Hello all,
        Chris Jorgensen at IPC passed on the following question stated below
from Hillel Dzigen concerning a problem with the D-249. The specification
referenced is the Design Standard for Flexible Single and Double Sided
boards. The paragraph referenced within the 3.6 Mechanical considerations
section stated as "rigid reinforcement" is actually referring to what is
more commonly known as "stiffeners".  What the design parameter is
attempting to communicate has to do with producing the clearance holes in
the rigid stiffener material large enough to clear the lands(pads).  The
stated value in question references to the flex hole size instead of the
land size; the 0.014 inch (0.36 mm) clearance makes assumptions of the land
having an annular ring of less than .007 inches (0.18 mm) as to clear the
land.  This value actually does not give any allowance for registration
except that by default the smaller the annular ring the less likely to cover
the pad with the material.  This produces a conflict within itself, as you
noted with the confusion. One of the most critical aspects is to not overlap
the land area with the rigid stiffener material and allow adequate clearance
for the component leads and solder fillets.

        In the not yet released (Interim Final)of IPC-2223 Design Standard
for Flexible Printed Applications it is handled differently and summarized
as follows:
        Paraphrased from 5.2.10 Stiffeners and Heat Sinks. The designer
needs to:
1.      Shall state Material type, size, thickness, and adhesive type on the
Master Drawing.
2.      Shall state hole size and registration requirement on the Master
Drawing.
3.      Stiffener Should be at a minimum of 0.25 mm larger than the land to
allow for registration.
4.      The edge of stiffener next to the flexible section Should be
chamfered or filleted to prevent damage to the flex.

        Typically, you would size the holes in the stiffener to the maximum
allowed and still retain a safe web between the holes.  For example a
connector on 2.54 mm centers would have a maximum hole of 2.16 mm to keep
from breaking out.  In some cases on close center footprint components the
designer may want to slot the opening around the hole pattern grouping to
provide clearance.  The registration allowance will have to be calculated
from the worse case design condition.  Start with .2 to .25 mm T.P. at MMC
and work into it to determine if a though hole or slot makes the best
condition.

        Hope this helps clear this up.  Soon we hope to have the new Flex
Design guide out.

        Don Dupriest
        Lockheed Martin Vought Systems
        Dallas, Texas


        Mr. Dzigan wrote:
        > In your document IPC-D-249, Paragraph 3.6.4.4. you state:
"Interior holes in reinforcement should be at least 0.014" larger in
diameter than the corresponding holes in flex circuit for registration
allowance." We assume that when no diameter of hole is designated on rigid
reinforcement, the above is valid. Our question is: Since no maximum
diameter is stipulated, may the manufacturer of the board use any diameter
he wishes (i.e. 10 times that size, 0.14" or more) or does the inference
reflect 0.014" min. up to normal registration allowance? If so, what would
be normal registration allowance?

        In other words: What should be the maximum reinforcement's  holes
size if no maximum is define on the circuit drawing?

        Hillel Dzigan - Quality Manager
        Eltek Ltd.
        Phone +972-3-939-5022, Fax +972-3-930-9581
        P.O. Box 159, Petach-Tikva 49101, ISRAEL

        ################################################################
        TechNet E-Mail Forum provided as a free service by IPC using
LISTSERV 1.8c
        ################################################################
        To subscribe/unsubscribe, send a message to [log in to unmask]
<mailto:[log in to unmask]>  with following text in the body:
        To subscribe:   SUBSCRIBE TechNet <your full name>
        To unsubscribe:   SIGNOFF TechNet
        ################################################################
        Please visit IPC web site (http://jefry.ipc.org/forum.htm
<http://jefry.ipc.org/forum.htm> ) for additional information.
        For technical support contact Hugo Scaramuzza at [log in to unmask]
<mailto:[log in to unmask]>  or 847-509-9700 ext.312
        ################################################################

################################################################
TechNet E-Mail Forum provided as a free service by IPC using LISTSERV 1.8c
################################################################
To subscribe/unsubscribe, send a message to [log in to unmask] with following text in the body:
To subscribe:   SUBSCRIBE TechNet <your full name>
To unsubscribe:   SIGNOFF TechNet 
################################################################
Please visit IPC web site (http://jefry.ipc.org/forum.htm) for additional information.
For technical support contact Hugo Scaramuzza at [log in to unmask] or 847-509-9700 ext.312
################################################################