artnmotion
Mechanical
When you have a Dimension calling out MAX on a drawing (1.000 MAX), what keeps the machinist from giving you .800?
Is there a standard for this callout?
Thanks.
Is there a standard for this callout?
Thanks.
Tek-Tips is the largest IT community on the Internet today!
Members share and learn making Tek-Tips Forums the best source of peer-reviewed technical information on the Internet!
-
Congratulations cowski on being selected by the Eng-Tips community for having the most helpful posts in the forums last week. Way to Go!
Dimension + MAX (or MIN that matter) 4
- Thread starter artnmotion
- Start date
- Status
Re:"what keeps the machinist from giving you .800"
Nothing. Probably just "good workmanship"
The machinist can give you 0 (zero). It is smaller than 1.000
Just my opinion
How you make a distinction between: "good workmanship" versus "poor workmanship". By having a fully defined drawing.
1.000 MAX = The drawing/feature is not fully defined = drawing incomplete.
Nothing. Probably just "good workmanship"
The machinist can give you 0 (zero). It is smaller than 1.000
Just my opinion
How you make a distinction between: "good workmanship" versus "poor workmanship". By having a fully defined drawing.
1.000 MAX = The drawing/feature is not fully defined = drawing incomplete.
-
1
- #3
Use of MAX and MIN are allowed under Y14.5-2009 "where other elements of the design definitely determine the other unspecified limit" and "where the
intent will be clear, and the unspecified limit can be zero or approach infinity and will not result in a condition detrimental to the design."
“Know the rules well, so you can break them effectively.”
-Dalai Lama XIV
intent will be clear, and the unspecified limit can be zero or approach infinity and will not result in a condition detrimental to the design."
“Know the rules well, so you can break them effectively.”
-Dalai Lama XIV
I don't believe a drawing with 1.000 MAX is necessarily incomplete. There are cases (usually radii or chamfers) where it is useful, if you truly don't care if the feature you're defining can be small or even nonexistent.
I think that for what I would call a "complete feature of size" it wouldn't be useful, i.e. thickness of a plate, or diameter of a hole or cylinder.
It's a tool that can be used, if used correctly and intelligently.
To answer the OP question, there is no standard that I am aware for this - what you see is what you get:
1.000 MAX = 0.000-1.000
I think that for what I would call a "complete feature of size" it wouldn't be useful, i.e. thickness of a plate, or diameter of a hole or cylinder.
It's a tool that can be used, if used correctly and intelligently.
To answer the OP question, there is no standard that I am aware for this - what you see is what you get:
1.000 MAX = 0.000-1.000
- Thread starter
- #5
CheckerHater
Mechanical
See also here:
And here:
And here:
-
1
- #7
I use MAX on small radii all the time on non-critical corners. It can be sharp or the radius. This helps the machinists with tool radii.
I agree with the others.
Chris, CSWA
SolidWorks 14
SolidWorks Legion
I agree with the others.
Chris, CSWA
SolidWorks 14
SolidWorks Legion
Sorry greenimi what rot. There are times and places for Max & Min.
As mentioned, nothing stops the machinist giving you .800 since .800 is less than 1.000 in any form of math I can think of that would apply.
artnmotion said:
As mentioned, nothing stops the machinist giving you .800 since .800 is less than 1.000 in any form of math I can think of that would apply.
Posting guidelines faq731-376 (probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484
What is Engineering anyway: faq1088-1484
- Thread starter
- #9
artnmotion
Mechanical
2.5 SINGLE liMITS
MIN or MAX is placed after a dimension where other
elements of the design definitely determine the other
unspecified limit. Features, such as depths of holes,
lengths of threads, comer radii, chamfers, etc., may be
limited in this way. [highlight #8F5902]Single limits are used where the
intent will be clear, and the unspecified limit can be zero
or approach infinity and will not result in a condition
detrimental to the deSign.[/highlight]
MIN or MAX is placed after a dimension where other
elements of the design definitely determine the other
unspecified limit. Features, such as depths of holes,
lengths of threads, comer radii, chamfers, etc., may be
limited in this way. [highlight #8F5902]Single limits are used where the
intent will be clear, and the unspecified limit can be zero
or approach infinity and will not result in a condition
detrimental to the deSign.[/highlight]
Calling out "1.00 MAX" is defined. It's legal. It's determined with what you want your part to be.
If you can live with anything below that, like .800, so be it.
If you can't have .002 for example, that callout the limit tolerance needed.
Calling out "1.00 MAX leaves it to the machinist to make it anything 1.00 or below. It's also up to the engineer to make sure whatever the material is that the last process made to the part that the design holds up to 1.00 MAX (shrinkage, expansion, etc).
Chris, CSWA
SolidWorks 14
SolidWorks Legion
If you can live with anything below that, like .800, so be it.
If you can't have .002 for example, that callout the limit tolerance needed.
Calling out "1.00 MAX leaves it to the machinist to make it anything 1.00 or below. It's also up to the engineer to make sure whatever the material is that the last process made to the part that the design holds up to 1.00 MAX (shrinkage, expansion, etc).
Chris, CSWA
SolidWorks 14
SolidWorks Legion
-
2
- #11
Something for all to think about, which has nothing to do with ASME. As a courtesy to the machinist, when specifying a max. internal radius (say, in a pocket), avoid using something just less than a fraction, e.g. "R.12 MAX". This prevents the use of a 1/4 end mill (which would result in R.125), and forces the use of a smaller tool. Better to specify "R.13 MAX". Of course, if the design requires such, fine and dandy, but most of the time these things are not critical. Forcing the machinist to use a smaller tool with no benefit to the quality of the part may result in increased cost with no benefit.
It depends on the design.
It doesn't make a difference if "R.12 MAX" vs "R.13 MAX" is called out, the machinist has to make it per print.
When I call out an internal radius, I always look at the available tool size that can fit to help the machinist.
Chris, CSWA
SolidWorks 14
SolidWorks Legion
It doesn't make a difference if "R.12 MAX" vs "R.13 MAX" is called out, the machinist has to make it per print.
When I call out an internal radius, I always look at the available tool size that can fit to help the machinist.
Chris, CSWA
SolidWorks 14
SolidWorks Legion
ctopher, with all due respect, I think you're missing my point. The point is cost. If a non-critical internal radius is dimensioned in a way that causes more machine time (due to smaller tool), then extra cost may be being added to the part with no benefit. Designing for ease (read: economy) of manufacturing should always be considered...
TWJR,
I agree, I get the point.
It comes down to designing the part. Machine time, cost, ease of mfg, all has to be looked at.
But, whatever the drawing shows, the machinist has to make the part per print. Having a callout 1.00 MAX may (or may not) help make the part cheaper.
If the dim is a radius, the machinist can use a dull tool to make any radius smaller than 1.00.
Chris, CSWA
SolidWorks 14
SolidWorks Legion
I agree, I get the point.
It comes down to designing the part. Machine time, cost, ease of mfg, all has to be looked at.
But, whatever the drawing shows, the machinist has to make the part per print. Having a callout 1.00 MAX may (or may not) help make the part cheaper.
If the dim is a radius, the machinist can use a dull tool to make any radius smaller than 1.00.
Chris, CSWA
SolidWorks 14
SolidWorks Legion
So you're saying the only problem with the OP's drawing is that' it's 1.000 MAX not 1.010 MAX 
You make a valid point though TWJR, making a bit of allowance for DFM while tolerancing things should be common/good practice but isn't always.
You make a valid point though TWJR, making a bit of allowance for DFM while tolerancing things should be common/good practice but isn't always.
Posting guidelines faq731-376 (probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484
What is Engineering anyway: faq1088-1484
Kenat and ctopher,
I think you misunderstand me. I wasn't directly responding to the OP's issue. I was adding some useful info (to me) in general terms, when specifying MAX in the case of an internal radius. As a person with one foot in manufacturing (I design and program CNCs) I'm acutely aware of how a seemingly little thing can drive up the cost of a part. To say the machinist simply "has to make the part to the print" is technically true, but we as designers should be trying to make the parts as easy to make (read: cheaper) as possible without impacting the function. I'm sorry if it sounds like I'm trying to hijack this thread. I'm not. I was just trying to be helpful, but apparently I'm being taken to the woodshed.
I think you misunderstand me. I wasn't directly responding to the OP's issue. I was adding some useful info (to me) in general terms, when specifying MAX in the case of an internal radius. As a person with one foot in manufacturing (I design and program CNCs) I'm acutely aware of how a seemingly little thing can drive up the cost of a part. To say the machinist simply "has to make the part to the print" is technically true, but we as designers should be trying to make the parts as easy to make (read: cheaper) as possible without impacting the function. I'm sorry if it sounds like I'm trying to hijack this thread. I'm not. I was just trying to be helpful, but apparently I'm being taken to the woodshed.
TWJR,
I understand.
But, your response "To say the machinist simply "has to make the part to the print" is technically true" seems to me that you think it's not 100% true?
Machinists have to make the part to print, regardless how the designer (or whomever) made the drawing.
I agree the drawing needs to be complete and as cheap as possible, that's why the drawings need to be checked.
I see drawings every day that are dimensioned wrong and right, but misinterpreted wrong. So, it's our jobs to make them readable and understandable.
Chris, CSWA
SolidWorks 14
SolidWorks Legion
I understand.
But, your response "To say the machinist simply "has to make the part to the print" is technically true" seems to me that you think it's not 100% true?
Machinists have to make the part to print, regardless how the designer (or whomever) made the drawing.
I agree the drawing needs to be complete and as cheap as possible, that's why the drawings need to be checked.
I see drawings every day that are dimensioned wrong and right, but misinterpreted wrong. So, it's our jobs to make them readable and understandable.
Chris, CSWA
SolidWorks 14
SolidWorks Legion
Yes, you are correct. At the end of the day, the part has to be made to the print. Perhaps I'm not being clear. I'm just saying that what what we can do as designers can go a long way towards economy of parts. I've known a lot of engineers and designers that design stuff that's difficult to make and are extremely hard headed when it comes to designing with manufacturing in mind. We all should be doing that. I've programmed a lot of parts, and have made a lot of parts in my former career as a machinist which due to unnecessary tolerances, poor choices of material, or other things make a part much more expensive than it has to be to do the job.
I don't think anyone has said machinist's can't make it to print, or can even bend the rules.
All TWJR is saying is that the difference between ".12 MAX" and ".13 MAX" is quite significant. So simply rounding to the nearest even number is /NOT/ always the wisest decision. If the designer CAN tolerate .13, it is wise to do so, rather than rounding to .12. If talking about the IR of an otherwise rectangular pocket, the difference between .12 and .13 MAX IR is a tool change, a great shortening of tool path and therefore cut time, as well as money.
No one is saying anyone should make parts that are not true to print - it was suggested that you think about the context of your "rounding" and pick the best number for the design (including cost) rather than sticking to mindless rules (always round halves to the nearest even number) without considering their repurcussions.
_________________________________________
NX8.0, Solidworks 2014, AutoCAD, Enovia V5
All TWJR is saying is that the difference between ".12 MAX" and ".13 MAX" is quite significant. So simply rounding to the nearest even number is /NOT/ always the wisest decision. If the designer CAN tolerate .13, it is wise to do so, rather than rounding to .12. If talking about the IR of an otherwise rectangular pocket, the difference between .12 and .13 MAX IR is a tool change, a great shortening of tool path and therefore cut time, as well as money.
No one is saying anyone should make parts that are not true to print - it was suggested that you think about the context of your "rounding" and pick the best number for the design (including cost) rather than sticking to mindless rules (always round halves to the nearest even number) without considering their repurcussions.
_________________________________________
NX8.0, Solidworks 2014, AutoCAD, Enovia V5
- Status
Similar threads
- Question
- Question
- Question
