I hate to 'chime in' on this one, because I know it can be a bit controversial, 'BUT'... Here's the philosophy... for what it's worth.

We all know fabricators that can make boards without a drill or fabrication drawing.... all the critical questions can be answered over the phone, hole sizes and patterns, silk screens solder masks, etc, all are in the CAD data supplied... And you can successfully make a proto board for use in the LAB that way...

That being said, The PROBLEMS arrive when you need to INSPECT what is being received in the door for production. The QA inspector has to decide, 'Is this CONFORMING material or REJECTABLE material?'  How does he or she determine that?

He or she does this by reading your Drill/Fabrication drawing.... (oops)

If the Inspector sees a NO TOLERANCE Drawing or (no drawing at all) and there is NO qualifying reference to a controlling spec... All dimensions are absolute, +/- .000 ( ergo, not possible to verify )

In that case, It's up to the Material Review Board (MRB) to make a determination on whether or not they accept/reject the material based on their knowledge of the design and its application. However this is an unacceptable situation to have to put hundreds of boards through the MRB on a regular basis and it's risky because the boards are not being inspected...

I have seen old fab drawings that have no dimensions on them... The Quality Assurance Inspector will not inspect any feature of the board that is not dimensioned with a tolerance.

Most of us use a note in the notes block that refers the inspector to the controlling method of interpreting the drawing... i.e. Drawing to be interpreted per ASME Y14.5 etc...

On the other hand, IF I was a PCB manufacturer bidding a board design, putting the shoe on the other foot, I would send a "NO BID" on a board that has no tolerances because there is not a shop in existence that will be able to get it exactly on the dimension...as specified by the drawing.  There will always be a tolerance to take into account.

The designer needs to set those tolerances based on the knowledge he/she uniquely has in their possession having designed the board to fit in an enclosure of some sort, and make them as liberal as reasonably possible so that if the material comes in the door at the min or max it will still fit and function as designed. The designer has 'done their homework' and really spent the time to pay attention to detail and made a producible, INSPECTABLE product when they do this sort of a tolerance study and specify the appropriate tolerance on the dimensions.

Here are a set of the notes I use on my boards, Hopefully the design in question made some references to some of the IPC specs mentioned and has cover the bases somewhat...

NOTES: UNLESS OTHERWISE SPECIFIED,

1.      INTERPRET DRAWING, DIMENSIONS, AND TOLERANCES PER ANSI Y14.5M. DIMENSIONS ARE IN INCHES [MM].
2.      MATERIAL: 2 SIDED COPPER CLAD PLASTIC SHEET PER IPC-4101 TYPE GFN, NEMA FR4

LAMINATE USING PRE-PREG MATERIAL PER IPC-4101, TYPE PC-GF

MANUFACTURE IN ACCORDANCE WITH 1PC-6012A, TYPE 3, CLASS 2.

EXTERNAL LAYERS SHALL BE 1 OZ. (.0014 IN [0.035mm]) COPPER

BOARD THICKNESS TOLERANCE SHALL BE  +/- .007 IN. [.18 MM].

SEE STACK UP DETAIL FOR LAYER CONFIGURATION.

ALL LAYERS VIEWED FROM THE PRIMARY (COMPONENT) SIDE

3.      UNLESS OTHERWISE SPECIFIED ALL HOLE DIMENSIONS APPLY AFTER PLATING.

ALL PLATED THRU HOLES SHALL BE IN ACCORDANCE WITH IPC-6012 AND HAVE

A WALL THICKNESS OF .0008 IN  [.020mm] TO .0012 IN [.035 MM]

ALL HOLES SURROUNDED BY A LAND SHALL HAVE A MIN ANNULAR RING OF .002 IN [0.05mm]

LAYER TO LAYER REGISTRATION SHALL BE WITHIN .003 IN. [.08 MM]

4.      ALL HOLES SHALL BE LOCATED WITHIN A DIAMETER OF .006 IN [.15 MM] OF TRUE POSITION AS SUPPLIED IN CAD DRILL DATA
5.      FINISHED BOARD TO COMPLY WITH IPC-A-600E, CLASS II.
6.      FINISHED CONDUCTOR WIDTHS AND SPACINGS SHALL BE WITHIN 10% OF SUPPLIED ORIGINAL CAD DATA.
7.      BOW AND TWIST SHALL NOT EXCEED 0.75% (.00075 IN PER IN) IN ACCORDANCE WITH IPC-A-600F FOR SURFACE MOUNTED BOARDS WHEN MEASURED USING IPC-TM-650, METHOD 2.4.22.

8.      FINISHED BOARD SHALL MEET THE REQUIREMENTS OF UL796 WITH A FLAMABILITY RATING OF UL 94V-0 OR BETTER. VENDOR'S UL LOGO AND/OR DESIGNATION AND DATE REQUIRED, TO BE LOCATED ON THE SECONDARY (SOLDER) SIDE OF THE BOARD.

9.      MAXIMUM RADIUS ON ALL INSIDE SHARP CORNERS TO BE .063 IN [1.6 MM]
10.     SOLDERMASK LPI OVER BARE COPPER PER IPC-SM-840, TYPE B, CLASS 2, COLOR: TRANSPARENT GREEN. ALL EXPOSED CONDUCTIVE SURFACES TO BE DIAGONAL HASL (HOT AIR SOLDER LEVELED) AFTER SOLDERMASK.

11.     SILKSCREEN LEGEND(S) USING WHITE NON-CONDUCTIVE EPOXY BASED INK AS REQUIRED BY CAD DATA.
12.     ISOLATED OR UNUSED INTERNAL PADS MAY BE REMOVED AT MANUFACTURER'S DISCRETION.
13.     COPPER THEIVING ON EXTERNAL LAYERS IS ACCTEPTABLE FOR UNIFORM PLATING OUTSIDE THE BOARD AREA.
14.     TENTING OF VIAS IS PERMISSIBLE TO CONFORM WITH CAD DATA.
15.     BARE BOARD ELECTRICAL TEST IS REQUIRED. VENDOR TO SUPPLY CERTIFICATION OF BOARD CONTINUITY BASED ON CAD DATA SUPPLIED.

16.     SEE SHT 2 FOR PANELIZATION DETAIL.

The tolerance block on our drawings indicates the following.

Finished Hole diameter / Tolerance

.014 - .185     +.003/-.002

        .188 - .246             +.004/-.002

        .250 - .750             +.005/-.002

        .765 - 1.000    +.007/-.003

        1.015 - 2.000   +.010/-.004

        2.031 - 3.500   +.015/-.005

Dimensional Tolerances

.XXX    = +/- .005

 .XX    = +/- .010

.X  = +/- .020

Any other specific tolerance is noted in the dimension area and specified for that specific controlled feature.

IMHO the Fab drawing is the most important tool a company has to protect the quality of the PCB and product that it goes into. I think Kelly Dack has lectured on the importance of this subject at PCB WEST before. I try to remind the other designers that I meet that if you don't dimension and tolerance a feature, don't expect to get it inspected. Some times failing to dimension a feature can bite you in the rear when process variances go to their extremes and a part that used to fit and work in the Lab fails to work on the production floor 60% of the time. Expect to get a lot of flack for failing to specify the tolerance on the face of the drawing after all, you are the designer!  The company depends on you to avoid placing it in financially liable situations... the Fab drawing is the only thing you have to CYA... (protect your assets)

Hope that helps a bit... (steps down from his soapbox)

Bill Brooks, CID

-----Original Message-----
From: Tom Garman [mailto:[log in to unmask]]
Sent: Thursday, June 05, 2003 9:22 AM
To: [log in to unmask]
Subject: Re: [DC] IPC PCB Dimensioning standard

Barry;

I have looked at the specs that I have and could find anything about

"implied" tolerances. I do not have a complete set of specs though.

In my experiences we have always called out a default tolerance. Usually

.XXX = .005, .XX = .1

Tom Garman

PCB Designer

330-575-1636

[log in to unmask]

-----Original Message-----

From: DesignerCouncil [mailto:[log in to unmask]] On

Behalf Of Barry Gallegos

Sent: Thursday, June 05, 2003 10:35 AM

To: [log in to unmask]

Subject: [DC] IPC PCB Dimensioning standard

Good morning,

My Name is Barry and I have been asked to locate some information. As I

have

had great

experiences with TechNet, I thought I would Give the Designer Council a

Try.

So here goes.

I ask for some input on the following Message that I received this

morning.

We have an issue on a customer drawing, where the customer calls out

dimensioning on their data, to 3 decimal places, but do not provide a

tolerance table or tolerance indication at all. The exact method the

customer used to call-out dimensions on their drawing is: 250Mils or

530Mils

for example. The pcb shop that built these is saying that, in the

absence of

having a tolerance call-out, they default to IPC standard tolerance. The

customer service person at the pcb shop, cannot tell me which standard

he is

referring to, nor can he tell me what that default IPC standard

tolerance

might be. We do not have the 2221 IPC design standard nor do I know if

it

would cover this issue. We have issue with the dimensions of these pcbs

we

received, including hole positions.

Can you find out what the IPC default tolerance is for dimensioning of

pcbs,

in the absence of having a specific tolerance call-out?

Barry Gallegos

Western Electronics

------------------------------------------------------------------------

---------

DesignerCouncil Mail List provided as a free service by IPC using

LISTSERV 1.8d

To unsubscribe, send a message to [log in to unmask] with following text

in

the BODY (NOT the subject field): SIGNOFF DesignerCouncil.

To set a vacation stop for delivery of DesignerCouncil send: SET

DesignerCouncil NOMAIL

Search previous postings at: www.ipc.org > On-Line Resources & Databases

> E-mail Archives

Please visit IPC web site http://www.ipc.org/html/forum.htm for

additional

information, or contact Keach Sasamori at [log in to unmask] or 847-509-9700

ext.5315

------------------------------------------------------------------------

---------

---------------------------------------------------------------------------------

DesignerCouncil Mail List provided as a free service by IPC using LISTSERV 1.8d

To unsubscribe, send a message to [log in to unmask] with following text in

the BODY (NOT the subject field): SIGNOFF DesignerCouncil.

To set a vacation stop for delivery of DesignerCouncil send: SET DesignerCouncil NOMAIL

Search previous postings at: www.ipc.org > On-Line Resources & Databases > E-mail Archives

Please visit IPC web site http://www.ipc.org/html/forum.htm for additional

information, or contact Keach Sasamori at [log in to unmask] or 847-509-9700 ext.5315

---------------------------------------------------------------------------------