suggestions on my pcb design/layout

[circuit]

0402 pcb design rules

I need to design a rigid pcb that will have a silcon die wirebonded to it and then take the signals out of this board using a flex cable to a 4in x 4in 4-layer rigid FR4 board (I have already designed this big board and laid out except for the signals coming in from the flex cable). at the bigger board end I intend to have a ZIF connector for the flex cable. There are 20 signals that the flex cable need to carry. My question is,


there are differential signals coming out from the smaller pcb, they must be routed together right.. i know they must be placed close to each other and maintain some distance from other signals. but the problem is i am using 3 mil traces and they are separated by 3-4 mils ( because of the restriction on the size of the board). so i can have other signals only at 3 -4 mils from the differential signals....how do i take care of this (crosstalk issues ) ?

what about the impedance mismatch, since i will be routing the signals at 10 mils on the bigger board...

i am having power and ground signals brought in through the flex cable. i can and should provide a solid ground plane. but the traces that carry the power to the pads i cant make them more than 5 mils. how do i overcome this coz there will be a voltage drop.

i am thinking of using a flex cable to take out the signals. does this usually need to have all the signals on one layer ( I know there is rigid-flex board but i heard its very expensive ) please provide any suggestions..thanks !

ps: in these kinda design where do we usually place the bypass capacitors ( I am trying to have it in the bottom layer of the board)

 

[Uky]

flex cable simulation

I have had a similar design challenge. I went about it in the following manner:

You can cope with the trace widths if the width/distance ratio is kept both in the flex and the rigid board. If the signal are very high frequency, you will need to make sure that the connector can handle them. Generally speaking; If you have 1ns rise time and 2 inches of trace length - then you have a problem!

I know that Mentor Expedition can make differential timing controlled routing, and I think that Cadence Allegro can do it too.

(BTW: I have designed 800MBit/s LVDS repeaters using a cad system with no differential routing capabilities at all, so If you are careful it can be done)

I did NOT use a ZIF connector. The design was for a hand held unit. ZIF connectors have a tendency to slide out as the unit gets worn. Instead I designed the flex cable with a stiffener at the end and used a HiRose miniature type board2board connector.

The flex cable was designed as a multi layer cable, using two sides as VCC and GND respectively. I got a good ground plane for the high frequency signals, and a wide conductor for the supply voltage. Do a calculation and you will be surprized about the voltage drop.

Have a meeting with the flex cable manufacturer and ask him to supply you with their design rules and constraints. There are a number of different manufacturing technologies, each with pro's and con's.

Some flex manufacturers are happy to do the design work for you just to get it right the first time!

Since the design of flex cables is much a mechanical design work involving many rounded arcs and tapers, some folks prefer using a mechanical drafting package (such as AutoCAD) together with a DXF2Gerber translator (e.g. Artwork Conversion Software, Inc.) (I do not work for them, but I am using this software myself).

Bypass capacitors should be placed close to the components that are to use them as high frequency charge supplys in such a way that the loop fomed by the circuit and the capacitor becames as small as possible.

Double sided assemblies cost $$$. Bear that in mind.

 

[circuit]

flex cable impedance calculator

thanks for your reply !

>You can cope with the trace widths if the width/distance ratio is kept both in the flex and the rigid board. If the signal are very high frequency, you will need to make sure that the connector can handle them. Generally speaking; If you have 1ns rise time and 2 inches of trace length - then you have a problem

on the mini pcb where the die is wirebonded, i have the pads at 3 mils spacing and traces are 3 mil spaced. i will fan them out to 25 mil spacing coz of the flex cable pitch. but on the other end rigid board, I cannot maintain the 25mil spacing, i will have to neck them down to 10 mil. my question is if i use a Flexible printed circuit, is the wirebonding of the die a problem and what is with the stiffness ? and in this case i can design it a double layer FPC with a solid ground plane. the signals are differential and are going to run max at 15-20Mhz.


designing a flex cable is an option but i am not aware of any mechanical design. i got to find out how feasible it is to have a flexible printed circuit)

 

[Uky]

pcb probe lvds differential

The flex manufacturer can make a "seamless" transition from a multi layer flex cable harness to a multi layer circuit board made from fibre glass (FR-4) type material.

To go from there to wire bond at the edge, I do not know, but I have seen rather complex boards that "seamless" transforms into a flex cable harness so it can be done.

I have not made designs using wire bonded technology but - I have seen JTAG interfaces fail to perform at 6 MHz because of bad signal integrity. (Signal reflection caused the clock to make one extra false trigger for each clock cycle). If you have no access to a signal integrity tool, the only way to cope with possible problems is to first make the best possible of the situation. There are free tools out there (e.g. TXLine from AWR) which I just now do not know if it can do impedance calculations for differential signalling).

I have used a free paper slide rule calculator from National Semiconductor "Transmission Line Rapidesigner" Part# 633200-001. NS referrs to an Appnote AN905 which I can not find right now.

I was in the lucky situation that I dealt with one way communication. Thus, I placed small 0402 sized series resistors as close to the transmitters as possible and a series combination of R-C at the receiver side from the lines to GND at the receiver. Also a resistor across the two lines were used.

They had to be "TBD" since I could only do paper based optimization.

Using a FET probe (NOT a common 1MOhm/10pF probe) and a *SHORT* ground strap I was able to verify and adjust until the reflections was minimized.

Yes - there is a flaw in this verification in that I should have used a differential probe, but unfortunately I had not access to such a probe.

I have used PCB tools from both Cadence and Mentor. Both will allow you to design flex cables. One aspect where Cadence (Allegro) and Mentor (BoardStation) excels is the fact that individual footprint pins can be moved when in the layout editor. This may seem awkward at first but it will enable the designer to create the wire bond part footprint with movable pins so that the layout can be optimized.

 

[circuit]

differential impedance calculations national semi

thanks much for your suggestions. we had a discussion with the wire bonding guy and the pcb guy and decided that we are going to go for a double sided flex printed circuit and have a (die)chip-on-a-flex. but it was very good information for me !

after the wire bonding to the pads on the flex, i am just fanning it out to a wider area. but as you said i will have to find out one of the signal integrity tools. i understand that this is very critical. i am having bottom layer of flex circuit as ground plane and probably wide strips for power planes.

yeah i also could not get hold of the "Transmission Line Rapidesigner" but found somewhere that if we call and request them they send it to you.

thanks once again,