how to decide the impedence of board

[v_kumar]

help

I am new in high speed design, i am using xcs(xilinx ic) on the board.

1) what must be the impedance of the board are there any standars.
2) how to decide the impedance of the board.
3) what will be the stack up for 4 layer board.(what will be trace width and dielectric thickness)

thanks in advance

 

[circuit]

help

I am new in high speed design, i am using xcs(xilinx ic) on the board.

1) what must be the impedance of the board are there any standars.
2) how to decide the impedance of the board.
3) what will be the stack up for 4 layer board.(what will be trace width and dielectric thickness)

thanks in advance

Check these out for some of your answers

Regarding the stack up for planes in four layer board, a good post by one of the members...


For calculating trace impedance of copper,
**broken link removed**
http://www.ultracad.com/calc.htm

try getting hold of High-Speed Digital Design: A Handbook of Black Magic by Howard Johnson. It covers a lot of things you want to find out.

Regarding traces I would recommend fat traces for the power signals ( you need to check the load current/ allowed temperature rise etc...) but yeah having dedicated power/ ground planes will help a lot. And usually 10/20 mil traces are followed for the signals but it depends on lot of issues. good luck !

 

[jdhar]

50 ohm trace impedance is usually the norm to use - depending on how fast your circuit is, you may or may not even need controlled impedance. If you are designing something for home use, chances are that you don't... a general rule is that if the rise time is 1/6th of the traces electrical length, you will need controlled impedance.

 

[v_kumar]

Hello,
After the stackup is fixed suppose for 4 layers
than i have seen two different configurations which are as followes.

1) Is it possible to fabricate any kind of stackup if i design for any other impedance than the spacing will vary inbetween the layers.
2)what is the differance inbetween FOUR LAYER and SINGLE PLY. why we call them as four layer and single ply is there any differance in fabrication.

configuration 1
FOUR LAYER
S
0.0156"
P
0.023"
G
0.0156"
S

configuration 2
SINGLE PLY
S
0.0083"
P
0.038"
G
0.0083"
S

thanks in advance

 

[House_Cat]

The term 'plies' refers to the number of sheets of prepreg that are stacked to get the desired thickness between layers.

A four layer board is usually made by taking 'core' material, placing one or more 'plies' of 'prepreg' on either side of the core, and then placing copper foil or another core on top of the prepreg.

'Core' is cured board material with foil on one or both sides. 'Prepreg' is uncured board material used to bind the layers together - it is cured by pressing the board at elevated temperature. 'Foil' is just what it sounds like - it is copper of thickness 1/4oz, 1/2oz, 1oz, etc. that is bonded to the board by the prepreg.

There is no difference in fab for the two examples you show, other than the stock thicknesses of core and/or prepreg used to lay up the board. You can specify any distance between copper layers you want - as long as the fab can find the proper thicknesses of core and prepreg to combine to give you what you want. You can't properly design a stackup without discussing the capabilities of the fab with them in advance - they will tell you what materials and thicknesses they can get and use.

 

[v_kumar]

thankyou house cat

but
mr JDHAR has explained that normally the boards are designed for 50 ohm impedance. But i heard from one of my friend that normally it is followed from 50 ohms to 75 ohms.

1) So what factor decides that we must follow 50 ohm or 75 ohm impedance for the boards.

Does it depend on the IC'S we use on the board. so that the IC fabricator recomends that we must follow 50 ohm impedance boards.

 

[House_Cat]

The traces on a circuit board are transmission lines. To transmit the maximum energy with the least distortion (also called maintaining signal integrity), the transmission line impedance should equal the load impedance for critical signals. Critical signals would be those that contain intelligence, or those that affect the signals carrying intelligence. Signals such as data lines, analog signals, clocks, etc, are generally those you would want to keep as undistorted as possible.

Not all traces have to be controlled impedance, only those that contain sensitive signals. The required impedance can be anything, depending on the type of circuit. 50 and 75 ohms are common, but you also find 100 ohms, 120 ohms, 300 ohms, etc. You need to look at the devices, the function of the circuit, and the desired response of the circuit to determine the appropriate impedance.

Control circuits for servos, motors, relay controls, audio circuits, etc, typically don't require controlled impedance traces. High speed digital circuits, RF circuits, measurement circuits, etc, typically do require controlled impedance. The most common impedances in high speed digital circuits are 50 and 100 ohms - but, these are by no means the only impedances that might be required.

 

[eedac]

The line impedance depends on board material, core and copper thickness, and signal freq.

To: House_cat
For v_kumar case, do he need to care equal-length of wires? and how to determine a length tolerance among them?

 

[House_Cat]

For v_kumar case, do he need to care equal-length of wires? and how to determine a length tolerance among them?

It takes time for a signal to move along a circuit board trace. The signal edge can be signficantly delayed on long traces. To determine which traces should be matched or controlled in length, you must use a timing diagram for the type of logic being used on the board. You then determine a "timing budget", or the allowable variation in timing among the various clocks and control signals.

If differential signals are used, you would want to match trace lengths on the two sides of the signal to keep the same signal delay on both sides. On fast edge-rate signals, failure to control skew can cause distortion and/or jitter - depending on the type of signal with which you are dealing.

Note that it is the edge-rate of digital signals you want to watch with respect to delay - not the base frequency. You can have a high frequency signal with a low rise time that will not suffer as greatly as a lower frequency signal that has a fast rise time. The reason for this is that most digital circuits with which you will work use the pulse edge to trigger events. Anything that affects the pulse edge will have consequences in the circuit operation.

 

[tux]

which pcb tool ur using for pcb. if ur using cadence
tools i can give u generic tech file for it

 

[circuit]

@ House_Cat and others,

I understand that signals have a return path on the ground plane underneath the signals to have the shortest path. And so if I am using a 4 layer board with Sig-Gnd-Power(number of islands for different supplies)- Signal and move the signal from layer1 to layer4 for a short distance, do I need to provide capacitors between supply and ground to provide path for return signal? . What happens in the case of a differential signal wherein both signals are moved to layer4 and then back to layer 1?

How is the signal integrity analysed for routing the signals on a board. Say, If I am manually routing the signals, how do I know the crosstalk between any signals/ differential signals. What tools are used here.

how do we use to perform simulation for board level design. We need spice models of all the components to perform this ? If I need to design a board with an temperature sensor/ A/D converter/ power supply, clock etc, how do I simulate this at system level ?

Thanks much,
TD

 

[House_Cat]

Circuit - you really need to get some text books and start studying. The questions you are asking are pretty involved for a quick answer to be completely correct.

That being said, I'll take a shot at some short answers. Please realize that there is much more to the subject than I will attempt to answer here.

The 'islands' on your planes are called splits. You are using split planes. Whenever a high frequency signal path passes over a split in a plane, there is a change in impedance. That change in impedance is a function of the width of the split, the frequecy components of the signal edge (for digital signals), and the availability of an alternate path. Such impedance discontinuities cause signal distortion. The alternate return path, when the plane is discontinuous, can be through bypass capacitors, or around and/or through other components. You should have the power supplies well bypassed at each critical IC, so the most likely route will be through the nearest bypass capacitors. In general, it is best to avoid routing over splits in the first place.

Differential signals do not rely upon the underlying plane for signal return. However, the impedance of each side of the line is determined by the proximity of adjacent planes, as well as the spacing between the two sides of the differential pair. You should try to avoid making a transition from top to bottom with sensitive differential pairs - again, realize that low frequency, low rise time, signals will not be affected to any measurable extent. The concern is with fast edges, or high frequency RF.

There are many software tools available for analyzing crosstalk. A good one that is easy to use (but moderately pricey) is Hyperlynx from Mentor. A simple, much less accurate tool, is free from: http://www.ultracad.com/ct_calc.htm
An expensive, but sophisticated and accurate tool is: **broken link removed**

As you suspect, board level simulation needs something like PSPICE, or SPICE. Each component needs to have a model appropriate for the frequecies in use.

Do a little searching on Google. There is a lot out there to help you get more information on all of the above. An excellent place to start is:
**broken link removed**

 

[jdhar]

Just as a comment, there is no short-cut for signal integrity analysis - there are no generic rules or templates that you can use. Well, that's the case with almost any engineering topic, but SI in specific... pick up a good book and read it. I recommend Howard Johnson's High speed Digital Design; a handbook in Black Magic. All the good points House-cat have made are explained in depth there. Also, the site he posted, www.sigcon.com is Dr. Johnson's web site.

 

[prakash13]

refer book of black magic by Howard Johnson