Be careful of the electrical performance if your customer has
the thicknesses on the print. Are you doing the assembly? Look
for some of these clues (if it is a digital board):
oscillator components over 50mhz
single resistors from 10-60 ohms
resistors in pairs at 100's of ohms
resistors paired with capacitors
logic devices of FCT, HCT, ABT, 10K, 100K, 10H or any fast proc-
cesor chip (I probably missed some)
If some of these are present the customer may be making a specific
electrical performance without buying expensive impedance controlled
boards. Even if it is not exact impedance they may want to make
sure all lots have the same electrical characteristics, there is
a noticeable difference in what your fabricator suggests.
To make a specific electrical performance (impedance) the copper
thickness is also specified. The best way to check that is to cut
a board and measure.
It may be that the fabricators's suggestion will work but the
values of the resistors you found above may need to change.
Sorry I can't help much about the warping!
Good Luck, and Best Regards,
Jeff Seeger Applied CAD Knowledge Inc
Chief Technical Officer Tyngsboro, MA 01879
[log in to unmask] 508 649 9800
---------------------------------------------------------------------------
From: SMTP%"[log in to unmask]" 9-MAY-1996 18:36:58.82
To: Poh Kong Hui <[log in to unmask]>
CC:
Subj: Re: FAB: PCB Fabrication Drawing.
It means your PCB fabricator is trying to encourage you to build the PCB
with materials that are either lower cost to them or currently in their inventory.
Another way of saying this is they may have 'standardized' on this construction
to get volume pricing on these materials.
From:
--------------------
.4 mm thick
--------------------
.6 mm thick
--------------------
.4 mm thick
--------------------
To:
--------------------
.11mm x 2 (2 plies 2116 or?)
--------------------
1.0 mm (core)
--------------------
.11mm x 2 (2 plies 2116 or?)
--------------------
Your fabricator would like to construct this with 2 plies of 2116 (or similar) prepreg
on each side of the 1.0 mm thick innerlayer core (L2/L3). If 1/2 oz copper is used
throughout, the total thickness would be 1.51mm over outside copper, after lamination,
but before plating. Can your design tolerate the difference in dielectric spacing?
This suggested construction may cost less for this PCB maker if he doesn't carry
an inventory (or get good pricing) on 7629 prepreg. 2 plies of 7629 on each side of
a .6mm core should provide the originally desired construction spacing at about the
same cost.
Fred J. Paul, Sr. Process Engineer
PCB Operations, FLUKE CORPORATION
direct: 206 356-5734 fax: 206 356-6070
[log in to unmask]
On Thu, 9 May 1996 09:29:52 -0700 Poh Kong Hui wrote:
> From: Poh Kong Hui <[log in to unmask]>
> Date: Thu, 9 May 1996 09:29:52 -0700
> Subject: Re: FAB: PCB Fabrication Drawing.
> To: [log in to unmask]
>
> Dear Technet,
>
> I hv an issue with a 4-layers boards. I am not sure what my customer's
> requirement, because I am not familar with PCB fabrication. Pls escuse me.
> >From the fab diagram, this is one of the drawing what being showed.
>
>
> Customer's Requirement: ______________
> 0.4
> --------------
> | 0.6 |
> --------------
> 0.4
> --------------
>
>
> PCB supplier's recommendation: ______________
> 0.11 x 2
> --------------
> | 1.0 |
> --------------
> 0.11 x 2
> --------------
>
> Could anybody can explain to me what it means ? And what the differecnce
> between the cust's requirement & the supplier's recommendation in term of
> board processing and also when come to PCB assembly.
>
> And could anybody tell me how to determine the PCB inner & external copper
> thickness. I realise some of our boards, of same model, but differ in
> weight & thickness, and sometimes twist after reflow from batch to batch.
>
> Thks and Regards..
>
> Poh Kong Hui
> Nera Electronics
> Email: [log in to unmask]
>
|
