I am dimensioning a sheet metal part. There are many holes and I am using two edges of the part to locate the first hole, which will be my (0,0) datum. All of the other holes will be dimensioned from this datum using ordinate dimensioning. I am doing this because our sheet metal fabricator can only hold +/- .010 from the edge to the holes, but they can hold +/- .005 between holes. No matter which hole I choose as the datum, there will be other holes located on either side of it. Is it proper to make the ordinate dimensions on one side of the (0,0)datum positive values and the ordinate dimensions on the other side of the datum, negative values, or is it correct to just show all the ordinate dimensions as positive values, no matter which side of the datum they appear on? If there is any documentation on how to do this, please let me know. 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 TugboatEng on being selected by the Eng-Tips community for having the most helpful posts in the forums last week. Way to Go!
Datum dimensioning 2
- Thread starter TJK1
- Start date
-
1
- #2
All dimensions on a drawing should be +ve, regardless of the dimensioning method (polar, coordinate, chain, ordinate, etc.) or direction. There can't physically be a negative distance, can there? Beyond the logic of it, when my former company was corrected on this some time back, there was another ASME standard referenced at the time to confirm this; unfortunately I have no idea which one. Anyone?
Jim Sykes, P.Eng, GDTP-S
Profile Services TecEase, Inc.
Jim Sykes, P.Eng, GDTP-S
Profile Services TecEase, Inc.
TJK1,
Been there, done that.
What CAD package is going to mark the minus signs on your dimensions, and then update correctly when you move the holes?
However logical it is, it is a can of worms. Don't do it.
PEM, and an a couple of other manufacturers, make press-in floating nuts. These are an excellent work-around for sheet metal bending tolerances.
JHG
Been there, done that.
What CAD package is going to mark the minus signs on your dimensions, and then update correctly when you move the holes?
However logical it is, it is a can of worms. Don't do it.
PEM, and an a couple of other manufacturers, make press-in floating nuts. These are an excellent work-around for sheet metal bending tolerances.
JHG
-
1
- #4
PaulJackson
Automotive
TJKI,
It is nieve to establish a coordinate system on any part from a single hole unless all features are coaxial with that feature and rotation of the coordinate system is irrelevant! You have a "sheet metal" part and assuming that means that the "hole depth" is insignificant... you would need a surface feature to serve as the primary datum feature. If you chose a single hole to establish a "(0,0)datum" as you say you would still need a tertiary feature on that part to stop rotation so that coordinate displacements +X+Y, -X+Y, -X-Y, and +X-Y could be determined (not to mention +Z, -Z for the sheet metal surface conditions).
The point is that measurement (reporting the associated +/- displacements) depends upon defining "a coordinate system" A surface (three tangent points), an edge (two tangent points), and another edge (one tangent point)... or a surface, one diameter, and a slot... or a surface (primary) and a pattern of features (secondary and tertiary simultaneously) "as described in your case" are needed to do any repeatable measurement.
Basic dimensions do not need to be specified for their specific coordinate +/- signs on the design specification! If they were it would limit the design to specifying only one coordinate system for measurement... but that is not the case in many designs. Each feature control frame defines its own "coordinate system" and the only "customer relevant information about the measurement results is whether they comply or not with or without probability estimations.
This is not to say that what you propose has not been done... but if you do it "do it right". Function... let me say that again FUNCTION should drive the selection of datum features (Primary, Secondary and Tertiary... as necessary)! Once that is accomplished and there is only one specified DRF that deserves functional recognition and it is consequently soley specified... and detailing complexity warrants that a table of basie dimension values is favorable to detailing conventionally... then illustrate the X+,Y+,Z+ related to the X0,Y0,Z0 thereby defining the origins for translation and rotation of the basic dimentions in the table.
Failing all of those prerequisites and precautions detail the basics conventionally without signs. They describe the theoretical exact form, orientation, and/or location of the feature "AS ILLUSTRATED" on the mechanical specification.
Paul
It is nieve to establish a coordinate system on any part from a single hole unless all features are coaxial with that feature and rotation of the coordinate system is irrelevant! You have a "sheet metal" part and assuming that means that the "hole depth" is insignificant... you would need a surface feature to serve as the primary datum feature. If you chose a single hole to establish a "(0,0)datum" as you say you would still need a tertiary feature on that part to stop rotation so that coordinate displacements +X+Y, -X+Y, -X-Y, and +X-Y could be determined (not to mention +Z, -Z for the sheet metal surface conditions).
The point is that measurement (reporting the associated +/- displacements) depends upon defining "a coordinate system" A surface (three tangent points), an edge (two tangent points), and another edge (one tangent point)... or a surface, one diameter, and a slot... or a surface (primary) and a pattern of features (secondary and tertiary simultaneously) "as described in your case" are needed to do any repeatable measurement.
Basic dimensions do not need to be specified for their specific coordinate +/- signs on the design specification! If they were it would limit the design to specifying only one coordinate system for measurement... but that is not the case in many designs. Each feature control frame defines its own "coordinate system" and the only "customer relevant information about the measurement results is whether they comply or not with or without probability estimations.
This is not to say that what you propose has not been done... but if you do it "do it right". Function... let me say that again FUNCTION should drive the selection of datum features (Primary, Secondary and Tertiary... as necessary)! Once that is accomplished and there is only one specified DRF that deserves functional recognition and it is consequently soley specified... and detailing complexity warrants that a table of basie dimension values is favorable to detailing conventionally... then illustrate the X+,Y+,Z+ related to the X0,Y0,Z0 thereby defining the origins for translation and rotation of the basic dimentions in the table.
Failing all of those prerequisites and precautions detail the basics conventionally without signs. They describe the theoretical exact form, orientation, and/or location of the feature "AS ILLUSTRATED" on the mechanical specification.
Paul
I don't believe the OP is refering to this datum relative to GD&T, but more as an identifier to denote the dimension origins.
When the people fear their government, there is tyranny; when the government fears the people, there is liberty. - [small]Thomas Jefferson [/small]
When the people fear their government, there is tyranny; when the government fears the people, there is liberty. - [small]Thomas Jefferson [/small]
PaulJackson,
I take it you meant "naive"?
I have done the exact thing the OP is talking about. My sheet metal part had flanges on all four sides, each with tolerances of ±.015". I specified the bottom of the panel as Datum[ ]A. I selected one hold as Datum[ ]B. I used one side as Datum[ ]C. Datum[ ]B controls X and Y. Datum[ ]C controls rotation. This meets all the requirements of ASME Y14.5M-1994.
I have tagged datum dimnensions on one side of zero, with netative signs, but was a long time ago, on a drafting board. I did not need to make assumptions about software, and I did not understand GD&T back then.
JHG
I take it you meant "naive"?
I have done the exact thing the OP is talking about. My sheet metal part had flanges on all four sides, each with tolerances of ±.015". I specified the bottom of the panel as Datum[ ]A. I selected one hold as Datum[ ]B. I used one side as Datum[ ]C. Datum[ ]B controls X and Y. Datum[ ]C controls rotation. This meets all the requirements of ASME Y14.5M-1994.
I have tagged datum dimnensions on one side of zero, with netative signs, but was a long time ago, on a drafting board. I did not need to make assumptions about software, and I did not understand GD&T back then.
JHG
PaulJackson
Automotive
Thanks ewh for your comment I guess I didn't read the OP's post with a CAD hat on.
There are so many people that confuse "O-lines" as identifiers of datum features that I have told designers that it is just as correct to put your "O-line" intersection in the corner of the drawing and dimension all features in the first quadrant as it is to place it at the intersection of the most commonly or most important datum feature reference specified. If you are choosing where to put the O-line the best choice is typically at the origin of the most commonly or most important datum feature reference specified. Sometimes on complex design specifications multiple "O-line" designations are used among the various sheets for local system depictions.
I found it interesting when GM and Ford were jointly developing the FWD six speed transmission case structures that GM typically didn’t use O-lines but rather dimensioned all features with leader lines originating from local functional assembly or system DRF’s where Ford typically had O-lines coincident with the manufacturing nest DRF. It was difficult suggesting a common strategy for both companies and getting the designers to buy into it.
Pet-peeves,
... When two dowels are designated as a secondary datum feature pattern put the O-line smack-dab-in-the-center of the pattern equidistant from each dowel feature rather than placing it at the center of one of the pattern features. In function typically that is how a two equivalent clearance round dowel pattern works neither dowels has precedence for locating and orienting to the mating pattern they do it collectively/simultaneously as a pattern. Typically in function both dowels experience equivalent outboard or inboard interference or they have slight clearance resulting in marginal datum shift.
…It is just plain laziness or ignorance when designers snap coordinate dimensions at one end of an angled hole where it intersects with a surface. Inspectors have to figure the rotated axis displacements from the DRF origin, measure the feature location and report the location deviation… but then they often have to convert those measured “rotated axis displacements” back into coordinate deviations consistent with those snapped coordinates at the modeled surface condition just to satisfy reviewers of the measurement data. Designers should take a little more time and detail those displacements correctly so that down streamers don’t have to deal with lousy dimensioning.
Paul
There are so many people that confuse "O-lines" as identifiers of datum features that I have told designers that it is just as correct to put your "O-line" intersection in the corner of the drawing and dimension all features in the first quadrant as it is to place it at the intersection of the most commonly or most important datum feature reference specified. If you are choosing where to put the O-line the best choice is typically at the origin of the most commonly or most important datum feature reference specified. Sometimes on complex design specifications multiple "O-line" designations are used among the various sheets for local system depictions.
I found it interesting when GM and Ford were jointly developing the FWD six speed transmission case structures that GM typically didn’t use O-lines but rather dimensioned all features with leader lines originating from local functional assembly or system DRF’s where Ford typically had O-lines coincident with the manufacturing nest DRF. It was difficult suggesting a common strategy for both companies and getting the designers to buy into it.
Pet-peeves,
... When two dowels are designated as a secondary datum feature pattern put the O-line smack-dab-in-the-center of the pattern equidistant from each dowel feature rather than placing it at the center of one of the pattern features. In function typically that is how a two equivalent clearance round dowel pattern works neither dowels has precedence for locating and orienting to the mating pattern they do it collectively/simultaneously as a pattern. Typically in function both dowels experience equivalent outboard or inboard interference or they have slight clearance resulting in marginal datum shift.
…It is just plain laziness or ignorance when designers snap coordinate dimensions at one end of an angled hole where it intersects with a surface. Inspectors have to figure the rotated axis displacements from the DRF origin, measure the feature location and report the location deviation… but then they often have to convert those measured “rotated axis displacements” back into coordinate deviations consistent with those snapped coordinates at the modeled surface condition just to satisfy reviewers of the measurement data. Designers should take a little more time and detail those displacements correctly so that down streamers don’t have to deal with lousy dimensioning.
Paul
On your dowel point, we've been using hole and slot more since this may achieve better results in some situations. It costs a bit on machining but if you want good location control it gets it done. In this case making the pin that goes in the hold second datum makes sense, doesn't it?
On your angled holes, could you better explain how you believe they should be toleranced, I'm not sure I follow you.
KENAT,
Have you reminded yourself of faq731-376 recently, or taken a look at
On your angled holes, could you better explain how you believe they should be toleranced, I'm not sure I follow you.
KENAT,
Have you reminded yourself of faq731-376 recently, or taken a look at
PaulJackson
Automotive
Kenat,
I put together a little slide to better explain what I meant about the coordinate detailing on angled holes. Please overlook all of the obvious housekeeping mistakes in detailing and dimensioning. It is crude but it shows what I object to... I see this all the time on designs.
Holes and slots are fine being declared secondary and tertiary respectively... and putting a round pin in the slot (or even diamond pin in a tertiary round hole) is common practice. Many precision assemblies however, are (and have been for many years) controlled with two hole dowel patterns. Wheather the pins are solid or compressible "roll pins" the typical tolerances for location and consequential manufacturing and thermal variation result in slight interference fits... but that is expected and acceptable to a degree. By severly limiting or eliminating "shift" and by using both holes to locate and orient simultaneously the pattern moderates location errors in the assembly.
My only point is that when these patterns are used as such as they commonly are (same size pins, same size holes, and same spreads)... don't make one the secondary and the other tertiary... and don't stick the O-line at the center of one. Make the pattern itself secondary and stick the O-line in the center between the two holes.
Inspection should then find the center between the two holes an move origin there for measuring subsequent features toleranced from the pattern "just the way it functions".
Paul
I put together a little slide to better explain what I meant about the coordinate detailing on angled holes. Please overlook all of the obvious housekeeping mistakes in detailing and dimensioning. It is crude but it shows what I object to... I see this all the time on designs.
Holes and slots are fine being declared secondary and tertiary respectively... and putting a round pin in the slot (or even diamond pin in a tertiary round hole) is common practice. Many precision assemblies however, are (and have been for many years) controlled with two hole dowel patterns. Wheather the pins are solid or compressible "roll pins" the typical tolerances for location and consequential manufacturing and thermal variation result in slight interference fits... but that is expected and acceptable to a degree. By severly limiting or eliminating "shift" and by using both holes to locate and orient simultaneously the pattern moderates location errors in the assembly.
My only point is that when these patterns are used as such as they commonly are (same size pins, same size holes, and same spreads)... don't make one the secondary and the other tertiary... and don't stick the O-line at the center of one. Make the pattern itself secondary and stick the O-line in the center between the two holes.
Inspection should then find the center between the two holes an move origin there for measuring subsequent features toleranced from the pattern "just the way it functions".
Paul
PaulJackson
Automotive
Ringster,
Equivalent? Yes. Practical for downstream users of the design? No. That is my point when this is done others have to convert the basics to measure... then because reviewers of the inspection want to see measurement results in the same form as the specified basics... the inspectors have to convert the results back into X,Y,Z coordinates at the modeled surface coordinates "for the position of the hole".
If the profile was added to the first example then the inspectors would have to convert the profile deviation into the X,Y,Z coordinates at the modeled perfect location of the hole.
It is all to confusing. Either you have to convince the quality reviewers that the measured deviations from basic have been converted for measurement and they should just trust the results... or get the designers to but the basics in the same form that they will be measured... I fight for the latter!
Paul
Equivalent? Yes. Practical for downstream users of the design? No. That is my point when this is done others have to convert the basics to measure... then because reviewers of the inspection want to see measurement results in the same form as the specified basics... the inspectors have to convert the results back into X,Y,Z coordinates at the modeled surface coordinates "for the position of the hole".
If the profile was added to the first example then the inspectors would have to convert the profile deviation into the X,Y,Z coordinates at the modeled perfect location of the hole.
It is all to confusing. Either you have to convince the quality reviewers that the measured deviations from basic have been converted for measurement and they should just trust the results... or get the designers to but the basics in the same form that they will be measured... I fight for the latter!
Paul
So effectively you measure from the projected point/line that datum planes A & B meet.
I have to admit that seems awfully like measuring to a corner rather than an edge. I think I see the distinction but I'm still not sure I follow you full argument.
KENAT,
Have you reminded yourself of faq731-376 recently, or taken a look at
I have to admit that seems awfully like measuring to a corner rather than an edge. I think I see the distinction but I'm still not sure I follow you full argument.
KENAT,
Have you reminded yourself of faq731-376 recently, or taken a look at
PaulJackson
Automotive
Kenat,
You have to walk a mile in the inspector's shoes to see this one.
Paul
You have to walk a mile in the inspector's shoes to see this one.
Paul
Well, I suppose that IF ONE had the convenience of knowing with certainty the method to be used for verification, you would have a point. However, Y14.5 as I understand, has managed to avoid getting to preferential inspection techniques. (open setup vs gages vs CMM)
Otherwise I do not see and advantage.
Otherwise I do not see and advantage.
PaulJackson
Automotive
Ringster, There are only five relevant displacements from the Specified Datum Reference Frame for the hole's position. Whether the position is compounded or not there are three relevant rotations and two translational degree of freedom constrained. with one (one translation) remaining unconstrained (position along the axis). For an angled hole at least one of the three rotations must be specified while the others can be assumed parallel or a right angles to the DRF coordinate system if illustrated so.
No matter whether the part is gauged in an open set up or with a CMM or with an attribute gage these parameters must be figured in the process to permit the one unconstrained degree of freedom its liberty! When a designer specifies three translational degrees of freedom... he is stopping translation along the axis to describe the basic dimensions and that information must always be converted to accomplish the inspection! Trust me... It is a pain in the ass for reporting deviations.
Likewise for the profile... five degrees of freedom are constrained (three translational two rotational) with one rotational remaining unconstrained. If designers could think more in terms of degrees-of-freedom that are being constrained by the GD&T callouts that they specify then they could detail the ones that are relevant to the measurement.
Paul
No matter whether the part is gauged in an open set up or with a CMM or with an attribute gage these parameters must be figured in the process to permit the one unconstrained degree of freedom its liberty! When a designer specifies three translational degrees of freedom... he is stopping translation along the axis to describe the basic dimensions and that information must always be converted to accomplish the inspection! Trust me... It is a pain in the ass for reporting deviations.
Likewise for the profile... five degrees of freedom are constrained (three translational two rotational) with one rotational remaining unconstrained. If designers could think more in terms of degrees-of-freedom that are being constrained by the GD&T callouts that they specify then they could detail the ones that are relevant to the measurement.
Paul
PaulJackson
Automotive
Ringster,
I stated that the illustration was crude "2D" and not comprehensive... Isaid forgive me for the dimensioning and detailing faults... consider it without those discrepancies and please consider the scenarios I presented verbally. BTW, I failed to mention that the translational degrees-of-freedom are always oriented to the specified feature location rather than the specified DRF. That should help explain witch ones are constrained or unconstrained.
Paul
I stated that the illustration was crude "2D" and not comprehensive... Isaid forgive me for the dimensioning and detailing faults... consider it without those discrepancies and please consider the scenarios I presented verbally. BTW, I failed to mention that the translational degrees-of-freedom are always oriented to the specified feature location rather than the specified DRF. That should help explain witch ones are constrained or unconstrained.
Paul
PaulJackson
Automotive
I am sorry Ringster,
I didn't answer your last question very well. Let me try again. Consider that A, B, and C are surfaces perpendicular to each other establishing a traditional 3-2-1 DRF. All feature controls that declare that DRF for location must be measured in relation to the origin… (the intersection of the those planes as created by the registry of those features upon the datum feature simulators employed for inspection whether in open layout, in a gage, or simulated from points mathematically on a CMM). Measured features that are nominally parallel or perpendicular will align with one or more of the DRF's axes but those features that are not must be compared to the DRF's origin X0,Y0,Z0 at their specified rotations.
I hope that explanation helps.
Paul
I didn't answer your last question very well. Let me try again. Consider that A, B, and C are surfaces perpendicular to each other establishing a traditional 3-2-1 DRF. All feature controls that declare that DRF for location must be measured in relation to the origin… (the intersection of the those planes as created by the registry of those features upon the datum feature simulators employed for inspection whether in open layout, in a gage, or simulated from points mathematically on a CMM). Measured features that are nominally parallel or perpendicular will align with one or more of the DRF's axes but those features that are not must be compared to the DRF's origin X0,Y0,Z0 at their specified rotations.
I hope that explanation helps.
Paul
- Status
Similar threads
- Question
- Question
