they limit the number of phone calls you get.

Sure, I'd trust a real machinist to do a little math, or figure out a fit, but inspectors often enough seem to be pulled from the casual labor pool.



Mike Halloran
Pembroke Pines, FL, USA