Depth of a CB hole on a incline 2

[GunT]

Hello all,

I am looking for standard definition of depth of a CB hole on a inclined surface.

For e.g., I have a triangular gusset. I have a CB hole on the inclined surface parallel to the base. So the depth of the CB hole varies from a min. value to a max. value. So when I do a hole callout annonation in a drawing for a CB hole what should the depth be? Min. value, max. value or value at the center? What is the standard manufacturing practice?

And is there any standard that defines this and what is it? Any help would be really appreciated.

Regards,

 

[ewh]

I dimension this type of hole in a section view so that I can reference a surface from which to measure.

 

[ctopher]

I agree with ewh. You can dim from a surface or a defined point. The min, max, etc is up to you.

Chris
Systems Analyst, I.S.
SolidWorks/PDMWorks 05
AutoCAD 06
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[GunT]

ewh and Chris,

Thanks for the quick replies. Section view makes sense.
So a regular CB hole callout using a CAD software would be ambiguous and incomplete?

If not how is the machinist going to interpret it?

Regards,

PS: I have used "a" instead of "an" before an vowel in my previous post. Sorry, it was a typo

 

[ctopher]

So a regular CB hole callout using a CAD software would be ambiguous and incomplete?

If not how is the machinist going to interpret it?

Can you clarify? How can it be ambiguous and incomplete using CAD?

Chris
Systems Analyst, I.S.
SolidWorks/PDMWorks 05
AutoCAD 06
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[GunT]

As explained in my above example, I have created a CB hole using SolidWorks hole wizard and made the drawing of the part. And called out the CB hole using "Hole Callout" Annotation of the software.

The callout is as follows:

<dia sym>hole thru
<CB sym>CB hole <depth sym> depth of CB head.

The depth you obtain is the max depth by default(If no subsequent operation is performed on HW hole).

But some machinists I talked to say that the depth should have been "Value @ Center of CB" not min or max.

Hope this clarifies.

 

[ctopher]

It should be a nom depth by default. Then dim it on the dwg with tol.
But, depending on your design, it could be called out as min or max. I don't know what the CB is used for.
Create your holes, make a sect view, then dim dia and depth.
Your callout looks good to me. Draw a centerline thru the center of the hole on the dwg. The machinist should never have a problem with it.
I hope I understood you correctly and I made sense.

Chris
Systems Analyst, I.S.
SolidWorks/PDMWorks 05
AutoCAD 06
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[ewh]

The problem with measuring from the center is that the center point no longer exists when inspecting. The machinist may want to machine it that way, but I would get the opinion of an inspector as to how it should be called out on the drawing.
This is one of those situations that are not always covered by today's cad packages.

 

[wes616]

Look at your application to determine how to best dim the CB... for example

1. The CB is for a socket head cap screw, and you do not want the head exposed, well then, a Min Depth will be your guide.

2. You are using the CB to fit a bushing. You don't require an amt lenght of bushing, but you must maintain a minimum wall thickness on the machined part... then you should specify a max depth, and trim the bushing.

there are numerous examples where only experience will tell you which way to go... but hey, that why we get paid the Big Bucks right?

Wes C.
------------------------------
When they broke open molecules, they found they were only stuffed with atoms. But when they broke open atoms, they found them stuffed with explosions...

 

[GunT]

I am sorry if I created any confusion by calling min. and max. depth. I am not talking about "Tolerances". And I definitely understand " Design Intent" and know how to accomplish it.

My question relates to a depth callout of a "Variable Depth CB hole" and how does one interpret it.

I have obtained 3 different answers and unable to find a standard definition of depth in case of a variable depth hole.

Here are the three answers:

1. Depth is measured from the point where a full cylinder of the feature is defined aka Min Value of the depth ( Not tolerance).

2. Depth is measured from the center of the CB hole cause it is to where the location of the hole is measured.

3. Depth is measured from the point the probe makes initial contact aka Max value of the depth.

So my questions are "If I specify the CB depth (of a variable depth hole)o n my print how is the machinist/inspector going to interpret it? Min value, Max value or the Mean value. Or the callout incomplete without a section view? And what standard defines it and where can I find it?"

I appreciate the discussion guys. Thanks a lot.

 

[MadMango]

If you use a section detail of the hole as ewh stated there is no room for misinterpretation.

[green]"I think there is a world market for maybe five computers."[/green]
Thomas Watson, chairman of IBM, 1943.
Have you read faq731-376 to make the best use of Eng-Tips Forums?

 

[MikeHalloran]

The logical way is to use the section view, and dimension not to the angled surface, but to the feature behind the hole that's most likely to be used to support the part while milling the cbore. That way the quill stop depth setting doesn't have to change for parts with variations in location of the angled surface.



Mike Halloran
Pembroke Pines, FL, USA

 

[GunT]

MadMango,

I agreed to it already. I am asking about the scenario where the section view was not created. How does one deal with such situation?

Is the callout completely illegal without a section view or section view just adds clarity to drawing. IMO both are completely different scenarios. And I am looking for Standard which addresses the issue.

Regards

 

[ctopher]

You can not call out a variable depth CB. If you did, you could get anywhere from a spot face to a thru hole. Call out one depth with a tol.

Chris
Systems Analyst, I.S.
SolidWorks/PDMWorks 05
AutoCAD 06
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[ajack1]

I agree with Mike Halloran, easy to understand and everything you need to know, what could be easier?

 

[MikeHalloran]

Okay, you _could_ adopt a _local_ standard saying, e.g., the depth of the cbore is measured from the theoretical intersection of the hole axis and the surface that it penetrates.

One problem becomes apparent immediately, even beyond the nonexistence of your datum:

- The usual tools for measuring cbore depth intrinsically assume the existence of a datum surface normal to the hole axis.

The problem gets worse if your angled surface is also nonplanar.



Mike Halloran
Pembroke Pines, FL, USA

 

[TheTick]

Dimension in a section view. Specify depth at either maximum or minimum depth. Keep tolerance such that one can check with a scale (nearest +/-.015" should do), as it is likely a caliper or depth mic will give an erroneous reading due to the incline and curvature.

 

[GunT]

Initially what MikeHalloran said in his first post looked like a great solution. But it does not address the issue in all cases.

What if I take away the vertical surfaces i.e. that if I have a part shaped like a rhombus or a parallelogram then my problem surfaces again.

Also if ones dimensions like MikeHalloran asks, then one can accumulate the tolerances! And you will loose design intent.The problem is not just restricted to CB holes but can include tapped holes also.

Whats scary is that I was not able to find a theoritical definition of the depth of the CB hole anywhere in the literature so that I can extrapolate.

Yes I can make my "Local standard". But the problem is it will be not be interpreted like that in all cases and I have to communicate the standard each and every time. And that really baffles me cos this should be part of the standard literature somewhere. I don't think this is a trivial issue. And I really appreciate the discussion.

Regards,

 

[MikeHalloran]

It isn't covered in the literature to any depth (no pun intended) because putting a counterbored hole in an inclined surface kills your manufacturability. You can't use a standard counterbore, piloted in the through hole, because the side loads will break the tool; you have to mill the counterbore. Which I guess makes it a milled pocket, not a counterbore at all.

Why would anyone devote any effort to producing a standard for a bad practice?



Mike Halloran
Pembroke Pines, FL, USA

 

[GunT]

So a CB hole on an inclined surface need to be milled and is no CB any more. I never knew this. I am taking your word for it.

But what about a threaded hole. Is it still called a threaded hole?

Thanx for the info