×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Thru hole dimensioning in deep part
15

Thru hole dimensioning in deep part

Thru hole dimensioning in deep part

(OP)
Really need help with this.

I have a cube that is eight inches square.  There are four holes to be drilled through the entire depth of the part and the centerline of the holes are dimensioned only on the top view.  The holes are 1/4" diameter.  There is a drawing tolerance of +/- .010.

The hole pattern dimensioning uses no control boxes, neither does it have any requirement for perpendicularity, celindricity, parrellism, etc.  All that is shown is the distance to the first hole from the part edges and the center-to-center location for the hole pattern.

The part was manufactured by a outside shop. Where the holes exit the part on the "bottom" they do not fall within the drawing tolerance as measured from the edges at the bottom of the cube.

I contend that the drawing does not control the exit hole locations and so our inspection department should not flag this as discrepant.

My question is this:  What controls the exit hole tolerance for thru holes drilled through thick parts when the holes are dimensioned on a drawing only on the "entrance" view of the hole?

RE: Thru hole dimensioning in deep part

Without the benefit of a specific standard, such as Y14.5, there is no clear cut definition of the allowables.

IMHO.

RE: Thru hole dimensioning in deep part

To me, the use of "THRU" would indicate that the entry hole positions and the exit hole positions are required to have the same tolerance.  But as noted above, if there was no use of GD&T, the tolerances are open to interpretation.

A good shop would have drilled 4" and rotated the parts for the other 50%.

"Art without engineering is dreaming; Engineering without art is calculating."

Have you read FAQ731-376: Eng-Tips.com Forum Policies to make the best use of Eng-Tips Forums?

RE: Thru hole dimensioning in deep part

2
The tolerance of its size is for the whole length of the hole.  ASME Y14.5M 2.7.1.1 states "The actual local size of an individual feature at each cross section shall be within the specified tolerance of size."

To fix this, it might be useful to use GeoTol's to actually loosen the specifications.

Matt Lorono
CAD Engineer/ECN Analyst
Silicon Valley, CA
Lorono's SolidWorks Resources
Co-moderator of Solidworks Yahoo! Group
and Mechnical.Engineering Yahoo! Group

RE: Thru hole dimensioning in deep part

  I disagree with that blanket statement Mango. That would be the correct course of action if the holes were for alignment like a coupler or something where 2 coaxial sets of blind holes would have worked, but if the purpose was to run a single .250 shaft all the way through the hole then that method would not work because there would be a mismatch in the middle that would prohibit it.
  The drawing is definitely open to interpretation in the absence of any specified standards. In my opinion, a good shop would have known that a drill bit over 8" long was going to walk and they would have either asked about the importance of the exit hole or they would have taken measures to prevent the hole from walking such as center drilling, then drilling with a jobber length bit, then a standard length, then maybe go back through with the full length drill bit. This shop very well may have done all this but it still didn't work out.

Powerhound, GDTP T-0419
Production Supervisor
Inventor 2008
Mastercam X2
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

RE: Thru hole dimensioning in deep part

If I were actually intending to put a shaft through the hole, and the location at both ends was important, I'd specify the hole location tolerance at both entry and exit, and I'd probably draw the holes with a 'bottle bore'.

Bottle bore:  The central 3/4 or more of the length of the  hole is drawn enlarged, i.e. with a diameter larger than the diameter of either end of the hole, with a tolerance loose enough to allow drilling from both ends with a little mismatch at the intersection.  Actually making a bottle bore is possible, but probably not easy at that size, so I might add a note that gundrilling the entire hole to size would also be acceptable...  and I'd expect most machinists to just use a stock gundrill.


In the extant case, it sounds like you're obligated to buy the parts even if the distal ends of the holes come out of the corners, since you didn't specify otherwise.



Mike Halloran
Pembroke Pines, FL, USA

RE: Thru hole dimensioning in deep part

Being a cube, how do you know which 4 holes are exit holes? :)
Depending what the part is used for and if it mates with others, I would use GD&T (projected tol on the holes or...?)
For a length of eight inches, call out the hole size needed per it's max depth on both sides, another size between the two holes.
I can't say for sure without knowing the part.

Chris
SolidWorks 08 0.0/PDMWorks 08
AutoCAD 06
ctopher's home (updated 10-07-07)
ctopher's blog

RE: Thru hole dimensioning in deep part

(OP)
Thanks to everyone for the quick replies.

It sounds like, as ringman said above, "without the benefit of a specific standard, such as Y14.5, there is no clear cut definition of the allowables." The drawing does not call out any standard.

The drawing is not very old, and came from a well-known entity. Our inspection department flagged the exit holes as non-conforming (though the deviation is minimal even by their interpretation of the design requirements). My position was that the drawing fails to control the exit hole locations (and now I'll add, fails to state any controlling standard), and consequently there is no criteria against which the exit locations can be checked.

This part bolts to another part with a matching threaded hole pattern. I know the "intent" of the designer was that the exit locations match what is shown for the entrance. And I feel confident the part will work as intended, as is. But, whereas this is a technical issue, subject to interpretation, I still must convince inspection that the part conforms to the drawing. The points made here are very helpful. Thanks again for all the help.

RE: Thru hole dimensioning in deep part

I would have to agree with ringman, if their is no callout on the drawing such as "interpret all dimensions and tolerances per asme y14.5m-1994" then you really get what the machinist decides to give you.

Heckler   americanflag
Sr. Mechanical Engineer
SWx 2007 SP 4.0 & Pro/E 2001
      o
  _`\(,_
(_)/ (_)

This post contains no political overtones or undertones for that matter and in no way represents the poster's political agenda.

RE: Thru hole dimensioning in deep part

Carelessness on multiple fronts:
  1. As mentioned, no standard, no perpendicularity, etc.
  2. What manufacturing genius ignored the fact that the holes were so deep as to almost guarantee that the drill would wander?
  3. If exit location is that important, why not spell it out?

batHonesty may be the best policy, but insanity is a better defense.bat
http://www.EsoxRepublic.com-SolidWorks API VB programming help

RE: Thru hole dimensioning in deep part

2
Ringman pretty much covers it, the drawing is effectively incomplete.

If 14.5 were invoked it would be as fcsuper points out.

I don't think rejecting the part can be justified as the drawing is incomplete, unless there is some workmanship standard etc. invoked on the contract somehow.

KENAT, probably the least qualified checker you'll ever meet...

RE: Thru hole dimensioning in deep part

With all due respect to everyone here, I don't think anyone of the respondees has this right.

ANSI 14.5 may not have been specified on the drawing, and whilst ANSI Y14.5 could have been invoked to enable less rigid manufacturing methods, that doesn't mean that the specification for the hole and its location is incomplete.  

Outofsquare tells us the hole was specified as a THRU hole...a THRU hole...in case you haven't got it by now it was specified as a THRU hole.  

That THRU hole (according to the drawing) is to be located a certain distance from two surfaces of the part. The hole location has been measured in reference to the two surfaces of the block and has been found to be out of spec.

RE: Thru hole dimensioning in deep part

Mousetrap,

You are right! The drawing is as it is. The problems only surfaces when one tries to compare the part to it!!! Everyone that must deal with the contract... those that "designed function" engineering, "specified fit" CAD, "measured result" inspection, "predicted conformance" quality, "speculated cost" manufacturer or "expected performance" customer.... trust that apples are being compared to apples. Without constraints on the scrutiny the expected and actual conclusions tend to diverge.

Paul     

RE: Thru hole dimensioning in deep part

Has been located a certain distance from which two surfaces of the part? If not specified, how can it be out of spec?

Chris
SolidWorks 08 0.0/PDMWorks 08
AutoCAD 06
ctopher's home (updated 10-07-07)
ctopher's blog

RE: Thru hole dimensioning in deep part

Hi OutOfSquare

If the hole centres on one face are given and the tol is +/-0.01" then I would expect the entry and exit holes to fall within that.
If the hole needed to be tighter controlled then a squareness or position tol should have been specified from the appropriate face.
The parts should be rejected.
I would however make reference here to the unpractical situation of trying to drill a hole a 1/4" dia through a 8"
block.
From memory a rule of thumb about drilling hole depths is
8*drill dia.
I think that the holes were drilled from both sides which makes it a very difficult job to get the holes to meet without error.

regards

desertfox

RE: Thru hole dimensioning in deep part

Mousetrap,

Do you know of a  standard that imposes the conditions that you state should be applied to the holes?

At one time I worked for a company that had its Standard of Acceptable Workmanship, which I think would have covered the hole positioning, even before Y14.5.  But without some applicable standard, I think there is a definite problem.

RE: Thru hole dimensioning in deep part

  I see your point mousetrap, you are saying that the use of the word "THRU" makes the hole a 3D object instead of the 2D object shown on the print, and thus the tolerance applies to the entire object, top to bottom. The problem is that it is still an "interpretation" with nothing but good reasoning backing it up. What is good reasoning to you and me may not be good reasoning to others. Simply stating ASME Y14.5M-1994 on the drawing would have invoked the fundamental rules of GD&T and we wouldn't even be having this discussion.

Powerhound, GDTP T-0419
Production Supervisor
Inventor 2008
Mastercam X2
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

RE: Thru hole dimensioning in deep part

I agree with DesertFox on this one. I would check the holes on both sides for the coordinate tolerance shown but would not check to see if the holes were straight, size and location only.

Using the word "THRU" may be more precise but if I did not see a depth of the holes somewhere, I would assume it would be thru.

Stating on the drawing "complies with ASME Y14.5M-94" does mean that GD&T rules apply including rule #1 but how many out there in industry really know the rules. There are only about 300 - 400 ASME GD&T Professional - Seniors and a similar number of Technologist and we still argue (discuss) GD&T in this forum.  

Dave D.
www.qmsi.ca

RE: Thru hole dimensioning in deep part

(OP)
My question was not whether it's practical to drill a 1/4" hole, 8.00 deep, to +/-.010, or whether feature control frames, positional tolerances and datums would make for a better design.

My real world question was: Using the drawing described, what's the permissible deviation for exit hole locations and how is this determined from a technical perspective? What I was looking for is, what STANDARDS can be relied upon in making any determination about how the part may be built? As pointed out above, the question begs another question: Deviation from what?

I appreciate Mousetrap's contrary argument because it forced me to re-evaluate my position. I needed some way to demonstrate the lack of enforceability of the "assumption standard". This has given me even greater confidence in my original conclusion.

Using Mousetrap's argument, the strictest interpretation is that: "The part is presumed symmetrical, and every feature must fall within +/-.010 of every other feature (point, edge or surface)."

Another, equally valid interpretation howerver is that: "The stated tolerance applies to every dimensioned feature through the thickness of the part relative to the respective feature's reference point, edge or surface (datum)."

The design has three views: Top, Side 1, and Side 2. Overall dimensions are shown on all three views. The design width, height and depth is 8.000. Hole locations are shown only on the Top View and are referenced from only the "sides" or "edges" (depending on interpretation). Drawing tolerance is +/-.010, with no angular tolerance given.

Let's look at this part from the side view. In this instance, the top surface is "Datum A". The right-most top edge (TE) is "Datum B". The dimension to the centerline of the first hole is 2.500 from Datum B. Distance to the second hole is 3.000 from the first hole. (right or wrong, it's the way it's drawn.)

Here's one way the part could be built (measurements shown represent possible tolerance extremes):


TE

|<------------------8.000----------------->[B]

|<--2.480-->|<---3.010--->|<--2.510-->|
 __________________________________ ___TOP___
|\               /|                   /|                /|\           [A]  

|<------------7.990~8.010------------>[B][B][B]


(TE = Top Edge opposite Datum B. The solid horizontal line represents the top surface which is Datum A. The vertical and angled lines represent sides and hole centerline locations. At the bottom, shown are three possible locations for Datum B. The opening at the bottom of the triangles each represent .010.)

The sides may be out-of-square, relative to "Datum A," top-to-bottom, by +/-.010.  Right?

From Datum B, the centerline of the first hole has +/-.010, left-to-right, and +/-.010, top-to-bottom. If Datum B slanted out at the bottom and the first hole slanted away from Datum B, this first hole could be up to .020 greater from its nearest bottom edge than it is at the top.

The next hole likewise has +/-.010, measured from the first hole, and also +/-.010, top-to-bottom (through the part).

The exit hole on the bottom left could be as much as .050 closer to its nearest edge than is the first hole from Datum B!

Some seem to want to argue that the right-most surface is the reference surface for the hole pattern, in which case it would effectively be "Datum A". If this is "Datum A", then how about the hole at the top-left which is .020 closer to its nearest edge. Out of tolerance? Would the part have to be made .010 smaller in order to hold both the overall AND hole-to-side tolerances?

What if the part tapers out on both sides at the bottom by .005, to 8.010. The overall dimension would be in tolerance, but you'd effectively reduce the exit hole tolerance to ".005" (I think I figured that right) relative to the two sides -- contrary to the stated tolerance!

If I'm seeing this wrong I'm still open to constructive, technical opinions, backed up with some empirical standard beyond assumptions.

;)

RE: Thru hole dimensioning in deep part

(OP)
In the third from last paragraph, I should have asked, would the part have to be made .010 larger in order to make the second hole fall within tolerance.  And to reiterate, the drawings sets out no standard.

:)

RE: Thru hole dimensioning in deep part

Ootofsquare

Again, I believe tthat without SOME STANDARD being stated in the documentation package, NONE will be applicable.

RE: Thru hole dimensioning in deep part

Even if a standard was stated (as it should be on all drawings), you cannot assume perpendicularity for any hole axis.

According to ASME Y14.5, a feature control frame "True Postion" tolerance, when applied to to a cylindrical feature, correctly controls what some would expect in the situation, a perpendicualr hole.  IT defines not only the starting point of the feature, it also adds feature axis control. [ASME Y14.5M-1994 Section 5.2]

Since the drawing is incomplete (and therefore technically incorrect), arguements for both sides in the case, because of the ambiguity, are allowed to happen.

Remember...
       "If you don't use your head,            idea
                   your going to have to use your feet."

RE: Thru hole dimensioning in deep part

Mousetrap, ringman is correct, if you don't either reference a standard or explicitly explain on the drawing then it's ambiguous.

Most people will more or less interpret a drawing based on whatever standards or conventions they are used to if it doesn't explicitly state one.  However, this doesn't make it correct to do so.

The drawing is ambiguous, while I'd expect it to mean what you say it means it's not explicit.

KENAT, probably the least qualified checker you'll ever meet...

RE: Thru hole dimensioning in deep part

meintsi, your statement is correct, but it doesn't really seem apply to Outofsquare's question (as I understand it) in the way you've stated.  I agree that if perpendicularity is not called out, then it is not assumed.  However, if the dimension is placed on that hole, that dimension stands for the whole feature, per ASME.

With no standard applied, he still has a tough sell because the drawing still communicates a specification.  I actually would suggest the drawing is complete per the design intent, and the parts are out of spec because the dimension is understand by itself without the existance of a standard.  It is a specification as to what is desired, regardless of how unrealistic that specification is.  To say that no standard means no interpretation is silly.  It's like saying we need state Webster Dictionary as our standard each and every time before we speak.

With that said, I would suggest the drawing is updated to state the ASME standard in order to apply GeoTols to that feature to allow for the variation they are observing in the part. (GeoTols are much more complex and even with a standard are open to interpretation, but contrast a simple dimension is common enough to be understood even by people outside the industry.)

Matt Lorono
CAD Engineer/ECN Analyst
Silicon Valley, CA
Lorono's SolidWorks Resources
Co-moderator of Solidworks Yahoo! Group
and Mechnical.Engineering Yahoo! Group

RE: Thru hole dimensioning in deep part

5
No stated standard? Then the only thing that controls the "exit" hole (or entrance hole for that matter) is the the dimensions on the drawing that pertain to that feature, i.e. the size tolerance and the x-y tolerances of the hole located from the edges of the part. If you find that the "exit" hole is within the acceptable maximum stacked tolerance of those dimensions, then the part meets the drawing. If not, then it doesn't meet the drawing.

Whether that was the intent of the person who drew the drawing or not, is a different story. If it doesn't meet function--tough--he/she should've defined it better.

V

Mechanical Engineer
"When I am working on a problem, I do not think of beauty, but when I've finished, if the solution is not beautiful, I know it is wrong."

- R. Buckminster Fuller

RE: Thru hole dimensioning in deep part

Without a standard stated, why do we assume that the dimension & tolerance apply all through the hole/to both entry & exit?

Now as I've hinted before, I'd make that assumption because that's what the standard I normally work to says, but if it came to court of law type situation I wouldn't put any money on it.

KENAT, probably the least qualified checker you'll ever meet...

RE: Thru hole dimensioning in deep part

Ignoring all the tolerancing chatter and thinking from a manufacturing point of view, have you looked into gun drilling the holes?

RE: Thru hole dimensioning in deep part

I believe the part has been fabricated.  the original question pertained to the inspection with regards to the dimensioning method on the drawing.  MOST CERTAINLY, IMPROVEMENTS CAN AND SHOULD BE MADE ON THE DOCUMENTATION.  But the problem remains on what to do with the existing part and how to inspect.  

RE: Thru hole dimensioning in deep part


There is no implied relationship between features in any standard.  In addition, no standard puts a numerical valve on any allowance or tolerance. The standards only communicate the methods required to depict design intent.  

It is when people fully understand that since there is no implied relationship between features that the need for additional geometric control becomes clear.

A diameter dimension shown on one surface is a "feature of size" and does not dictate how that feature is "drilled thru" in relationship to the block.  Only that at every individual cross-section, it is within a defined limit of size.

In practicality, industry has found that a relaxation of the strict enforcement of the Taylor Principle (ASME Y14.5 Rule#1) is left to the discretion of inspection of alternate quality function.  A micrometer check will not verify the perfect form at MMC.

KENAT hit this point above, because of the standards one is used to working with, people will make assumptions based upon them (see vc66's post), but as this drawing is described by the asker, it would still be IMHO technically made to print.

This could be one example of why the standards were written in the first place.  To give people the tools to clearly define design intent.

Remember...
       "If you don't use your head,            idea
                   your going to have to use your feet."

RE: Thru hole dimensioning in deep part

So meintsi, what you're saying is that the hole size, and dimensions from the edges need to be defined on the drawing, at each singular cross-section through the entire hole if there is no standard?

I think that people rely too much on the letter of the law. Relying on there having been no drawing standard, to get you out of making a bad part, is asinine. Although I agree that standards are necessary to guide people, as a person who had worked in a machine shop before I got my degree, I can honestly say that any machinist who looks at a drawing with deep thru holes, and only measures on one side of the cube to check size and distance from the edges, is a careless machinist.

Neither the drawing creator nor the machinist are without fault, here. The drawing should've been defined better, and the machinist should've had the common sense to realize that the drawing was vague before making the part. In the end, common sense is just as important as drawing standards.  

Keep in mind, this is all my two cents, and I don't mean to offend anyone.

V

Mechanical Engineer
"When I am working on a problem, I do not think of beauty, but when I've finished, if the solution is not beautiful, I know it is wrong."

- R. Buckminster Fuller

RE: Thru hole dimensioning in deep part

I obviously agree with vc66.  I actually think Out0fSquare is actually trying to claim the drawing says something which is does not.  The drawing is clear based on what Out0fSquare has stated.  The hole must fall within the stated spec.  What Out0fSquare is adding to the drawing is "this dimension only applies to the entry side of the hole".  But the drawing itself doesn't say that.  It only says "This thru hole is to be such and such distance from the edge" by having the dim.  There's nothing implied.  It is an absolute specification that even has a tolerance to its location.  

The only open question for incoming inspection is how to determine the edge and hole hole surfaces, and how to measure there relationship.  The only variable is in the measurement process itself, not in the specification.

Matt Lorono
CAD Engineer/ECN Analyst
Silicon Valley, CA
Lorono's SolidWorks Resources
Co-moderator of Solidworks Yahoo! Group
and Mechnical.Engineering Yahoo! Group

RE: Thru hole dimensioning in deep part

As dimensioned, I would interpret is based on the tolerance information given.  The entry points are defined, the axes direction is defined.  If the entry points are correctly located and the axis is normal to the entry face within the angular tolerance (if there is one), then the part should pass regardless of the exit locations, even if functionally it is not a good part.

RE: Thru hole dimensioning in deep part

ewh, I think you are adding specification that isn't on the drawing by mentioning axes of direction.  The specification actually has nothing to do with the surface upon which the hole starts, only the dimension from the edge surface to the center of the hole.  .

Matt Lorono
CAD Engineer/ECN Analyst
Silicon Valley, CA
Lorono's SolidWorks Resources
Co-moderator of Solidworks Yahoo! Group
and Mechnical.Engineering Yahoo! Group

RE: Thru hole dimensioning in deep part

I agree that the axes have nothing to do with the start surface, other than both are defined by the view orientation.  They ARE defined as being normal to the view, however, or the feature would not be circular, but elliptical.  This is not per a specification, but simple geometry.

RE: Thru hole dimensioning in deep part

ewh, I understand what you are saying, but let me play devil's advocate. Say that we have the cube in question, and there is NO difference at all between any of the faces, and all the holes are drilled directly in the center of the faces of the cube. Now, I hope you'll agree that there are no "entry" and "exit" holes, here. What I may consider an exit hole, you may consider an entry hole. So, if the drill wanders from the "entry" point during machining, and you inspect it, it's good, because your choice of entry hole happens to be correct, but directly on the other side of the cube, I measure, and whaddya know? it's out of spec. This is why I would measure both sides, because I have no idea which side is which. If either side is out of tolerance, I assume that this is the "entry" side, and it's out of spec.

This is safe inspection. If this is a life saving device, and I just measure one of those sides, and that distance from the edge is critical to function, then it's better to be on the safe side and reject it, until I'm told it's OK by the design engineer, who couldn't be bothered stating a standard and calling out straightness and perpendicularity.

I obviously realize that a life saving device would be better-engineered, but you understand my point.

V

Mechanical Engineer
"When I am working on a problem, I do not think of beauty, but when I've finished, if the solution is not beautiful, I know it is wrong."

- R. Buckminster Fuller

RE: Thru hole dimensioning in deep part

However, arguably the drawing only shows the holes to meet that tolerance/dimension on where they break one surface.  If you measure it and it meets spec on one surface it's good right?

That's pretty much the root of the argument isn't it.

KENAT, probably the least qualified checker you'll ever meet...

RE: Thru hole dimensioning in deep part

ewh, in addition, as meintsi stated above, "there is no implied relationship between features in any standard."  The have a tolerance you mentioned would require a GeoTol to establish the relationship between entry surface and the hole.  With a datum and a control frame, their is no specification for such.  A relationship cannot be assumed, even on a drawing view that is square to the part.  The drawing view by its own right is no a specification, nor does it have tolerance to its orientation.

If ASME was mentioned on the drawing, 90deg angle is assumed for all unspecified angles.  But if ASME is mention, this is actually a moot point because of paragraph 2.7.1.1, sited above.  BTW, this is where meintsi's statement is wrong.  ASME Y14.5M does imply a 90deg angle for unspecified angles.  

Matt Lorono
CAD Engineer/ECN Analyst
Silicon Valley, CA
Lorono's SolidWorks Resources
Co-moderator of Solidworks Yahoo! Group
and Mechnical.Engineering Yahoo! Group

RE: Thru hole dimensioning in deep part

Exactly, KENAT. In my example, which surface is that? If everything is literally symmetrical, how do we know which surface corresponds to the one on the drawing with the dimension?

Hence, I would check them all to be safe.  

V

Mechanical Engineer
"When I am working on a problem, I do not think of beauty, but when I've finished, if the solution is not beautiful, I know it is wrong."

- R. Buckminster Fuller

RE: Thru hole dimensioning in deep part

KENAT,  the surface of exit and entry are not part of the specification that Out0fSquare stated.  As stated above, such a relationship could only be establish with GeoTols.  The dimension as stated would be required the hole to be at the distance specified for infinity.  The entry and exit cross sections are no different from each other or from any other cross section when it comes to whether or not the hole falls within the specification stated.  

Matt Lorono
CAD Engineer/ECN Analyst
Silicon Valley, CA
Lorono's SolidWorks Resources
Co-moderator of Solidworks Yahoo! Group
and Mechnical.Engineering Yahoo! Group

RE: Thru hole dimensioning in deep part

My point is that if you measure it on one surface and that surface passes then the part is good isn't it?  It meets the drawings requirements.

Even if you measure one side and it fails, then you measure the other side and it passes then the part still meets the drawings..

In this case if you only have to find one 'corner' where it meets drawing requirements and arguably it's ok.  So you have 8 chances!

This is really taking it to extremes but ...

KENAT, probably the least qualified checker you'll ever meet...

RE: Thru hole dimensioning in deep part

KENAT, I don't think this could be considered correct.  It is implying a specification that isn't on the drawing, being "Dimension only needs to apply at one point."  Without this statement on the drawing, if any point of the hole can be found to be out of the stated spec, then the hole is out of spec.  The argument really doesn't work the other way around, as you've stated.  If any point is found to be in fault, then there is a fault.  Without a statement saying to ignore those faults, there is a failure to meet the spec.

Matt Lorono
CAD Engineer/ECN Analyst
Silicon Valley, CA
Lorono's SolidWorks Resources
Co-moderator of Solidworks Yahoo! Group
and Mechnical.Engineering Yahoo! Group

RE: Thru hole dimensioning in deep part

If you checked both sides to be safe, how can you justify rejecting it when only one side is off?  Turn the other side and the part still meets the drawing.

If there is a tolerance block on the drawing that covers angular tolerance, it would apply to ALL angles on the drawing (unless otherwise specified), including "assumed" 90's.  Otherwise, there is NO way to control the shape.

In a front view of a drawing of a cube, we "assume" that the sides are vertical and the top and bottom are horizontal.  We assign the angular tolerance to this, as it is "assumed" to be 90 degrees, and because no part can ever be perfect.  If we did not assume this, the part could be a trapezoid with parallel 15 degree sides and still meet the drawing.
These are based on general drafting practices, not necesarily an approved standard.

RE: Thru hole dimensioning in deep part

I can justify it using exactly what fcsuper just stated. It only takes one fault on a feature to reject it, the opposite (it only takes one good part of a feature full of faults to accept it) is not true.

I agree with your second statement, ewh, but I don't understand what you're trying to say? By your logic, the assumed angle is 90°, even for a hole, and therefore if one side is not parallel to another, it's out of spec, no? So why is it that a hole assumed to be in one spot on one side of a cube that's not in the same spot (or at least within dimensional x-y tolerance) on the opposite side, is not wrong?

V

Mechanical Engineer
"When I am working on a problem, I do not think of beauty, but when I've finished, if the solution is not beautiful, I know it is wrong."

- R. Buckminster Fuller

RE: Thru hole dimensioning in deep part

I'm lost now with who's agreeing with what.

Back to the OP, common practice would probably suggest that the inspection department is correct and the part should be rejected.

However, what is invoking that common practice, why should it be applied?

The drawing is ambiguous, so before accepting or rejecting the part the person/organization responsible for the part should probably be asked for clarification.

KENAT, probably the least qualified checker you'll ever meet...

RE: Thru hole dimensioning in deep part

Out of Square

Can you give us some clues as to the functioning of this part?  Does it have chances of becoming a piece of space equimment or flight hardware for starters?

Strange that an Aerospace company in the year of 2007 would not impose some standards on its drawing definitions.

RE: Thru hole dimensioning in deep part

I'm with you, KENAT. I just looked back at the posts, and I have no idea what's going on. I actually think I contradicted myself two or three times.

V

Mechanical Engineer
"When I am working on a problem, I do not think of beauty, but when I've finished, if the solution is not beautiful, I know it is wrong."

- R. Buckminster Fuller

RE: Thru hole dimensioning in deep part

fcsuper slipped that in while I was typing winky smile

As to my second statement, it is because NO feature is perfect, and there has to be an allowance for those imperfections.  The sides will never be perfectly parallel to each other.  If one side is not parallel to the other WITHIN THE BLOCK TOLERANCE, it is to be rejected.
You are starting to make me reconsider some though... any variation from "perfect" sides should be accounted for in the dimensioning of the holes, but then who's to decide what variation is acceptable if we don't apply the block tolerances?

This is turning into a more philisophical discussion about drafting in general, and I have to agree with KENAT, as to the original post, the drawing is incomplete, and the part can only be made using assumptions.

RE: Thru hole dimensioning in deep part

No offence being taken vc ...  and no I was not implying that at all. A diameter dimension is single feature dependent.  At any particular point it is checked, standard or not, it must fall within the defined limits of size.

As far as the implied 90° angle (2.1.1.2), the way I understand the convention it is that I would agree with you only if the hole was depicted in both side views with centerlines depicted.  After rereading it again, I don't think that a centermark alone on the top surface is enough to invoke the Y14.5 implied 90° angle.  But it is interesting that even if this did apply, with general title block angle tolerancing usually at ±1°, over 8" this translates to ±.140" at exit.

I love the letter of the law comment, and I totally agree with you (I spent two years in a machine shop also).  Possibly, the vendor would remake the part if rejected without question, but if not, he could make a very strong case about this part being made to print.

Oh, and yes, OutOfSquare, COMPLETE the print.

Remember...
       "If you don't use your head,            idea
                   your going to have to use your feet."

RE: Thru hole dimensioning in deep part

meintsi,
The centermark should be enough to imply 90, whether per the standard or not.  When you get down to spitting hairs, don't we assume that the drawing views are 90 degree projections?  Why?  There is no standard stated.  Is it first or third angle projection?
I agree, get them to fix the drawing and let QA and the vendor sort this one out.

















RE: Thru hole dimensioning in deep part

(OP)
This is a real print, and real part. The part was machined by an outside vendor. It's goes on a test fixture, not flight hardware.

There's one threaded hole on top, near one edge which distinguishes top from bottom and gives the part an orientation.

On the drawing all features appear square, perpendicular, parallel, circular and symmetrical, (except for the threaded hole on the top).

Inspection has flagged some of the exit hole locations as "out of tolerance". This was checked by laying the part on it's side and measuring from the test surface up to the centers.

I'm responsible for responding to a Corrective Action Report, stating why the "error" occurred, and what action will be taken. My outside vendor is willing to correct any discrepancies, but I need to tell him what's discrepant.

Here's where I have a problem with this test. The test, as administered, ASSUMES that the drawing imposes parallelism between the thru holes and a side. Why was this assumed? Answer: Because it "looks" parallel on the drawing, and, that's they way they always do it.

Why then, isn't every possible positional and feature-control imposed on every feature, uniformly, checked against every other feature? (This is a rhetorical question of course.)

Consider this: On the "high side" the cube could be (8.010). The first hole could be on the low side at 2.490, and the second hole at 2.990 (or, 5.480 to the CL of the second hole from the referenced edge). This leaves 2.530, if measured from the second hole to the far side. That's .020 greater than the drawing tolerance. And yet, all of the features are within tolerance with respect to the dimensions shown on the drawing, checked only at the locations shown. These features are all drawn symmetrical. However, they weren't checked for symmetry. When asked why, the answer was that it's because there's no dimension shown on the drawing between the second hole and the far side so it doesn't have to be checked!

How about Perpendicularity? Let's call the "right side," Datum A". The top is "Datum B." (It's not that way on the drawing, this is for discussion only.) What would be the tolerance zone for perpendicularity between B and A? Since no angularity tolerance is given, we could argue: "Datum B must be perpendicular to Datum A, to within +/-.010, measured at the far corner opposite the intersection of A and B." (Picture an "L" with equal legs and the intersection being the pivot point.)

Now, assume that the intent was for the holes to be perpendicular to Datum B (the top surface), without regard to the sides. Using simple geometry, the exit holes will rotate along with Datum B, the same amount as Datum B rotates around its intersection with A. (Picture an "E" with the bottom line as Datum A, the vertical line as Datumm B, and the other two upper lines as hole centerlines with the open side being the "exit" side.) Using the drawing tolerance +/-.010, the exit hole locations could deviate by +.010, or -.010 on the exit surface due to angularity differences between A and B. Add to this the positional tolerance for the hole, and you have an exit hole tolerance of +/-.030. (This is one argument that can be made.)

I've concluded that, absent any expressed standard, checking ANY feature -- other than those explicitly dimensioned, at the  points indicated -- necessitates that subjective and arbitrary assumptions must be made.

In the immediate case, (and similar cases) the options appear to be three (generally stated). We can either: [1] Check ONLY the features dimensioned, only at the points shown; or, [2] Assume we know what the designer intended and impose any combination of control constraints we think appropriate; or, [3] Apply the drawing tolerance to every feature relative to every other feature, measured from every point, edge and surface, in which case the tolerance for some features will unnecessarily be reduced in order for other features to remain in tolerance.

It appears that Option "1" is the only one that would likely "hold up on court" so to speak. All others require varying degrees of assumptions and subjective speculation, in which case there's a high degree of probability that designers, buyers, estimators, machinists, and inspectors will never agree on issues such as this without some controlling standard.

RE: Thru hole dimensioning in deep part

"The test, as administered, ASSUMES that the drawing imposes parallelism between the thru holes and a side. Why was this assumed? Answer: Because it "looks" parallel on the drawing, and, that's they way they always do it."

I disagree with this wholeheartedly.  From what you described, there are no assumptions.  The dimensions established a relationship between the center of the hole and the part edge, period.  Without further modifying notes, this is absolute to infinity.  The start and ending cross sections are not part of the specificaion, only the distance between the center of the hole and the edge (and center of the center to the center of the next hole).

My arguement here is that the spec on your drawing is too tight, not that it's not saying anything at all.  I believe you should use GeoTols to loosen the tolerance.


"How about Perpendicularity?"  

Perpendicularity is not assumed from what you described.  Again, there is no relationship between the holes and their starting and ending cross sections.

"[1] Check ONLY the features dimensioned, only at the points shown;" and "It appears that Option "1" is the only one that would likely "hold up on court" so to speak. All others require varying degrees of assumptions and subjective speculation..."

Again, I wholeheartedly disagree.  Option 1 is the most assumptive of the options you believe you have.  It does the most to add specification to the drawing that the drawing itself does not state.  But you are free to your own opinion and you must choose the course best for you in this matter.

Matt Lorono
CAD Engineer/ECN Analyst
Silicon Valley, CA
Lorono's SolidWorks Resources
Co-moderator of Solidworks Yahoo! Group
and Mechnical.Engineering Yahoo! Group

RE: Thru hole dimensioning in deep part

Without a spec or some convention invoked even the principle of measuring from the surface is in doubt.

The drawing shows the dimension to the top edge, measuring from that may get a different result than from measuring to plane created by the 3 highpoints on the surface.

Is there an option 4, ask for clarification from the design authority?

KENAT, probably the least qualified checker you'll ever meet...

RE: Thru hole dimensioning in deep part

(OP)
"The dimensions established a relationship between the center of the hole and the part edge, period."  Is that in the Bible or something?

RE: Thru hole dimensioning in deep part

There may be an opportunity here.

If you approach the vendor with something like, "I didn't do a great job of conveying the design intent; but now that we all understand it, let's work together to prevent a recurrence.  For example, tell me what sort of flag/ callout/ note on the drawing would have told you that the hole had to be real straight?".  In which case, you will end up with a drawing that at least one vendor won't misinterpret ever again.

And in the spirit of cooperation, I'll bet that vendor could bush and redrill the offending pieces so the repair would be detectable only with difficulty.  Design constraints permitting, of course.

Mike Halloran
Pembroke Pines, FL, USA

RE: Thru hole dimensioning in deep part

(OP)
Personally, I think I were going to apply the "because that's the way I do it" standard, the hole pattern SHOULD be the controlling feature, with some perpendicularity constraint with regard to the mating surface.

If we were to apply the "common sense" rule, or "common practice" rule, on this particular part it would appear that, since nothing mates to the sides -- and since the distance to the sides has NO IMPACT on whether or not the THRU HOLES will match up with the matching threaded holes to which the part attaches -- the distance from the hole pattern to the sides should be of minor concern.  That's why I think discussion of the assumed "parallelism" requirement with regard to the relationship to the holes relative to the sides is without merrit.

I believe that the part may be accepted as built.  Or, the holes could possibly be counter-bored to open up the clearance (they are, after all, clearance holes with no particular "fit" with regard to the fastener). No determination has yet been made by the customer.

RE: Thru hole dimensioning in deep part

(OP)
The drawing was provided by the customer.

RE: Thru hole dimensioning in deep part

So can you ask the customer for clarification then as the design authority.

If nothing else you could say something like 'we weren't sure whether to manufacture/inspect against ASME Y14.5 or the isos, could you tell us what spec applies'?

Whichever one they invoke it should clarify.

KENAT, probably the least qualified checker you'll ever meet...

RE: Thru hole dimensioning in deep part

(OP)
Yes, I could ask for clarification. But the part has already been made. And, it was made under sub-contract to a third-party shop. I can't very well now go to them and ask that they re-make the part in accordance with some "new" standard! Fortunately, the order was for only one and not five-hundred! Nevertheless, it's made from some rather expensive, somewhat exotic material, and so we really need to make this one work. Hopefully, the part can be used as built, or perhaps we can open up the "far-side" holes with a counter-bore.

RE: Thru hole dimensioning in deep part

Maybe another way to help save the piece is to open up the tolerances on the dimensions locating the hole pattern...say from +/-.010 to +/-.06 as OutofSquare stated the sides don't mate with anything and then maybe the holes could possibly be counter-bored to open up clearance for the fasteners if the holes are not satisfactory in their present condition.

RE: Thru hole dimensioning in deep part

(OP)
fcsuper, said, "The dimensions established a relationship between the center of the hole and the part edge, period."

Your position is precisely the one for which I'm asking for some supporting evidence. You seem to be equating "center point" with "center axis". And that "edge" equates with "surface". I disagree. What says that "point=axis" and "edge=surface".  I see this could truly cause a great deal of dead parts.

Also, using your own "standard", why are you giving me .030, more tolerance from the second hole to the bottom far side, but holding me to .010, on the near side? These sides and hole relationships are drawn perfectly symmetrical. But you didn't say the part has to be symmetrical. Why not?

What if the part made to these dimensions, it's 7.995 across the top, and 8.005 across the bottom [+.010 wider on bottom than top]. The first hole is at low tolerance from the dimensioned "side" [-.010], and next hole is also at its low tolerance [-.010], and make the top "out-of-square" to this side (obtuse) such that it measures an additional +.010, at the far corner. (The part is out of square, side-to-top within tolerance, and the opposing sides are out-of-parallel, side to side, but within tolerance.) All dimensioned features are in tolerance (according to your interpretation), and we've imposed the drawing tolerance to the exit hole centers relative to their dimensioned side, and yet the second hole exits the part .040 further from its nearest corner than does the similar hole that's being checked. Why are you allowing an additional .030 on the far side when these holes are drawn symmetrical in all views?

RE: Thru hole dimensioning in deep part

If only one part is involved, why not functionally check it on its related test fixture?  Is that a possibility?

RE: Thru hole dimensioning in deep part

OurOfSquare said, "What says that "point=axis" and "edge=surface"."

If you have a hole in a part, and you mark the face of that hole with a centermark--it represents and infinite straight line through that cylinder, the axis. It can't be anything else. Any person who looked at the drawing and was asked what that cross represented would say, "that's the center axis of that hole."

As for the edge = surface--If you're measuring from your "edge" and you don't consider that part of the surface, you're going to have a hell of a time trying to measure from and infinitely thin line to an imaginary point which only exist on that face of your part. That's why there are assumptions made, WAY before standards are enforced. Using your logic, normal inspection would be impossible without a CMM.

V

Mechanical Engineer
"When I am working on a problem, I do not think of beauty, but when I've finished, if the solution is not beautiful, I know it is wrong."

- R. Buckminster Fuller

RE: Thru hole dimensioning in deep part

You can't be absolute about these things.  A center point may be locating a hole at an angle.

The edge may be a part of the surface, but it does not indicate whether that surface is out of plane.  A dimension from the edge is not necessarily the same as the distance from the surface from which the edge came.  It can't be less, but it can be greater.

RE: Thru hole dimensioning in deep part

Quote (vcc66):

If you have a hole in a part, and you mark the face of that hole with a centermark--it represents and infinite straight line through that cylinder, the axis. It can't be anything else.

True but not complete, a centermark is a point locational reference only.  It defines the point where the axis and the plane the centenline rests upon intersect.

As ewh's example shows, centermarks are commonly used to locate entry points for angled holes.

Remember...
       "If you don't use your head,            idea
                   your going to have to use your feet."

RE: Thru hole dimensioning in deep part

Sorry, you're both correct, I should've clarified that I'm speaking to the situation where the hole is shown "perpendicular" to the face in which it is drilled and a 90° angle is implied.

V

Mechanical Engineer
"When I am working on a problem, I do not think of beauty, but when I've finished, if the solution is not beautiful, I know it is wrong."

- R. Buckminster Fuller

RE: Thru hole dimensioning in deep part

Given Outofsquare's intensity, I'll state that this is my opinion based on not seeing the drawing.

First, I would disgree with 90deg being implied because no standard is stated on the drawing which establishes this rule.  

OutofSquare, to answer your question directly: The dimension as stated on the drawing makes no differentiation between any of the cross sections of the hole.  To say one cross section has more value than any other is to say something that isn't on the drawing: it is an assumption.

Further, even if 90deg is implied (which it is not because no standard is stated which says this) that doesn't mean the hole is created to that specification.  The only specification is between the edge and the centermark or between centermarks (per what you described).  Given the fact there are no cross sectional preferences on the drawing, this would apply to all cross sections of those features.  Where the edge surface deviates from 90deg, so would the hole have to in the same fashion.  

Further, it is an assumption to state the view itself is 90deg to the surface being viewed.  This is assuming a specification which is not on the drawing, even if ASME Y14.5M is employed.  There is no such thing as tolerancing to drawing views themselves.  In my mind, the only way to establish an unassumed relationship between the entry surface and the surface of the hole across its many cross sections is to use feature control frames and datums.

You can argue this out all you want.  In the end, you need to do what is right for you.  If I was in your shoes (which I am not :)), I would say (given your description of everything) "Accept parts as is because specification is unnecessarily restrictive.  Part will work as is.  Action item is to work with the customer to fix drawing to better reflect the functional requirements of the part."  This doesn't give my vendor ammo to use on me in the future, I accept the part that I know will work as is, and I fix the problem for the future.

Good luck with your situation.  In fact, I hope you've already resolved it in whatever way works best for you, and that this discussion is academic for you at this point.  

Matt Lorono
CAD Engineer/ECN Analyst
Silicon Valley, CA
Lorono's SolidWorks Resources
Co-moderator of Solidworks Yahoo! Group
and Mechnical.Engineering Yahoo! Group

RE: Thru hole dimensioning in deep part

Surely if you have a drawing of a cube with three orthographic views, it is safe to ASSUME that the sides are an implied ninety degrees from each other, with or without a stated standard.  If not, how do you proceed?

RE: Thru hole dimensioning in deep part

To assume makes an ass out of you and me.

The drawing is incomplete/ambiguous.

When quoting the job either ask for clarification or give your price and state that you're assuming standard drawing conventions per the relevant standard are in place.  (I realize it's too late for the OP)

I used to prepare quotes (not for machined jobs specifically) and it always amazed me the stuff that wasn't explicitly stated in the document pack we were tendering to.  I'd either ask for clarification or make sure any assumptions I'd made were stated on the cover letter to our quote.

Of course this takes time which from other posts it seems people prepparing bids for drawings don't have.  However, it appears other people in the organizations have plenty of time to chase down this issues once the job is accepted and there's some liability.

KENAT, probably the least qualified checker you'll ever meet...

RE: Thru hole dimensioning in deep part

I agree, really.  No stated standard, no basis for interpretation.  Assumptions have a way of coming back and biting you.
However, if you were in a situation where it was imperative that this cube be made, you would have to make assumptions.  Some, I feel, are safer than others.
Anyway...deadhorse

RE: Thru hole dimensioning in deep part

I think I see its hoof twitching.

I've made assumptions for internal stuff but when it's a customer drawing I've normally flagged it, if nothing else explained our interpretation or similar.

KENAT, probably the least qualified checker you'll ever meet...

RE: Thru hole dimensioning in deep part

Absolutely. If the vendor drew it, and they also made it, then there's no question. Reject it. If you tell them what it needs to do, and they not only make an ambiguous drawing, but also produce a part that doesn't function the way you need it to, then it needs to be rejected.

All of my assumptions were made based on it being an in-house drawing.

OutOfSquare, I have a stupid question for you. Why are you trying to let the part pass inspection? Either way it's the vendor's fault (bad drawing or bad part). Letting it pass is like me drawing a house that's built on a slab of which the material is not called out, building it on a slab made of jello, putting it up for sale, and then having the structural engineer come in and check everything and say, "Oh yeah, the jello slab, that should be fine, because he didn't specify what material the slab was going to be."

Am I wrong in my assumptions?

V

Mechanical Engineer
"When I am working on a problem, I do not think of beauty, but when I've finished, if the solution is not beautiful, I know it is wrong."

- R. Buckminster Fuller

RE: Thru hole dimensioning in deep part

VC66, re-read out of squares posts.

It appears to be a customer drawing.

It appears the machining was subcontracted to a vendor.

So that's why he doesn't want to reject it.

KENAT, probably the least qualified checker you'll ever meet...

RE: Thru hole dimensioning in deep part

Aha, thanks KENAT. I read his second post, which stated that the drawing wasn't that old, and was created by a well-known entity. I assumed that meant a vendor.

Thanks for the clarification. It seems that we've gone so far down, I completely forgot what the original post was asking.

V

Mechanical Engineer
"When I am working on a problem, I do not think of beauty, but when I've finished, if the solution is not beautiful, I know it is wrong."

- R. Buckminster Fuller

RE: Thru hole dimensioning in deep part

(OP)
Correct, KENAT. Our company contracted to make this part amongst others in a bigger job. My customer provided the drawing, and I subbed-out the machining. Inspection rejected the part at receiving inspection.

I'm exptected to respond to a Corrective Action Report (CAR), stating why the error occurred and what action will be taken to "fix it". If some "corrective" action needs to be taken, I must also explain this to the machine shop.

After reading the comments here -- and having considered this from every possible angle (pun intended) -- I'm more convinced than ever that KENAT and ringman are correct. Without any stated standard there are no clear requirements to check against. It's my further opinion that, absent any explicit standard the part cannot be held to dimensional requirements beyond those points dimensioned on the print.

Perhaps this could be taken to a silly extreme, but it's equally irrational to inspect two select, un-dimensioned features for "uniformity", but leave other, equally important, yet un-dimensioned features un-checked.

There's a good chance our customer will accept the part, as-is, in which case no corrective action will have to be stated. I'll know very soon.

I'm certified in ANSI Y14.5 GD&T, so I prefer to see GD&T control frames on machined part drawings. Our customer most assuredly knows about Y14.5, but chose not to apply it on this design. Why should anyone else...

RE: Thru hole dimensioning in deep part

2
I would argue from the negative...  Is there a standard out there that permits the kind of interpretation that OutOfSquare is proposing to get the part through QA (that the hole locations only matter on one face).  I'm not an expert, but I don't think there is one.

Obviously the standard needs to be added to the drawing, but that doesn't give the machinist license to do whatever he likes.  The parts are clearly non-conforming.  If the vendor disagrees you can ask him to show you what standard he used to interperet the drawing.

-b

RE: Thru hole dimensioning in deep part

(OP)
FACT: The drawing gives dimensions for the cube in three views (three dimensions). The hole center points are dimensioned in only one view (two dimensions on one plane or surface). All of the dimensioned features are within the drawing tolerance at the points dimensioned on the drawing. The part is in tolerance, end of story.

Inspection assumed the holes “must” be equidistant from a certain side, top and bottom. This is NOT stated, implied or required by the drawing, any more or less than is symmetry, perpendicularity, or cylindricity. Inspection did not assume symmetry, neither did they impose perpendicularity constraints – only parallelism, and only with regard to the relationship between certain selected features, exclusive of other equally important features.

The part is in tolerance at every point dimensioned on the drawing.  What’s wrong with applying this most obvious standard?  This is the only standard which passes the, "would it hold up in court," test, and it’s the only one implicit in the drawing.  It's only when you start to assuming other “un-dimensioned constraints” that problems arise.

I can see how parallelism is the geometric relationship that's easiest for people to grasp. But for the sake of better understanding, disregard parallelism for a moment and apply the dimensions and tolerance relationships to this part in regard to diameter, perpendicularity, cylindricity and symmetry.  You'll find that on the generous side, the exit holes have a linear tolerance at the surface relative to other features greater than +/-.010, but not an unlimited tolerance.  On the other hand, if you apply the linear tolerance to all of these geometric considerations, you must reduce the tolerance on some relationships.  Either way, it's not an "unlimited tolerance for all features not dimensioned." But the tolerance at points other than those dimensioned on the drawing could vary greatly -- if measured -- depending upon interpretation and assumptions, absent any standard.


RE: Thru hole dimensioning in deep part

I'm sorry--standard or not, assumptions or not-- if you drill a hole perpendicular to a face, just so i starts cutting chips, and then turn the drill 89° so that the hole is 89° off kilter, just because the face dimensions of the hole are correct, does not mean that part should pass, or that the machine shop is not at fault. That is the last I will say about that, because it's either here nor there.

You are right (as far as my limited knowledge of standards go). Where there is no standard there are no assumptions. I feel that you're letting the machine shop off the hook, but I believe (now that I know that they didn't also make the drawing) that you're doing it for the right reason. I wouldn't want to scrap parts based on a bad drawing either.

I hope I'm clear in my response. I still think you should chastise whoever made the drawing, if only for the fact of forcing people to think about this topic.

Ok... took my medicine. I'm good now. 2thumbsup

V

Mechanical Engineer
"When I am working on a problem, I do not think of beauty, but when I've finished, if the solution is not beautiful, I know it is wrong."

- R. Buckminster Fuller

RE: Thru hole dimensioning in deep part

Does the part perform as intended/

RE: Thru hole dimensioning in deep part

OutOfSquare

Quote (OutOfSquare):

Inspection assumed the holes “must” be equidistant from a certain side, top and bottom. This is NOT stated, implied or required by the drawing, any more or less than is symmetry, perpendicularity, or cylindricity. Inspection did not assume symmetry, neither did they impose perpendicularity constraints – only parallelism, and only with regard to the relationship between certain selected features, exclusive of other equally important features.

I think parallelism, and perpendicularity (not symmetry unless there was a centerline) would be implied by ANY standard.  Otherwise your cube could be a 45 degree parallelogram and still be to print.

Your vendor has no defence.  Even using your fantasy standard of "dimensions only apply on that face", then the print was obviously underdimensioned (no exit hole locations were given) and the vendor should have asked.  

-b

RE: Thru hole dimensioning in deep part

... or lack of standard.
Thank you, bvanhiel.

RE: Thru hole dimensioning in deep part

Outofsquare.

My stance on this is based on my very limited law training at uni and stuff I've picked up over time etc.  I could be wrong, but I don't think I am.

It's common practice, perhaps even common sense to assume most of the things most others have stated that would support inspections point of view of rejecting the part.

However, how often does common sense hold up in a court of law, which is where in theory this could end up.

In the event of a dispute the drawing is a legal document and so needs to be unambiguous or there's a chance that a lawyer will find enought wiggle room to get his client off.

Outofsquare, As to your corrective action could it be something like this.

Add wording to our standard quote document that drawings which don't explicitly state a drawing standard will be assumed to generally be in accordance with ASME Y14.5M-1994.  Add wording to your standard purchase order that drawings are to be assumed to be generally in accordance with ASME Y14.5M-1994 unless otherwise stated either there or on the drawing.  Let the vendor know that the parts would have failed inspection to standard industry practices but as they were not explicitly invoked the part will be accepted as is.  Suggest increased inspection of the vendors part on the next few orders.

KENAT, probably the least qualified checker you'll ever meet...

RE: Thru hole dimensioning in deep part

(OP)
bvanhiel, you said, "Otherwise your cube could be a 45 degree parallelogram and still be to print."

No it couldn't, not based on the information provided above.

It was plainly stated, more than once, the cube is dimensioned on thre views -- in three dimensions. This precludes your false assumptions if you understand geometry.

You also said, "I think parallelism, and perpendicularity (not symmetry unless there was a centerline) would be implied by ANY standard." Again, do the geometry. When you enforce any geometric constraints on the part -- beyond those expressly shown -- you must make concessions, one way or the other. You don't seem to understand the geometry. Have someone draw it out for you.

Furthermore, the drawing does not show a "centerline" for the thru holes in the side views. What does that do to your, "no geometric constraint imposed absent a centerline" theory?

RE: Thru hole dimensioning in deep part

Actually, OutOfSquare, not to continue to beat a dead horse, but you're wrong based on your assumptions above. If you're trying to say the a point doesn't have to equal and axis and an edge doesn't have to equal a surface, then all those other dimensions on your drawing could be measuring, not from surface of one side of a cube to the other, but the dimension of the edge, and therefore as long as that infinitesimally thin line is in tolerance, the entire rest of the surface can be off kilter, and the width at the top of the cube doesn't necessarily have to match the width at the bottom of the cube. But if you dimensioned both, isn't that double dimensioning? But is it not double dimensioning as long as there is no standard to define what double dimensioning is?

I think this is more of an argument of what came first--the common sense or the standard? I'm voting for the common sense.

V

Mechanical Engineer
"When I am working on a problem, I do not think of beauty, but when I've finished, if the solution is not beautiful, I know it is wrong."

- R. Buckminster Fuller

RE: Thru hole dimensioning in deep part

(OP)
Court cases, many times, are decided based upon whether or not a claim is reasonable to the average person (jury).

The part meets all of the dimensioned requirements of the drawing. Any reasonable person would agree. Part's good. Case closed.

RE: Thru hole dimensioning in deep part

Quote (OutOfSquare):

It was plainly stated, more than once, the cube is dimensioned on thre views -- in three dimensions. This precludes your false assumptions if you understand geometry.

You may need to retake geometry.  Measuring across the flats of a parallelogram prism will give you three measurements of 8 inches just like a cube.  Get someone to draw you a picture.

[quote OutOfSquare]You also said, "I think parallelism, and perpendicularity (not symmetry unless there was a centerline) would be implied by ANY standard." Again, do the geometry. When you enforce any geometric constraints on the part -- beyond those expressly shown -- you must make concessions, one way or the other. You don't seem to understand the geometry. Have someone draw it out for you.[quote]  

What concessions am I making?  Show me ANY standard that does not assume parallelism and perpendicularity.  Any at all.

Quote (OutOfSquare):

Furthermore, the drawing does not show a "centerline" for the thru holes in the side views. What does that do to your, "no geometric constraint imposed absent a centerline" theory?

Not sure who you're quoting here, but it's pretty obvious that the holes are thru holes (they are called out as such).  The centerline is not really required to communicate intent.

You're being too lax in even considering accepting these parts as being to print.  It may be a bad drawing, but the part still doesn't meet the print.

-b

RE: Thru hole dimensioning in deep part

OutOfSquare, the drawing (as you described it) does not say anything close to what you are saying it says (based on your own description of the drawing and your comments here).  You are making very dangerous assumptions that challenge the validity of and drawings your company makes and that of your customers too.  I would suggest it creates a liability issue for your company and its customers.  Ultimately, it's not about this one drawing or this one customer.  It's about all the drawings and all of your customers.  You gotta do what's right for your company.

Also, all of us here are offering free help to you with your question.  Making accustions against us and devaluing our opinions kinda defeats the purpose of asking members of this forum for help.  Take what we have given you here for what it is: advice.  You are free to do with it as you please.

Matt Lorono
CAD Engineer/ECN Analyst
Silicon Valley, CA
Lorono's SolidWorks Resources
Co-moderator of Solidworks Yahoo! Group
and Mechnical.Engineering Yahoo! Group

RE: Thru hole dimensioning in deep part

Dont think it has been answered, so again is it possible to check the part for function on the related test fixture?

RE: Thru hole dimensioning in deep part

Yeah, but out of squares right winky smile

KENAT, probably the least qualified checker you'll ever meet...

RE: Thru hole dimensioning in deep part

(OP)
I very much respect and appreciate the comments of many of the individuals here, particularly comments such as, "without the benefit of a specific standard, such as Y14.5, there is no clear cut definition of the allowables," and, "... the drawing is effectively incomplete."

That answers my question.  All others are hypothetical or subjective.  The part meets the drawing. Imposing other requirements necessitates subjective conjecture.

RE: Thru hole dimensioning in deep part

(OP)
I hope to know in a few days whether the part will be accepted by my customer.  If not, we're fully prepared to make whatever adjustments they requrest and will promptly do so to maintain good relations. I will post the outcome.

RE: Thru hole dimensioning in deep part

(OP)
"Measuring across the flats of a parallelogram prism will give you three measurements of 8 inches just like a cube."

I think you're describing a parallelepiped.  smarty

Hope your parallelepiped doesn't have holes drilled perpendicular to the top, all the way through, 'caus when they check 'em for parallel with the sides, it won't pass. big smile

RE: Thru hole dimensioning in deep part

If I may be a voice of reason here.  I have tried to weed thru all the posts and now all I have is a headache. To quote an old adage used by one of my professors - "you can't see thru the forest for your nose is against the tree!"

Please understand that there is no disrespect intended for anyone who has contributed here, this is just my two cents to best help OutofSquare and then hopefully everyone can move on to the next intriguing topic.

First the part has been manufactured right or wrong, it really doesn't matter at this point? The question is will it work for the customer purpose?  Therefore, I would then submit it along with full disclosure of your findings to the customer for acceptance.  If it is accepted end of issue, if not, you the contractor are responsible for making it right, because you failed to flag/reject the incomplete spec(s)(I would imagine if there is one, then there is more) prior to sending it to the sub for fab and the customer's responsible for revising their own drawing(s).  This takes care of the correction of this undesirable situation.  

Now on to the corporate corrective action (CAR), it would appear that there are multiple root causes here.  However, you OutofSquare or your company are only responsible for your end of this undesirable situation.  Which is as I already mentioned  sending the incomplete/unambiguous drawing out for fab in the first place.

It is my recommendation that in the future or even immediately, have your companies procedure/process/work instruction for customer drawing review, prior to manufacturing release, revised to become a gate if you will.   Then train all involved to the revised process.  Include a drawing checklist form to be completed and signed, possibly using questions from the document attached.  These guidelines are to be used at your own discretion, you can simply tweak to match your specific industry or company needs, this is merely a suggestion.

I hope for you and your companies sake that this is an isolated incident and that there are not anymore of their drawings that are incomplete & unambiguous.  I fear that if this went to court there would be a shared liability verdict, but not necessarily 50-50.  Additionally, check all the contracts/PO's, there may be some verbage about which standard is referenced, it may even be buried in a customer's corporate procurement standard which supersedes the Y14.5 standard even if listed or not on a print.

So in the end, I would chalk this up as a learning experience and again hope that it is not to painful or costly for your organization to recover from.

RE: Thru hole dimensioning in deep part

(OP)
"you the contractor are responsible for making it right, because you failed to flag/reject the incomplete spec(s)."

Your solution is based upon a false premise. The spec is complete. The part fully meets the requirements of the drawing. No issue -- that is, until someone starts assuming that the drawing is not what the customer "really" intended, in which case, you've assumed something that isn't required by the drawing.

I'm not inclined to assume the customer doesn't know what he wants.

Should the customer not accept the part, that's called negotiation. The outcome will likely be based upon each party's overall "win-lose" assessment of their position.

RE: Thru hole dimensioning in deep part

OutOfSquare,

Thanks for looking up the name for me.  Then again a parallelepiped would still pass YOUR inspection, as you don't seem to think parallelism is implied of the holes,  which was the point of bringing it up.

-b

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources