Hello Colleagues ~ I work for a fairly large and diverse International company and have been “tasked” with implementing a “GLOBAL” 3D NX design standard to include the logic that “ALL parts are to be modeled to mid-range of tolerance”. Not a problem here in the USA, that’s how I was taught. However, it seems my European colleagues are NOT in agreement with this at all. Please help me to better understand their “rational” behind this. Thank you.
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What, if any, is today's "Industry standard" and/or "best practice" for creating 15
- Thread starter Kjroonie
- Start date
To be clear, nominal is not always the middle of the range. Is this the source of your disagreement?
.2500 +.0000/-.0004 would be modeled at .2500 if you were to model it to the nominal. Not .2498.
Some machine operators/programmers prefer drawing/programming to the MEDIAN of the tolerance, which would be .2498. This allows for equal deviation from the 'starting point' of manufacturing operations.
Just wanted to clarify your starting point since you seemed to equate nominal with mid-range of tolerance.
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NX8.0, Solidworks 2014, AutoCAD, Enovia V5
.2500 +.0000/-.0004 would be modeled at .2500 if you were to model it to the nominal. Not .2498.
Some machine operators/programmers prefer drawing/programming to the MEDIAN of the tolerance, which would be .2498. This allows for equal deviation from the 'starting point' of manufacturing operations.
Just wanted to clarify your starting point since you seemed to equate nominal with mid-range of tolerance.
_________________________________________
NX8.0, Solidworks 2014, AutoCAD, Enovia V5
Europeans like their standard limits & fits etc. which mostly do not start with mid range tolerance values as the 'nominal'.
Instead they'll start with the nominal hole/shaft size and may have double negative or double positive tolerances e.g 12 mm nominal +.1 +.5 or some such meaning the part could be between 12.1 & 12.5 mm.
Also from a tolerancing point of view 'min' and 'max' are valid - how do you model that at nominal?
Instead they'll start with the nominal hole/shaft size and may have double negative or double positive tolerances e.g 12 mm nominal +.1 +.5 or some such meaning the part could be between 12.1 & 12.5 mm.
Also from a tolerancing point of view 'min' and 'max' are valid - how do you model that at nominal?
Posting guidelines faq731-376 (probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484
What is Engineering anyway: faq1088-1484
- Thread starter
- #4
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CheckerHater
Mechanical
Both ISO and ASME are about the same on the matter
"For every expert there is an equal and opposite expert"
Arthur C. Clarke Profiles of the future
"For every expert there is an equal and opposite expert"
Arthur C. Clarke Profiles of the future
Kjroonie said:
Then I do not believe you are as standard as you believe. Design/Engineering models, in my experience, model to the "nominal" even if it is an unacceptable value in manufacturing. For example 1.5000" g5 (-.0003/-.0007)(ANSI B4.1 limits and fits). This is pretty common in the manufacturing world in the USA. It will be modeled at 1.5000" but woe on the programmer/machinist that cuts it to that size without reading the print. Which brings me to my next point:
I've only been in environments that push for the MEDIAN when they were machinists actually making parts. That, to them, is the "safe" place to start. It's also a lazy approach. I would say it's also a somewhat inexperienced approach, since you can change tool offsets if you're afraid of going too far past LMC/LMB on the first run.
So why do /you/ model to the MEDIAN? To me, that's extra work and more prone to human error as opposed to simply modeling to the nominal.
_________________________________________
NX8.0, Solidworks 2014, AutoCAD, Enovia V5
Model to what you need the final part to be.
If dim is .2500 +.0000/-.0004, then model at .2500.
If dim is .2496/.2500, then model at .2498.
Chris, CSWA
SolidWorks '15
SolidWorks Legion
If dim is .2500 +.0000/-.0004, then model at .2500.
If dim is .2496/.2500, then model at .2498.
Chris, CSWA
SolidWorks '15
SolidWorks Legion
If you're running in a fairly 'lean' (some might say lazy) environment where you want to virtually machine straight from the CAD model via CAM with minimal human input then most of the time going 'mean' with your model is the least likely to cause issues.
However, even if you ignore the 'standard limits & fits' aspect, there are other things. For instance drill sizes and resultant hole tolerances are often toleranced per the old Navy spec that ends up with +.005-.001 inch or similar. Also as I said, Min & Max are valid dimension schemes that are tricky to truly capture just with model geometry.
However, even if you ignore the 'standard limits & fits' aspect, there are other things. For instance drill sizes and resultant hole tolerances are often toleranced per the old Navy spec that ends up with +.005-.001 inch or similar. Also as I said, Min & Max are valid dimension schemes that are tricky to truly capture just with model geometry.
Posting guidelines faq731-376 (probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484
What is Engineering anyway: faq1088-1484
Kjroonie,
I model my parts in SolidWorks to nominal size. This suits machined and sheet metal parts, which is what I do. I like to use the ANSI/ISO fits and tolerances. This is easy when I model to nominal. Median size makes complete sense when your parts are being cast, forged, rapid prototyped, or otherwise fabricated directly from the model.
How does your company document and fabricate stuff?
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JHG
I model my parts in SolidWorks to nominal size. This suits machined and sheet metal parts, which is what I do. I like to use the ANSI/ISO fits and tolerances. This is easy when I model to nominal. Median size makes complete sense when your parts are being cast, forged, rapid prototyped, or otherwise fabricated directly from the model.
How does your company document and fabricate stuff?
--
JHG
It was long time practice to dimension the nominal to the MMC side as the machinist could then have the most margin against over-cutting, but various manufacturing methods have different offsets built into them. For milling, the machinist wants the greatest allowance for the tool wandering from the median line, while for laser or waterjet the median path runs the greatest risk of removing too much material and needs to be offset by the kerf, whatever amount that happens to be.
Shrinkage in castings and material expansion from heat treatment (due to shift in crystal structure) pose opposing requirements.
It seems like hiring some manufacturing engineers to customize derived models to be in line with specific manufacturing technology would be the best option and let the drawings and models do what they do best, communicate between engineers and Quality Assurance.
Kenat - I'm not sure where the Navy got their values (AND10387?), but the Machinery's Handbook stated the sizes of resulting holes in their tables was determined by drilling 1000 holes in either cast iron or steel with fresh drills and that actual performance will be different. Having see people try to drill room-temp rubber, I can certainly agree.
Shrinkage in castings and material expansion from heat treatment (due to shift in crystal structure) pose opposing requirements.
It seems like hiring some manufacturing engineers to customize derived models to be in line with specific manufacturing technology would be the best option and let the drawings and models do what they do best, communicate between engineers and Quality Assurance.
Kenat - I'm not sure where the Navy got their values (AND10387?), but the Machinery's Handbook stated the sizes of resulting holes in their tables was determined by drilling 1000 holes in either cast iron or steel with fresh drills and that actual performance will be different. Having see people try to drill room-temp rubber, I can certainly agree.
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MikeHalloran
Mechanical
The preceding discussion highlights a major shortcoming of 'modern' solid modeling technology; it doesn't capture the tolerances, so 'model based design and manufacturing' requires transmission of information to supplement the model file, whether drawings, standard assumptions, contractual boilerplate, whatever. There are opportunities for expensive mistakes, misunderstandings, and phase errors in such a situation.
Ask your CAD vendor when/how they'll come up to speed on tolerances.
Mike Halloran
Pembroke Pines, FL, USA
Ask your CAD vendor when/how they'll come up to speed on tolerances.
Mike Halloran
Pembroke Pines, FL, USA
Mike H -
PTC parametrics does capture most of the tolerances. Actually, when it was paired with VSA it did even more.
It is possible to go through the model and select dimensions to be nominal, minimum, or maximum for those dimensions with direct tolerances and regenerating the model will produce representative geometry, but it falls short for tolerances applied by FCFs. At least in the VSA arena those tolerances were accessible and the VSA software could make alterations to a mathematical representation of the varied geometry.
However, none of this helps because manufacturing methods require further alterations. For example, the model that is required for injection molding needs to be scaled up by varying ratios based on the plastic characteristics; a similar requirement exists for making patterns for sand casting. I cannot imagine any universal system addressing this, though I've had over 30 years of making CAD 3D models, many of which were taken for manufacturing use.
Then one runs into parts that have extra material for processing that must be removed afterwards, like formed tubes where the bend ends too close to the nominal end. Extra material to support the bending can be trimmed after, but it would not be a normal part of the model.
PTC parametrics does capture most of the tolerances. Actually, when it was paired with VSA it did even more.
It is possible to go through the model and select dimensions to be nominal, minimum, or maximum for those dimensions with direct tolerances and regenerating the model will produce representative geometry, but it falls short for tolerances applied by FCFs. At least in the VSA arena those tolerances were accessible and the VSA software could make alterations to a mathematical representation of the varied geometry.
However, none of this helps because manufacturing methods require further alterations. For example, the model that is required for injection molding needs to be scaled up by varying ratios based on the plastic characteristics; a similar requirement exists for making patterns for sand casting. I cannot imagine any universal system addressing this, though I've had over 30 years of making CAD 3D models, many of which were taken for manufacturing use.
Then one runs into parts that have extra material for processing that must be removed afterwards, like formed tubes where the bend ends too close to the nominal end. Extra material to support the bending can be trimmed after, but it would not be a normal part of the model.
Mike, ASME Y14.41 attempts to set the baseline for Model Based Definition and various CAD packages have implemented it to varying extents and in integrated supply chains it has been made to work supposedly.
However, for those of us outside of that environment there are still more questions than answers.
However, for those of us outside of that environment there are still more questions than answers.
Posting guidelines faq731-376 (probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484
What is Engineering anyway: faq1088-1484
It looks to me like you are working on a problem that does not exist. If someone in your company asked you to come up with a "NEW GLOBAL STANDARD" than ask them why they do not want to use the existing global standard. Do they want to change what is used around the world?
I believe someone in your company does not have a clue what he is asking you to do. The world wide standard for manufacturing is laid out by ISO. ANSI is part of it. Get to know ISO 286. If you are a world wide company than that is the ONLY standard that is accepted world wide.
I believe someone in your company does not have a clue what he is asking you to do. The world wide standard for manufacturing is laid out by ISO. ANSI is part of it. Get to know ISO 286. If you are a world wide company than that is the ONLY standard that is accepted world wide.
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ASME 14.41 is how to draft without making drawings. Instead there are view dependent and view independent annotations (sigh. Because annotation is something added to an otherwise complete work and the 14.41 guys thought it meant symbology and other notations. The model is not complete without tolerances and notes, so they aren't annotation**.)
I don't recall 14.41 specifying a distinct CAD data format from which one could create a translator of all 14.41 compliant models and I don't recall them specifying a single interface for 'interrogating' the model so that everyone approaching the CAD data would have the same steps to get the same information.
Basically it translates what people used to do with 2D CAD drawing and adds some things that they thing would make it easier, but as it is all things to all users, it is nothing to anyone in particular. The only other thing it does is support oblique projections of text and notations.
MIL-STD-31000 is probably better, but only by a fraction. If I had to guess, I think 14.41 was driven more by Seimens and 31000 by PTC, but it's been a while so it's worth checking. For example, in 31000 is "The TDP format will be clearly stated in the SOW with an understanding of how lifecycle maintenance of the TDP will be performed. When specifying the TDP format, it is important to provide sufficient technical detail—for example, Creo 1.0 (native CAD with version number), STEP AP 203 E2, 3D PDF with PRC (ISO 14739), or other unambiguous electronic format specifications. Other format details should be provided as required in A.3.2.8 Block 8. Applicability of Standards—for example, specifying ASME Y14.5 and ASME Y14.41 for fully annotated 3D models."
**
An annotation is metadata (e.g. a comment, explanation, presentational markup) attached to text, image, or other data. Often annotations refer to a specific part of the original data.
1. a critical or explanatory note or body of notes added to a text.
I don't recall 14.41 specifying a distinct CAD data format from which one could create a translator of all 14.41 compliant models and I don't recall them specifying a single interface for 'interrogating' the model so that everyone approaching the CAD data would have the same steps to get the same information.
Basically it translates what people used to do with 2D CAD drawing and adds some things that they thing would make it easier, but as it is all things to all users, it is nothing to anyone in particular. The only other thing it does is support oblique projections of text and notations.
MIL-STD-31000 is probably better, but only by a fraction. If I had to guess, I think 14.41 was driven more by Seimens and 31000 by PTC, but it's been a while so it's worth checking. For example, in 31000 is "The TDP format will be clearly stated in the SOW with an understanding of how lifecycle maintenance of the TDP will be performed. When specifying the TDP format, it is important to provide sufficient technical detail—for example, Creo 1.0 (native CAD with version number), STEP AP 203 E2, 3D PDF with PRC (ISO 14739), or other unambiguous electronic format specifications. Other format details should be provided as required in A.3.2.8 Block 8. Applicability of Standards—for example, specifying ASME Y14.5 and ASME Y14.41 for fully annotated 3D models."
**
An annotation is metadata (e.g. a comment, explanation, presentational markup) attached to text, image, or other data. Often annotations refer to a specific part of the original data.
1. a critical or explanatory note or body of notes added to a text.
Here's what the NIST has on the matter specifically "A Portrait of an ISO STEP Tolerancing Standard as an Enabler of Smart
Manufacturing Systems"
Manufacturing Systems"
juergenwt, the OP is talking about modelling best practices, not just limits and fits.
Posting guidelines faq731-376 (probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484
What is Engineering anyway: faq1088-1484
I think the discussion about standards (ASME Y14.41, ISO, etc) is premature. I believe the solution is in the word "context" which comes before the question of which standard to follow.
The only reason not to model to the NOMINAL dimension is, as we have all discussed, for manufacturing purposes.
To me, (call it JN 101.1
), the solution to this is that there is an Engineering/Design Model separate from a Manufacturing/Programming Model. Or if it must be in the same model in-house, put some modeling features on a separate layer compliant with a company standard. Have the nominal model as the base of things. Have your "additional thickness for machining" and "scaled by .99965 to account for growth in oven" type modifiers on a separate layer. Leave the modified manufacturing models to the manufacturers. Ensure proper revision control and have a separate model for programming/machining than you do for the engineering model which needs the nominals to drive the proper dimensions, tolerances, annotation, etc.
If you decide to have separate models, then it's completely appropriate to ask which standard you adhere to for the Engineering Models/Documents, and then most likely you would use company standards for the manufacturing methods/models/modifications.
_________________________________________
NX8.0, Solidworks 2014, AutoCAD, Enovia V5
The only reason not to model to the NOMINAL dimension is, as we have all discussed, for manufacturing purposes.
To me, (call it JN 101.1
), the solution to this is that there is an Engineering/Design Model separate from a Manufacturing/Programming Model. Or if it must be in the same model in-house, put some modeling features on a separate layer compliant with a company standard. Have the nominal model as the base of things. Have your "additional thickness for machining" and "scaled by .99965 to account for growth in oven" type modifiers on a separate layer. Leave the modified manufacturing models to the manufacturers. Ensure proper revision control and have a separate model for programming/machining than you do for the engineering model which needs the nominals to drive the proper dimensions, tolerances, annotation, etc.If you decide to have separate models, then it's completely appropriate to ask which standard you adhere to for the Engineering Models/Documents, and then most likely you would use company standards for the manufacturing methods/models/modifications.
_________________________________________
NX8.0, Solidworks 2014, AutoCAD, Enovia V5
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CheckerHater
Mechanical
OK, let's go back to OP.
Imagine that we have "GLOBAL" design standard to keep our clearance holes to H14.
We model all the holes to the median.
Then some overzealous engineer decides to change it to H12.
Now we have to go back and re-model every hole to another median.
I don't see it happening. The only sane way I see is to model everything to BASIC.
Because when you have your nominal and your tolerance you can do anything you want, including creating separate model for manufacturing purpose.
And when all you have is model where everything is modeled to some bastard "median" - good luck! Especially after you convert this model to STEP and send to China.
"For every expert there is an equal and opposite expert"
Arthur C. Clarke Profiles of the future
Imagine that we have "GLOBAL" design standard to keep our clearance holes to H14.
We model all the holes to the median.
Then some overzealous engineer decides to change it to H12.
Now we have to go back and re-model every hole to another median.
I don't see it happening. The only sane way I see is to model everything to BASIC.
Because when you have your nominal and your tolerance you can do anything you want, including creating separate model for manufacturing purpose.
And when all you have is model where everything is modeled to some bastard "median" - good luck! Especially after you convert this model to STEP and send to China.
"For every expert there is an equal and opposite expert"
Arthur C. Clarke Profiles of the future
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