4 layer PCB (from 2 layer) + array of designs on one board

Do you have a question? Post it now! No Registration Necessary

Translate This Thread From English to

Threaded View


Hello,

My appplication is light detection -> using photodiodes and
transimpedeance amplifier (OPA657 from Texas Instruments). At this
point I have 2-layer working design. I need to increase the bandwidth
of the detector (from 10MHz to 40MHz) and try to reduce noise (also
reducing noise is always welcome, of course). I'm thinking about using
two inner layers for +5V and -5V power layers (I'm using free space on
top and bottom layers for ground layer). +-5V is currently connected to
the board from external power supply by soldering two wires (one for
+5V and one for -5V). I am using +-5V to bias photodiodes and to power
the opamp. The software I'm using is OrCAD. Even if going to 4 layer
from two wouldn't give me a significant improvement in terms of
reducing the noise level, I would like to know the answers for the
following questions.

1) Will traferring +-5V to separate layers (rather than just have the
power traces with filters) work? Since the inner layer is most likely
to be .5oz copper as opposed to 1oz copper of outer layers. There is no
way to specify that in gerber file, right? Will creating a power layer
give me more stable voltage (and high capacitance)? That's why people
are using multilayers as opposed to two layers, right? I guess I will
still need some decoupling capacitors at the vias.


2) The price differential between 2 and 4 layer boards is quite steep,
and I can easily fit a few prototype boards on one board and then cut
them (or have it cut by manufacturer). What is the easiest way to place
array of differemt designs on one board? I only have access to OrCAD,
but it can generate gerber files, so maybe some other software can be
used. Are the manufacturers ok with this? I would prefer them to cut
the boards, if possible, since I probably wouldn't be able to do it as
well without special equipment. (Something tells me they woudn't be
willing to make x by x board, and then cut it in y pieces, but just
checking). I do realize I might be able to place three designs side by
side and not require any cutting, but that might not always work for
me.

Merry Christmas,
Vitaliy


Re: 4 layer PCB (from 2 layer) + array of designs on one board



Quoted text here. Click to load it
single sided Ceramic daughter board for the OP-AMP and INPUT?
Also a hole in the board so that the chip is suspended via the
rails and output legs only also may help. I did something like that
years ago to remove the cap around the structure.


--
"I'm never wrong, once i thought i was, but was mistaken"
Real Programmers Do things like this.
We've slightly trimmed the long signature. Click to see the full one.
Re: 4 layer PCB (from 2 layer) + array of designs on one board


All components are smt (except for photodiodes). I also have the
components (resistors and capacitors) placed on both bottom and top
layers (2 layer board), with opamp being on the top layer. Top and
bottom are just relative terms in my case.


Vitaliy

Jamie wrote:
Quoted text here. Click to load it


Re: 4 layer PCB (from 2 layer) + array of designs on one board



Quoted text here. Click to load it

Gerber files only specify the copper patterns that are to appear on
the board.  Any other construction details, including copper weight,
and the order of layers on a multi-layer board, must be specified
separately.  I have a standard format for a text file that includes
such information.

When laying out a multi-layer board, you should put a wide track at
the edges of the board on the power or ground plane layers to keep the
copper on those layers away from the edge of the board.  (Anything you
place on a plane layer will end up as "no copper" on the finished
board.)
Quoted text here. Click to load it

Discuss the matter with your board shop.  If I have two or more boards
that I want built on a common panel, I'll usually produce separate
gerbers for each board, then ask the board maker to combine them on a
single panel.  However, a co-worker places multiple boards on a panel
himself, and sends gerbers for the full panel to the board shop.
Either way, the board shop will separate the individual boards if
asked.  If you panelize the boards yourself, you should first ask the
board shop what separation they want between boards - they need some
unused space to leave room for the router bit to go between boards.

Quoted text here. Click to load it

--
Peter Bennett, VE7CEI  
peterbb4 (at) interchange.ubc.ca  
We've slightly trimmed the long signature. Click to see the full one.
Re: 4 layer PCB (from 2 layer) + array of designs on one board


Quoted text here. Click to load it
I think I'm missing something: should I leave some space between the
edge of the board and power plane (which will be internal plane)?


Quoted text here. Click to load it
OK, I will look into panelizing the boards myself (also I would like to
panelize different designs (same # of layers though) on the same
board). If you can suggest a program that can take two gerber files and
create one board will be great (I'll check if this can be done in
OrCAD).


PS. I will respond to other suggestions a bit later on today.

Thanks a lot,
Vitaliy


Re: 4 layer PCB (from 2 layer) + array of designs on one board



Quoted text here. Click to load it
Yes.  If you let the copper on the planes extend to (and beyond) the
edge of the board, you may get short circuits between planes or
between a plane and a metal card guide.
Quoted text here. Click to load it

I use Protel, which does allow cutting-and-pasting from one board
design to another, or within a board design.  When I make a panel,
I'll finish all the board designs in individual files, then copy and
paste them into a new blank design.  In Protel, when pasting designs,
you have to use a "Paste Special" command, and tell the program to
permit duplicate reference designators - otherwise Protel will
re-number components on the second and later boards.

--
Peter Bennett, VE7CEI  
peterbb4 (at) interchange.ubc.ca  
We've slightly trimmed the long signature. Click to see the full one.
Re: 4 layer PCB (from 2 layer) + array of designs on one board


Quoted text here. Click to load it

The power planes on 4 layers boards are more useful for high switching
current and high speed digital stuff. There is a good chance it may
make little or no difference for application depending on your layout.
4 layers will give you greater ability to achieve a lower noise layout,
but if you don't know exactly how to achieve this then it's not going
to help you much, it could even make things worse, I have seen that
happen before.

Quoted text here. Click to load it

Simply ask the manufacturer to do it, do waste time and effort
yourself. Just supply them the layout for one board and tell them you
want X number of boards. For the prototype services they will usually
fit as many as they can on the one panel for you, you pay per panel.

For high production designs it's usually different, you have to worry
about panel handling and tooling hole/marks etc.

Quoted text here. Click to load it

Some manufacturers will do up to say 3 different designs on the one
prototype panel for you, if that's what you want.

Dave :)


Re: 4 layer PCB (from 2 layer) + array of designs on one board


Quoted text here. Click to load it
To start off, I will read you tutorial from pcb123 and hopefully
improve a few things in my design from that manual. I want to add the
power layers to reduce the length of power traces (I might need to add
the 2nd stage to the detector, and that will definitely require
more/longer power traces without power layers).
Quoted text here. Click to load it
Any recommendations, I'm using pcbexpress, will try to get a hold of
them after New Year's day, local manufacturers are charging per panel
(but I will see if they can put a few designs on the same panel).

John Devereux wrote:
Quoted text here. Click to load it
What I meant was: I must increase the BW but see if there is a way to
reduce the noise (it does not have to be less than what I have right
now).
I was thinking differently: if I can provide more stable voltage to
both opamp and photodiodes, I can get less fluctuations during current
generation and amplifications and power plane should give more stable
voltage, right? (I can be totally wrong about this)

John Larkin wrote:
Quoted text here. Click to load it
I'm using InGaAs PIN (Small Area/Fiber-Optic) photodiodes, which
according to the datasheet should be biased at 5V, wavelenth of the
signals varies between 800nm to 1700nm. NEP of the photodiode is <0.02
pW/sqrt(Hz) @1550nm according to the datasheet.


Vitaliy


Re: 4 layer PCB (from 2 layer) + array of designs on one board



Quoted text here. Click to load it

These requirements tend to be mutually exclusive... i.e., more
bandwidth lets in more noise.

What is the source of the "noise"? E.g. source noise, photocurrent
shot noise, transimpedance amplifier noise, external interference?

Until you do this it seems pointless to speculate about numbers of
layers in boards.

<SNIP>

Quoted text here. Click to load it


--

John Devereux

Re: 4 layer PCB (from 2 layer) + array of designs on one board



Quoted text here. Click to load it

More layers won't necessarily improve speed or reduce noise. If you
increase trace capacitance (from thinner dielectrics) it might make
things worse.

10 or even 40 MHz isn't very fast for a photodetector; I've got 180
MHz from cheap opamps. What detector device are you using? Increasing
the photodiode back-bias should help speed a bunch, maybe 2:1 if you
go from 5 volts to something like 20.

What's the application? How much noise do you see, in equivalent
optical power?

John


Re: 4 layer PCB (from 2 layer) + array of designs on one board



PCB stack is an invention to minimise the EMI radiation and improve the
speed of signals talking in terms of microwave or high frequency
propagation.
Jumping from 2 to 4  layers will not gave you many improvements in EMI
as long the major signals are still routed on top and bottom. The first
stack with some performance is a 4 layer stack (counted from top to
bottom)as PWR-signal-signal-GND and 6 layer stack
(top-signal-PWR-GND-signal-GND-bottom or other similar versions) where
top and bottom are mixed signal/ground planes
Will be no noise improvement if +5 and -5V routes becomes planes, could
be worse.
In analogic and RF design the supply lines are usually routed radially
from the source (supply) to destination. This not means a contiguous
supply plane could be worst as long is in the neigborhood af quiet
ground planes.

best regards,
Vasile Surducan
senior application engineer
National Institute R&D for Isotopic and Molecular Technologies
Cluj-Napoca
Romania



Vitaliy wrote:
Quoted text here. Click to load it


Site Timeline