[PCB_FORUM] Re: Multi-layer stackup design

This stuff we call FR-4 has a breakdown voltage of 1100 Volts per mil of
thickness, so 2 mils would work for 1500 Volts DC.  However, copper
protrusions between copper layers often reduces the thickness to as
little as a mil.  As a result, we don't like to use laminates and
prepregs that are less than 3 mils when we have this spec.

 

As to airgap for this voltage, through the air the minimum spacing is 2
mm or 80 mils and over the surface of a PCB it is 2.8 mm or 224 mm.
Hope this helps.

 

Jelena

 

 

________________________________

From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Jose Magnaye
Sent: Tuesday, February 21, 2006 8:56 PM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: Multi-layer stackup design

 

 

Yes, our standards specify at least 0.41mm if using a core material
(laminate).  If less than or equal to 0.40mm then we need to specify 3
layer prepreg (sorry for the wrong spelling before) but there were no
minimum thickness specified.  

 

After asking several vendors we also found out that there are no
published dielectric breakdown voltages for prepreg materials so we
cannot compute for the minimum.  Of course we can always use the 2.0mm
PCB thickness but without proper justification ( i.e. literature or
computed values), how can we convince our sales dept and the customer to
go with the higher PCB price?


BTW, is this Off-Topic?  Are we allowed to discuss things like these
here?

 

- JM
 

On 2/22/06, richard moffat <richard.moffat@xxxxxxxxxxxxxxxxxxx> wrote: 

0.2mm?  Possibly  (dare I say probably without any legal ramifications?)


 

The kind of spec it looks like you're referring to calls for 0.4mm.
However, that figure is negotiable.  Creepage distance on the outer
layers is more troublesome. 

 

You're certainly doing the right thing by layering more than one
prepreg.

 

 

 

  
__________________________
Richard Moffat
PCB CAD Manager
Allied Telesis Labs
ph. +64 (3) 3393000
richard.moffat@xxxxxxxxxxxxxxxxxxx


>>> josemagnaye4@xxxxxxxxx 22/02/2006 3:51:48 p.m. >>>
 

Hi Claude

 

We're trying to design it to be as generic as possible since we will be
using several vendors.  They can define which materials they can use for
the prepeg but the stackup design should be fixed.

 

Basically what we are trying to determine if 0.2mm thickness will be
enough for the 3 layer prepeg to withstand at least 1.5KV.

 

On 2/22/06, Claude Meyers <claude.meyers@xxxxxxxxxxxxxx > wrote: 

This is a question you should be asking your fabrication house. Every
PCB Fab house has different requirements. 

 

________________________________

From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Jose Magnaye
Sent: Tuesday, February 21, 2006 6:00 PM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Multi-layer stackup design

 

Hi!

 

We are designing an AC-DC power supply on a 4 layer board and we are
currently looking at any literature on how to design the stack-up.  

 

Some of our primary and secondary tracks overlap and we were told that
we can let them overlap as long as we use 3 prepeg layers in between.
Unfortunately, we cannot find any info on the minimum allowed thickness
of the 3 layers.  

 

We are concerned with the thickness since we will be using a 1.6mm 4
layer FR4 board with 2 Oz copper on all layers.  

 

JM

 

 


 


NOTICE: This message contains privileged and confidential
information intended only for the use of the addressee
named above. If you are not the intended recipient of
this message you are hereby notified that you must not
disseminate, copy or take any action in reliance on it. 
If you have received this message in error please
notify Allied Telesyn Research Ltd immediately.
Any views expressed in this message are those of the
individual sender, except where the sender has the
authority to issue and specifically states them to 
be the views of Allied Telesyn Research.

Other related posts: