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deveation question 2
- Thread starter beebo666
- Start date
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)
Chris
SolidWorks 06 5.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 01-18-07)
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.
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
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
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)
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)
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1
- #25
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.
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.
aardvarkdw
Mechanical
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
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
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.
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.
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.
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.
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
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
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?
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?
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.
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.
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
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
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