calling out bolt circles

[BODIE]

Following ASME Y14.5M standards is it ok to call out bolt circles with the hole call out example 12X 1/4-20 THD THRU
ON A 12.00 DIA B.C.
It only shows it being called out seperate in the book and I have 5 different bolt circles on a 9.5 dia part. If I call them all out seperate I'm afraid it will be to cluttered. Thanks

 

[ewh]

Bodie,

Though it is not specificaly addressed in the standard, it is common practice to call out bolt circles in this manner, except that you should also specify if the holes are "EQUALLY SPACED" with one hole located angularly or "SPACED AS SHOWN" with the relative angular dimensions included.

i.e. 12X 1/4-20 UNC-2B THRU
EQ SP ON <dia>12.00 BC

or 12X 1/4-20 UNC-2B THRU
EQ SP AS SHOWN ON <dia>12.00 BC

Note that "THD" is not required (would actually be redundant), but thread type and class should be included.

Hope that helps!

Eric

 

[ewh]

OOPS!

In the above post, "12X 1/4-20 UNC-2B THRU
EQ SP AS SHOWN..."

should read "12X 1/4-20 UNC-2B THRU
SP AS SHOWN..."

 

[drawoh]

BODIE,

I do not like the idea of writing out a note on a drawing, especially a CAD drawing where you were careful to draw everything to scale. This is particularly true of drawings generated using parametric CAD programs like SolidWorks, where someone might change the model and assume that all the drawings updated okay.

The usual ASME Y14.5M dimensioning procedure is to draw a broken-line circle through the holes and apply a diameter dimension to it. I believe this is called a pitch circle. Then, you show an angle between two of the holes and indicate the number of angles and holes. In a six hole pattern, your dimensions are...

<dia symbol>12.000
6 X 60<degrees>
6 X 1/4-20UNC-2B THRU

3D parametric CAD is a complete waste of time if you are not using their built-in dimensioning features.

JHG

 

[ewh]

drawoh,

I agree with you about avoiding non-associative notes on CAD drawings and the USUAL dimensioning procedure, but your example doesn't fully solve the problem. Bodie is concerned with cluttering his drawing (a sign of a good drafter).

Following your example, nothing prevents the dimension from being incorrect if one of the holes is clocked other than 60 degrees after the drawing is created. The only way to avoid this would be to dimension each angle, thus you would have 6 separate degree dimensions defining your hole pattern. You would also have to dimension each hole separately, in case someone decided that one of the holes should be of a different size. Of course, in trying to create a fully associative document, you end up with a cluttered, hard to decipher drawing. In creating a concise, easy to interpret drawing, some shortcuts are necessary and desirable. It is not a requirement of ASME Y14.5-1994 to fully define each and every feature and location separately, or it wouldn't allow for "X" to denote the number of places.

I have not been "careful to draw everything to scale" since I was on the drawing board. That is part of the function of the software. I do model everything to scale, but that is the only way to create a valid model.

There are ways to call out the bolt circle in a note that are associative. I suppress the leader line when dimensioning bolt circles, add the “EQ SP ON” and "BC" notation and move the dimension below the hole callout, resulting in an associative "note" type of callout that you recommend against. Do you add separate diameter and depth dimensions for counterbored holes (I do, using the same method as for BC)? How do you ensure that a tapped hole is UNC and not UNF? How about the angle of a countersunk hole? Having to show all of these details separately can result in a five page drawing vs a one page drawing.

You should never assume that your drawing is correct after updating your model. Granted, if care is taken in your dimensioning, mistakes should be minimal, if any.

I'm sorry to rant about this, but I feel that some shortcuts are necessary in complex drawings. The intent is to create an accurate, CONCISE definition of a part, something easily understood by the fabricator of that part.

Eric

 

[drawoh]

ewh,

When you typing notes in SolidWorks, you can click on dimensions and embed them in your note. This makes for nice neat notes with embedded parametric dimensions. I can create parametric thread specifications, at least with metric threads. I assume that ProE and other 3D CAD programs have similar capabilities.

I agree with you about keepting drawings neat, but we need a rigourous process for applying and maintaining the dimension values too. Applying the pitch circle dimension and the angle does not protect you if someone decides to "key" the bolt circle so that there is only one way to assemble the part, but applying each angle would mess up the drawing too much.

Written out notes require the reader to speak English. The ASME Y14.5M notation is independent of language. I believe that this was their intent.

JHG