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deveation question
2

deveation question

deveation question

(OP)
is it acceptable practice to show two negatives in a tolerance. for example .756 -.001/-.002? thank you.

RE: deveation question

I have seen this done on manual drawings, but it doesn't meet the requirements of associative dimensioning with most CAD drawings/models.  The model should represent the actual part, and such a dimension would not reflect the size of the actual hole without manually editing the dimension.
While I am unaware of any, there may be CAD packages out there that will handle this type of dimensioning.

RE: deveation question

There certainly are CAD systems that can work this way and it is a perfectly normal way to dimension shafts and holes.

RE: deveation question

Take a look at your tolerance stackups, there may be a good reason for this.

David

RE: deveation question

ajack,
I was hoping that there was some software that could handle this (model at actual, dimension at two negative or positive limits - not actual).

RE: deveation question

There is. Vero certainly does it.

RE: deveation question

Inventor will allow you to do this!

David

RE: deveation question

Dumb question, but "Why would you want 2 minus tolerances?"  Have not seen or heard of.

RE: deveation question

Nominal size hole with a press fit maybe?

David

RE: deveation question

(OP)
man i really opend a can o worms here. but i asked because i got a customer drawing with that double minus tolerance.and from what i have read that is acepatable in metric drawings but not is US units. thanks for all the responses.

RE: deveation question

ewh,

   I did not know there was a CAD program that did not support double (-) or double (+) tolerances.  The advantage of this procedure is that your dimension shows the nominal dimension.  This is useful design information, however weird it looks to the fabricator.  What matters to you?

   I suppose you need a convention in your CAD office about how you model dimensions.  I model to exact nominal size, and I apply tolerances.  If I have to design something that mates to your part, I must examine your drawings, or at least look at the tolerances you applied to your 3D_model.  This is true even if I understand how you scale your features.  The size of your model, however you did it, is not an adequate guide.

                          JHG

RE: deveation question

We have to model to the actual finished dimension.  We could use double negative or double positive tolerancing, but we would either have to lose the associativity to the feature by editing the dimension, or model the feature at the nominal, which may not reflect the actual finished part.
Please don't get me started on non-associative dimensioning.  They cause nothing but problems for us.

RE: deveation question

ewh,

What program do you use?

David

RE: deveation question

UGS NX4

RE: deveation question

I also don't know why anyone would do this. I have never seen it. But, doesn't mean it isn't possible.

Chris
SolidWorks 06 5.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 01-18-07)

RE: deveation question

I understand the reasoning behind its use, but I think it may be becoming rarer as MBD comes into its own.  Depends on how the software is used and what the company dictates.  To use it effectively, you have to model to nominal dimensions rather than actual, which may cause problems downstream in regards to any further analysis on that model or any higher assemblies.

RE: deveation question

I have never used UGS so I can't say anything in respect to it but I know Inventor allows you to dimension nominally and then appl a tolerance directly to the model dimension which is then parametric between the drawing and the model. I beleive Solidworks has this cabability as well. I agree with Chris though I don't see why you would want to do this except under a pretty specific set of circumstances. One instance that comes to mind is one in which you have a nominal size part like a dowel pin that you are then polishing to a slip fit. The nominal dimension would then be larger than any acceptable tolerance. Just a thought...

David

RE: deveation question

David,
When you dimension nominally, is your part modeled at nominal?

RE: deveation question

Yeah, which means that you don't have a graphical representation of the tolerance and if you use the measure tool to check the feature size you get the nominal size. The sketch dimensions show the tolerance if you tell the program to display them that way.

David

RE: deveation question

David, that is good. Models should always be modeled at nominal.

Chris
SolidWorks 06 5.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 01-18-07)

RE: deveation question

I generally agree with that, Chris, especially when the tolerances are equidistant from the nominal.  In a situation such as the OP brings up though, I still won't model to a nominal size that the feature will never be.  I would model it at the center of the two tolerances.  If a stress engineer wants to analyize it later, he will see the true interference or clearance based on that midpoint.

RE: deveation question

ewh,

   The ANSI standard fits are based on ISO tolerance classes.  Assume my nominal diameter is 3/4", that I want to use an FN2 fit, and that I want to check stresses.

Shaft:   .750+.0019/+.0014, ISO s6
  .7519
  .7514
  or we could go .7514+.0005/0

Hole:  .750+.0008/0, ISO H7
  .7508
  .7500

   The interference goes from .0006" to .0019".  If you are working out stresses and torques, you can work with the nominal size and the maximum and minimum interferences.  I cannot see that the difference between the nominal size and the median allowable size is significant.  

   Meanwhile, I want to change from an FN2 fit to an FN1 fit.  If everything is modeled to nominal size, I review four tolerance values.  If I used median values, I have to recalculate the two median values and then fix the four tolerance values.

                        JHG

RE: deveation question

ewh,
I model to nominal mainly for CAM purposes.
If stress analysis is critical for the part, then I would create configurations of the tolerances.
Everywhere I have worked, this always has been an issue ... "what exactly do we model to?" We always end up with nominal.

Chris
SolidWorks 06 5.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 01-18-07)

RE: deveation question

nominal, nominal, nominal

I seem to recall double negative, in fact I think I've had to force Solid Edge to do it, it was a while back though and I can't recall how or why, I think it may have been rivet holes but I'm not sure that sounds right.

And while your at it don't have dimension in the model to an infinite number of decimal places while the corresponding dimension on the drawing is only displayed to 1, 2 or 3 DP.

RE: deveation question

Chris,
That is the main reason we model as we do - CAM.

RE: deveation question

Kenat,

I agree wholeheartedly! That is one of my biggest pet peeves. I see it all the time where I work, people getting lazy with dimensions (not giving a value just eyeballing) and then the problem continues throughout the whole assembly because you can't force the software to accept a mate constraint that is .0001 off.

David

RE: deveation question

KENAT,
I understand your position on this, and agree from a drawing standpoint, but how do you allow for MBD and CAM if you only use nominal dimensions in your model?  The CAM programmers I know seldom if ever look at a drawing when programming, but will go back and tweak their program after the fact.  This is an opportunity for mistakes.

RE: deveation question

I have seen the dbl neg tolerance on a lot of machine designs. Also the Carr-Lane bushings are all dbl neg..

I don't know anything but the people that do.

RE: deveation question

I've not looked at 14.41 so will admit I'm not really adressing MBD.  However from what little sending of dumb solids out to machinists I've done I thought nominal (as in halfway between max and min, not 'nominally 1" when it's actually .997-.999) was preffered.

The one exception I think I have to this is our standard hole settings which are based around drill sizes & tolerances which aren't unilateral.

Perhaps I'm misunderstanding your post as I thought you agreed on my understanding of nominal.

RE: deveation question

In our company we allways create the models in the mean size,(upper limit+lower limit)/2
doesn't matter how the dimension appears on the drawing.

RE: deveation question

Y14.41 allows for models at max, least, or mean condition.

Kenat brings up a good point regarding drill sizes and their tolerances.  I've always assumed +.005/-.000 for most.  

RE: deveation question

We agree, KENAT.  I was referring to "nominal" in the sense of the OP (1.00 -.xxx/-.xxx), which the actual part will never see.

RE: deveation question

rltlw,

Are you speaking for the tolerances on the drill bit or the tolerances on the drilled hole?

RE: deveation question

Drilled hole.  I'm not sure where I saw that or what the drill size range is for that...

RE: deveation question

rltw,

   The tolerance of drilled holes is explained in the Machinery's Handbook.  They have a table showing the dimension range you should expect from a given size drill in steel and cast iron given an average machine shop and a properly ground drill.

                     JHG

RE: deveation question

On the main CAD system we use if you wish to add a H7 tolerance for example you have to model it to the nominal size, say 30 mm, if you model to the mean say 29.995 you lose that option.

If you model to nominal the tolerances including the H7 and limits come from a drop down menu, as stated above as this is an ISO standard I have always assumed this is the correct way, could I be wrong?

RE: deveation question

I'm not sure there is a single wrong/right answer.  Different CAD systems do some things differently.  There are so many things to consider in model creation as well as the basic design - keeping feature tree manageable, keeping file size down, making it easy for future users to change, modeling to support the drawing (assuming non MBD), support CAM, support use in stress analysis, and others I've probably missed, that keeping everyone happy off one model isn't always possible.  To some extent things like different configurations & simplifications of parts/assemblies help but still may leave dissatisfied customers!

Our hole settings are based on the tables in machinery’s handbook, adjusted to suit our needs.  For instance one table we looked at the C'bore for the screws weren't big enough and didn't fully allow for float of the screw in the hole, so we enlarged them.  We also worked out C'bore for button heads which may sound odd but means for our application we often can use buttons heads instead of CSK so preventing a 'fixed-fixed' tolerance situation.

ewh - perhaps for what I was using nominal isn't the best term, perhaps mean is better, but nominal is what I've always tended to hear used.

RE: deveation question

ajack1,

   As I noted above, I would prefer that things are modeled to the nominal dimension.  You process works fine for me.

   As I also noted above, if I am going to fabricate your part or design a mating part, I have to learn your tolerances.  I must carefully examine your drawing, and compare the tolerance text with the text on my drawing.  It would be more convenient if each of us followed a standard, predictable procedure, but if you are outside my organization, I cannot make assumptions.

   Here is another limitation of CAD.  In the FN2 fit I described above, the MMC sizes, the median sizes and even the LMC sizes interfere.  If I use any of these sizes in SolidWorks, I am not going to see the seam in my isometric drawing views.  If both features are nominal, SolidWorks works fine.

   What about nominal dimensions like 19.05mm?

                         JHG

RE: deveation question

Some CAD systems (at lease Solid Edge) can deal with showing 'interferences' in the drawings.  It takes more processor power so by default is off but can do it.

RE: deveation question

NX can handle interferences on the modeling side quite well, but sometimes gets confused on the drafting side.  Instead of two edges for example, it sometimes won't show any.

RE: deveation question

Metric drawings tend to show a double - or a double + number. Their drawings use a standard mm dimension and then deviate with the tolerances.

RE: deveation question

A tolerance with both on the minus side just doesn't make sense in the real world but I have seen them on some European drawings.

On the shop floor, one still has to calculate the centre value or nominal and convert to a bi-lateral tolerance and there is a bigger chance of math errors.

Don't do it. It does not help anyone and rather confuses.

Dave D.
www.qmsi.ca

RE: deveation question

I must say I do find the view of Dingy 2 strange, is Europe not in the real world?

Using double plus or minus has long been a standard over here in the UK going back long before ISO or metric, the concept is simple you look what sort of fit you want, drive, slide, clearance etc look at the corresponding values and there you have it.

This of course makes all sizes standard, most bearings, shafts, bushes, couplings and the like are toleranced in this way, what could be simpler, unless of course you struggle with very basic maths?

I must say I am amazed  this is not a standard in the USA. I am sure I have seen it on NAMMS standard flying cams for example, perhaps I am wrong.

RE: deveation question

It is used in the US, it just isn't standard.  Our standards tend to reflect manufacturing and inspection.  For design purposes, using a nominal value with double - or double + tolerance can be of value.  In the "real" physical world, those values are never seen and thus we tend to not use them.

RE: deveation question

ajack1,

   My understanding is that when you place an accurate dimension on a diameter, limit dimensions are clearest to the fabricators and inspectors.  As a designer, I like to see nominal dimension and tolerances.  I do not care if they both go in one direction.  It makes sense to me because I can see the mating part, although other people seem to get confused.  When I finalize drawings, I try to remember to convert my tolerances.  

   You have to ask yourself who is going to be using your drawings.  From my design point of view, a shaft goes into a hole.  I mark the ANSI fit class on my assembly drawing or arrangement.  The dimensions on the fabrication drawings are nothing more than the solution to an arithmetic problem.

                      JHG

RE: deveation question

I must say I find this strange, to take the most basic example a dowel in a reamed hole we would call up for example a 12mm m6 dowel and a 12mm H7 hole. So do ½” dowels not exist as they are .5001 dowels and ½” reamed holes not exist, as they are .4998” ? The exact figures maybe wrong.

If you do have ½” dowels and reamed holes why is a shaft, bearing, bush or whatever any different?

RE: deveation question

ajack1,

   As far as I am concerned, 1/2" dowels do exist.

   Try to distinguish between nominal diameter and mean or median diameters.  For a 1/2" hardened, ground dowel pin, I claim that the nominal size is .5000", or 12.7mm.  If the size range is between .5001 and .5003", the median size is .5002".  

                      JHG

RE: deveation question

I am a UGS consultant and the as for mentioned tolerance is a valid callout. This is applied mostly in the Aerospace domain.

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