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

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

Reply to
Vitaliy
Loading thread data ...

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.
 Click to see the full signature
Reply to
Jamie

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:

Reply to
Vitaliy

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.)

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.

--
Peter Bennett, VE7CEI  
peterbb4 (at) interchange.ubc.ca  
 Click to see the full signature
Reply to
Peter Bennett

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.

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.

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

Dave :)

Reply to
David L. Jones

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.

--

John Devereux
Reply to
John Devereux

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

Reply to
John Larkin

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)?

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

Reply to
Vitaliy

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.

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  
 Click to see the full signature
Reply to
Peter Bennett

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).

Any recommendati>

What I meant was: I must > More layers won't necessarily improve speed or reduce noise. If you

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

Reply to
Vitaliy

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:

Reply to
vasile

ElectronDepot website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.