×
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

COUNTERBORE
7

COUNTERBORE

COUNTERBORE

(OP)
Hi everyone. I submitted this question August 28 and only had one
response. Let me reword the question. Figure 5-37 in the standard for
positioning a through hole and a counterbore hole with one positional
control. The question is, does the through hole and the cbore hole have
two different zones with the same tolerance size where the cbore hole
can tilt or shift in a different direction than the through hole, or
the two diameters must have one axis within one zone for the length of
both features?

RE: COUNTERBORE

(OP)
please ignore the August 28th date. It was from a different memo. I do not know how to delete the statement.

RE: COUNTERBORE

Gary,

Perhaps the committee violated one of its FUNDAMENTAL rules here in specifying a manufacturing process.  Perhaps the proper way would have been to specify the diameters individually with the tolerancing as required to provide the proper clearnaces for the head and the body of the screw.

But as far as the example goes, I would have to go with a single tolerance zone for both features simultaneously.

RE: COUNTERBORE

They are two individual features therefore an axis can be constructed for each feature independently.  

RE: COUNTERBORE

  The axes of the two features must fall within the same tolerance zone but they are independent of each other. Reading 5.7(a) on page 135 it says "Identical diameter tolerance zones for hole and counterbore are coaxially located at true position relative to the specified datums". This is a clear indicator that the tolerance zones, although identical, are separate.
ringman,
 I don't see where there is a manufacturing process specified. What am I missing?

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

RE: COUNTERBORE

I have always thought that Cbore was manufacturing process which required the use of a Counterbore (tool) .  Would that not be specifying the process rather than the geometric definition?

RE: COUNTERBORE

I would make one callout for the hole and CBore, and one FCF for it. Treat them as one. It would be up to the machine shop if they want to machine them separate, but within the tol indicated.

Chris
SolidWorks 07 4.0/PDMWorks 07
AutoCAD 06
ctopher's home (updated 04-21-07)

RE: COUNTERBORE

I agree that we have 2 features with the same tolerance and are independent of each other.

Dave D.
www.qmsi.ca

RE: COUNTERBORE

3
My understanding was as majority of posters and as detailed by Power Hound.

That said this often seems to be overlooked by others, many assume the Cbore & hole are automatically co-axial, this includes people that prepare standard hole charts etc.

My checker actually went through a hole chart we'd been using and made this correction.  Of course now I'm not sure they match standard C'bore tools, sometimes you can't win!

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

RE: COUNTERBORE

ringman,
  Counterbore is what the feature is called, like countersink or counterdrill. The tool and the process may share the same name, but the feature is what is being referred to in the standard. They don't care how you apply the counterbore, it just needs to be there. On a CNC mill, I never use a counterbore tool to apply a counterbore, I interpolate the larger diameter with an end mill.

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

RE: COUNTERBORE

(OP)
As of this date, it is 5 to 1 in favor two separate axes.

It is my opinion, one axis for the length of both features:

 1. Figure 5-37 states 0.25 positional tolerance zone for hole and counterbore.  Not zones.

 2. It does not make sense to have two axis going in two directions.

 3. I think it implies one tool and one axis the total length of both features.

 4. If the workpiece cost thousands and the two features were machined separately at different angles within the 0.25 zones with no assembly there would be litigation.

 5. The bottom line is to state on the drawing next to the position callout the intended definition.

 Gary

RE: COUNTERBORE

So one might say "You can lead a horse to water, but you can't make him drink"

RE: COUNTERBORE

Given your background Gary (assuming you're the Gary Whitmire I think you are as in Genium & Drafting Zone, 14.5 commitee member...) I'm loathed to disagree but...

1.  In this case the figure doesn't quite appear to match the paragraph.  5.7a explicitly states 'zones'.  Given what paragraph 1.1.4 says about the figures only being illustrations etc then I assume the wording in the paragraph takes priority.

2.  Within the limits imposed by the pos tol, why not?  If as Powerhound details above the c'bore is made by a second operation the axis could be off slightly from 'perfect' however, so long as the resulting feature is still in tolerance, and was correctly toleranced in the first place, it would still work.

3. Wouldn't implying one tool contravene 1.4e as ringman points out.

4. I thought positional gives some control over the angle of the feature (figure 5-6).  Hence if toleranced correctly in the first place then if the holes are in tolerance it shouldn't prevent assembly.

5. To my understanding by referencing ASME Y14.5M-1994 on the drawing and dimensioning as paragraph 5.7a then additional clarification shouldn't be required.  By stating next to the drawing do you mean dimensioning as per 5.7c?

(Just to clarify I'm looking at ASME Y14.5M-1994)

I hope these counterpoints are taken in the spirit they were made.  Obviously this type of discussion can be healthy as it can lead to clarification of the standard or improved interpretation of it.

Ken

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

RE: COUNTERBORE

If the term Cbore were eliminated, and the holes were adequately defined and located by datum features and positional tolerances would we be having this discussion?

Is the current practice to specify drill, ream, or punch for holes?

RE: COUNTERBORE

To be fair Gary, I think that if one has the luxury of using a stepped tool to do both the hole and the counter bore simultaneously that may be ideal for process efficiency when both features have similar tolerances for size, finish, orientation, and location. The standard however, in defining how multiple coaxial attributes "features" that can be specified for location or orientatation with a single FCF for the sake of reducing "clutter" on the drawing.... is not suggesting how those features are processed. The following paragraphs in the standard state that when the tolerances ar not similar more FCF's are required.

Also to be fair it is exceedingly difficult to create a stable and repeatable axis from a shallow counter bore without making huge assumptions about its orientation... so the axis, if checked for its displacement, is either generally assumed oriented to the axis of the deeper hole or assumed perpendicular to the datum feature.

All this considered... the liberties and constraints in the standard regard the features independently and make no inferences about processing.    

RE: COUNTERBORE


 1. The paragraph that I cited specifically says "zones".
 2. It doesn't make sense to have the axes of the two features mis-aligned either but they are going to be, no matter how hard you try. The amount of mis-alignment that is permissible is up to the designer to determine.
 3. Nothing implies the use of a single tool.
 4. If the part is out of tolerance there SHOULD be litigation regardless of whether the part cost hundreds, thousands, or millions. If not, there shouldn't. If the counterbore is machined at the max inclination WRT the hole and the part doesn't work, then the tolerance is incorrect.
 5. An alternative is to use the example in FIG 5-38 and tolerance the counterbore tighter than the through hole. Notes are never an option when there is a geometric tolerance available.

Opinions are the reason that standards were created; to remove the error in interpretation. There are a few things that are still not addressed in the ASME standard and are still somewhat open to interpretation, this however is not one of them. The paragraph I mentioned in my first post to this thread is clear in it's meaning.

Paul,
  Amen to that.
  

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

RE: COUNTERBORE

ringman,

A counterbore is essentially just a larger diameter step in a hole.

A couterbore tool or bit is a tool designed to create a stepped hole.

They are different things, I do not believe anyone else on this thread is donfusing the two.

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

RE: COUNTERBORE

A dwg should never indicate how the feature is created. Just call out the hole and the CBORE together with one tolerance. How the machinist gets there is up to him/her.
Unless the CBORE is used differently other than for a screw or bolt.

Chris
SolidWorks 07 4.0/PDMWorks 07
AutoCAD 06
ctopher's home (updated 04-21-07)

RE: COUNTERBORE

ctopher,

I agree, but in reviewing my old Machinery's Handbook it appears that counterbore is definitely a process using rather specific tools. Hence the question WHY DO WE SPECIFY THE PROCESS on drawings?  Why not just the geometry?

RE: COUNTERBORE

Counterbore can refer both to the feature created and the tool used to create the feature.

http://www.answers.com/topic/counterbore-1?cat=technology

http://dict.die.net/counterbore/

While use of the word may have evolved out of the tool or process used to create the feature, its use to describe the feature is now so widespread and ingrained that it's not really specifying a process.

Ctopher, never say never ASME Y14.5M-1994 1.4e does allow processes to be on the drawing in certain circumstances.  However it also makes it clear that it is generally to be avoided.

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

RE: COUNTERBORE

A counterbore is a process AND a feature, just like a countersink. When the symbol for a counterbore is shown, it is specifying the feature, not the process. The same goes for a countersink. It's not specifying the process or the tool to do it, it just says to apply a countersink to the dimensions specified. As far as using specific tools for the counterbore; as I said before, I never use a counterbore tool yet I still am able to create a counterbore. That's because the tool, the process, and the feature are 3 different things.

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

RE: COUNTERBORE

A+ to KENAT...

Man you really do your homework. I just finished up my post and noticed you had squeaked one in on me.

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

RE: COUNTERBORE

So give me a starwinky smile

There are a lot of questions discusions I don't/can't contribute to due to lack of experience etc.  This topic however, is something I've looked at before and discussed with someone far more knowledable than I, so I'm going to town.

That way when I ask a question hopefully people answer.

I'll scratch your back...

Putting, or even hinting, at processes on a drawing is a red flag for me, I'll usually go off about even a poorly worded note.  

However, in this case I don't see putting Counterbore or |_| (that's meant to be the symbol) as implying a process.  

On the other hand, someone says "DRILL HOLE .125" or DRILL & TAP 8-32" I'll slap their wrist!

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

RE: COUNTERBORE

(OP)
KENAT: I do not disagree with your comments. My thinking was:

1.The text in paragraph 5.7(a) stated “ZONES”, and the text in figure 5-37 states “ZONE”. Which one is correct? I do not know. That is why I said a note under the feature control frame may be needed if there is a chance that the wrong definition may be used.

2.If the two axes tilt in two opposite directions, you are correct the hole sizes need to be calculated.

3.I should not have mention an implied counterbore tool, I know we do not mention the process on a drawing.

Thanks KENAT, I need to be more accurate in my statements.

RE: COUNTERBORE

Gary, you're probably more likely to know than I but given what 1.1.4 says about figures I'd expect the paragraph to take precedence over the figure, although it's not cut & dried.

This is the first time I've seen the confusion amongst what I'd take to be mostly fairly knowledgable parties, so up to now it's not something I'd have thought needed clarification.

This may be something worth pointing out to the ASME commitee for consideration for correction/clarification.  I strongly suspect the figure needs correcting but I could well be wrong.

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

RE: COUNTERBORE

Kenat,
I'll give you a star. Well said.

Chris
SolidWorks 07 4.0/PDMWorks 07
AutoCAD 06
ctopher's home (updated 04-21-07)

RE: COUNTERBORE

One might consider that the hole for the body of the screw would require a closer positional tolerance than the one for the clearance of the screw head.    Comments?

Then the question, what controls the relationship for the seating surface for the screw, if not the process?

Comments?

RE: COUNTERBORE

Positional tolerances do. Various processes can get you there one way or another.

Chris
SolidWorks 07 4.0/PDMWorks 07
AutoCAD 06
ctopher's home (updated 04-21-07)

RE: COUNTERBORE

I concur with Gary and Kenat on the "jist" of the callout. If you are using the symbol for CBORE and not the word (and you should be), then it ought to bre clear that you are delineating a feature shape, and not a machining process. Regarding ringman's last comment, I call out One FCF, and one tolerance for both the hole and its associated cbore, but I set the size of the cbore such that the screw shank limits travel at worst case tolerances rather than the screw head touching the cbore dia first. To do this, one may have to make the cbore larger than many of the screw charts out there. Moreover, I will use a looser tolerance (say +/-.005" on bolts <1/2" dia) on the cbore and stick with normal and close tolerances on the bolt shank and bolt hole. This may preclude using commercial counterboring tools in many cases, but many CNC machines are using end mills anyway. Machine tool makers have some pretty tight size tolerances on the cbore dia of many of the the counterboring tools relative to screw sizes, and I don't see many designers taking that into consideration with the hole position tolerances they specify.  

RE: COUNTERBORE

ringman,

Your first point is covered in 5.7 b & c.  However my preference is to have a single FCF and just make sure the Cbore dia is big enough to accomodate tolerances from all other features/components (as CheckerRon).  As I mentioned earlier and CheckerRon says, this can end up ruling out a lot of 'off the shelf' counterbore bits.  The use of a larger C'bore with looser tolerance achieves almost the same thing as a looser positional tol due to 'bonus tolerance'.

"Then the question, what controls the relationship for the seating surface for the screw, if not the process?
"

Umm, am I missing someting here?  The tolerances on the drawing control the relationship.  

The combination of the positional tolerance, the diameter tolerance and the c'bore depth tolerance should take care of this.  If you aren't specifying all these then your drawing is incomplete.  There are at least 2 common processes for creating a counterbored hole, either using a c'bore bit or creating the hole and c'bore separately as a 2 stage process.  If the drawing is created properly and the processes done correctly both are perfectly good options.

Ron,

I don't think Gary & I quite agree.  We both agree that figure 5-37 doesn't quite match the wording of 5.7a.  The paragraph clearly says zones, the figure says zone.  I believe that the paragraph takes precedence over the figure and so there isn't any ambiguity, the figure is just slightly wrong.  Gary doesn't agree that the paragraph necessarily takes precedence and so believes it's ambiguous and should be clarified with a drawing note or similar.

What do you think?

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

RE: COUNTERBORE

I don't see the ambiguity, as the figure shows two zones, even if it uses the word "zone", as it is an example of separately controlled hole/counterbore.  But then again, I didn't dig too deeply, as I have enough to ponder checking some GD&T that the designer obviously didn't understand.3eyes

KENAT, how would you like some side work?wink

RE: COUNTERBORE

ewh, I'm pretty sure your understanding would be better than mine, although checking GD&T that the Designer didn't understand is becoming my specialty.

I have side work, it's called trying to check for the other half of the business as well as the half CheckerRon used to take care ofwinky smile

CheckerRon might be interested though if it's any more than a joke.

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

RE: COUNTERBORE

Ctopher,

My question with regards to the seating of the screw head on the CBORED hole, is based on the example in the standard.  The only control that is apparently indicated is the one which controls the depth.  The depth allowance quite probably could exceed the angular misalignment with the body of the screw.  Where is the refinement, if not controlled by the tool?  Perhaps the example in the Standard needs some refinement.

Lets not forget that the Standard is supposed to provide for a "universal' interpretation of drawings.

Another look  at the example, and I ask "What is gained by the inclusion of the symbol for CBORE?.  Would it not fly just as well without it?"  There is a diameter and a depth.

RE: COUNTERBORE

ringman.

If the depth of the cbore has a fairly large tolerance then yes, the bottom of the cbore could be at quite an angle.

If this is problem you need to add a tolerance (eg, perpendicularity to the bore or more likely parallellism to the surface) to correct it.

The tool/process controls nothing, it is used to meet the requirements on the drawing.  If you have a requirement it needs to go on the drawing.  

Read paragraph 1.1.41 closely before you start talking about the figure being incomplete etc.

As to the symbol, are you serious?  It's a clarification.  If you have a cross section as figure 5-37 has then yeah it's pretty clear which diameter and depth is which.  Without the cross section it may not be clear.

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

RE: COUNTERBORE

To expound on KENATS last post, if the hole is not shown in a cross section, then ommitting the cbore symbol would necessitate noting the bottom profile (flat bottom) or risk getting a drill point angle.

RE: COUNTERBORE

(OP)
I do agree that the text is primary. On August 7th I did a white paper on counterbores showing two separate tolerance zones for a drawing having one positional control. When I was working on the DRM, I saw the word “ZONE” in Figure 5-37, so I asked the question on ENG-TIPS as to what members thought. I will stick with the two separate zones as stated in the Y14.5 text and my white paper.  So before I dig myself another hole, I would like to thank everyone for their input.

RE: COUNTERBORE

Again, taking the example at face value for the depiction provided, what is the benefit if any of having the symbol added? Is there any?  Gary?

RE: COUNTERBORE

I have seen dia and depth called out without the CBORE symbol. The outcome was a drill point where the CBORE should be. It's a good indication of what the feature should look like. The symbol should also be known with different languages.

Chris
SolidWorks 07 4.0/PDMWorks 07
AutoCAD 06
ctopher's home (updated 04-21-07)

RE: COUNTERBORE

EWH,

What if the depth tolerance were sufficient to allow a csk to be acceptable?  Again, it seems that the CBORE  tool controls the angle of the seat and additionally the corner radius.  Radius not previously mentioned in this thread, if I am not nistaken

RE: COUNTERBORE

  On page 1 of the standard, paragraph 1.1.4 it states that sometimes figures are incomplete by intent. This is probably one of those cases where the idea of how to tolerance a counterbore using a single FCF and how to interpret it was all that the figure was intending to show.
  Even taking that into consideration, I'm not sure what the dilemma is regarding the seating of the screw head. The axis of the hole will govern the orientation of the bottom of it and the axis is controlled by the tolerance in the FCF. I don't really know why you are so hell bent on eliminating the CBORE symbol from the standard. I suppose you think CSINK should go with it.
  I make the above comment in a quasi-jovial manner. I don't intend disrespect, I'm just a little amazed at how this point is being belabored...and I'm guilty of perpetuating it.
  Anyway, I won't belabor it any more.

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

RE: COUNTERBORE

ringman, have you read paragraph 1.1.4 regarding figures?

Quote:

1.1.4 Figures. The figures in this Standard are intended only as illustrations to aid the user in understanding the principles and methods of dimensioning and tolerancing described in the text.  The absence of a figure illustrating the desired application is neither reason to assume inapplicability, nor basis for drawing rejection.  In some instances, figures show added detail for emphasis.  In other instances, figures are incomplete by intent.  Numerical values of dimensions and tolerances are illustrative only.

You can't really take the figures at face value for anything more than the specific point they're trying to illustrate, and even then in this case there is the zone/zones ambiguity.

ewh (and ctopher) explanation for the cbore symbol is even better than mine.  

If you must insist on taking 5.37 literally then... There is no indication of where the cross section is taken/where it shows.  i.e. There is no section line "A-A" and the section itself doesn't say "Section A-A" so there, the Cbore symbol is needed so we know it's a Cbore and not a CSK or even a male feature.

Gary, sorry my misunderstanding of your viewpoint.

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

RE: COUNTERBORE

For ***** sake.  The tool or process CONTROLS nothing.

The angle has to be in the limits of the depth tolerance.  For extreme angles then the orientation of bore will control how the screw sits as Powerhound points out.

The corner is sharp within any relevant tolerances or drawing notes about sharp edges etc.

There's no guarantee a cbore bit will be used to create the cbore hole, it's just as likely these days to be a 2 stage operation with an endmill for the cbore.

Sorry, got a bit carried away there.  Powerhound probably has a point, the smell or rotting equine flesh will soon fill the air, que ewh with his favourite emoticon.

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

RE: COUNTERBORE

(OP)
ringman
The symbol is redundant.

Gary

RE: COUNTERBORE

ringman,
If the depth tolerance were sufficient to allow a csk or a drill pt to be acceptable you would be better off specifying a counterdrill, for which you don't need a symbol.

RE: COUNTERBORE

Gary,

Thanks.  

I did a quick check on CAD of the example in the Standard and the tolerances on the example allow an angle on the seat of approx 15 degrees off horiz. (Worst case).  

RE: COUNTERBORE

I only came up with 4.29 degrees off horizontal. I think your "quick check" was a little too quick.

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

RE: COUNTERBORE

Powerhound,  

I did a recheck and with a triangle of 1.554, .4, and 1.5,based on the diameters and depth, I still come up with 15 degrees.  What are your figures to arrive at 4.29 degrees?

I used diameters of 6.4 and 9.4 and a depth of .4.

RE: COUNTERBORE

Diameter 9.4, depth tol range of .4, I cheated and drew the triangle in CAD, it says it's only 2.44 off horizontal?

This assumes constant angle across the dia of the C'bore etc.

What am I doing wrong?

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

RE: COUNTERBORE

Well, Not for sure, but the triangle I drew represents the width of the seat for the head, based on the smallest head clearance hole and the largest body clelarance hole.  .4 is the depth.

This is only one side of the seat in the section view.

Does that make sense?.

RE: COUNTERBORE

Yep, if you're looking at only the land, and acting as if it had been made as a shallow csk then 15 degrees is about it.

Included angle of the csk about 150 degrees.

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

RE: COUNTERBORE

ringman,
  I only checked the deviation of the c'bore because as I said before, it is a separate feature. I drew the counterbore at LMC to get the largest amount of deviation so the diameter is 9.6, which makes the tolerance zone .45 in diameter. If you draw a line from X-.225 Y0 up to X.225 Y6.0 (6.0 represents the depth of the c'bore) you will get an angle from 0 of 4.59 degrees. If you make the counterbore to it's MAX depth of 6mm, the angle is 4.29 degrees.
  For the purposes of furthering the cause. I checked the entire depth of the counterbore and hole as if it were one feature and came up with the same thing as KENAT.

What are we missing?
  

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

RE: COUNTERBORE

Powerhound,

If I read this right, you are looking at the angle of the axis of the dia as allowed by the pos tolerancing. (I believe then your angle would be off the vertical)   I am looking at the seating surface for the head, and looking at the worst case with dimensions provided.  We are apparently looking at 2 diff things entirely.

My look at the worst case was assuming that we use this 'special toothpick' to generate the hole to the dimensions. This rather than a counterbore tool.

RE: COUNTERBORE

ringman, there's no implication that a c'bore tool has to be used to make the c'bore.  It is very likely the c'bore feature is made using an end mill or something, what's so confusing about this?  The feature on the part as defined by the drawing is process independant.

I'm also not convinced the included angle of 150 degrees is truely worst case.  In this case the edges of the screw head will still sit on a fairly even contact it will just be a very narrow ring, under a lot of load they'll probably brunel the cbore a bit.  For many applications this probably wouldn't cause too much problem.  In some it may in which case an extra/tighter tolerance should be called out on the drawing.

I'm pretty sure I've lost interest now.

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

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