Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

When the PCB design is considered to be high speed

Status
Not open for further replies.

Al Farouk

Full Member level 4
Joined
Jan 13, 2003
Messages
191
Helped
16
Reputation
32
Reaction score
16
Trophy points
1,298
Location
Egypt
Activity points
1,854
Dear all
I'm asking for figers of merit to consider the PCB design to be high speed desin. i.e what are the limit of frequency of the signals carried by the tracks, the length of tracks, ....etc.

Regards
 

mr_ghz

Full Member level 5
Joined
Apr 1, 2002
Messages
289
Helped
7
Reputation
14
Reaction score
5
Trophy points
1,298
Activity points
3,551
Hi Al Farouk

What do you want to design: a digital or an anlog system? In which
frequency range should the system be working?

Bye
 

Al Farouk

Full Member level 4
Joined
Jan 13, 2003
Messages
191
Helped
16
Reputation
32
Reaction score
16
Trophy points
1,298
Location
Egypt
Activity points
1,854
It is digital design and the maximum frequency about 50 Mhz but I have about 6 layers.
 

mr_ghz

Full Member level 5
Joined
Apr 1, 2002
Messages
289
Helped
7
Reputation
14
Reaction score
5
Trophy points
1,298
Activity points
3,551
Hi Al Farouk,

generally you have to take attention to three things:
- The impedance of the trace is to match the impedance of your sender.
The impedance is given by the width of the trace, the thickness of your
PCB and the material (er) of your PCB. You have to take this in account
for analog signals with a frequency over 100MHz and for digital signals
over 100MHz. So this point is not as interresting for your design
- The impedance of the receiver should be the same as the impedance of
your sender, or you will get reflections. In digital designs this can cause
to problems, when the length of a trace is more than 1/10 of the wave-
length of your signal. On FR-4 the wavelength for 50MHz is about
3meters. So if you keep your traces shorter than 30cm, everything is
OK. If this is not possible you have to work with resistors that will
terminate your lines.
- The line-length of a bus system should match more or less. The phase-
difference on two bus-lines should be no more than about 10°. So the
length of these lines should match to about 1/36 of the wavelength,
this will give about 8cm max difference. This should also be a reachable
value.
It is to say that a design for 50MHz can be made without big problems if
you have proper VCC and GND (planes!).
These values I gave above are estimations!

Bye
 

Al Farouk

Full Member level 4
Joined
Jan 13, 2003
Messages
191
Helped
16
Reputation
32
Reaction score
16
Trophy points
1,298
Location
Egypt
Activity points
1,854
Dear mr_ghz
thanks for your valuable information. I want to discuss with you two points
1- Did you get the wave length equal to 3 meter for FR4 and 50Mhz by considering that the signal travel with have the speed of light on PCB board?
2- I read that the rise of the digital signal dominat the PCB design more that the frequency of it in case it had sharp edges. as sharp edges cause high frequency components if it is analysed by fourier. so I think the rule of that 1/10 wavelengh can be mre suitably applied for the rise time of the signal rather that the ignal frequency in case of sharp edges, so the 50Mhz design can be treated as high speed design. what is your main?

Regards
 

mr_ghz

Full Member level 5
Joined
Apr 1, 2002
Messages
289
Helped
7
Reputation
14
Reaction score
5
Trophy points
1,298
Activity points
3,551
Hi Al Farouk,

A signal propagates with the speed of light in a dielectricum with er=1.
When this value is increased, the speed lowers. FR-4 has an er of about
4, so the speed will be about half. The wavelength can be calculated:
lambda=c/(f*sqrt(er)). This will result in the given 3 meters. (These
values are true when you have a proper ground plane).
Fact is that a digital signal has not only the frequency itself (e.g. 50MHz),
it also has all overtones (100MHz, 150MHz, ...). This will give the sharp
edges. This frequencies do not carry (direct) information. This frequencies
are already taken in account in the 1/10 of wavelength.
The bigger problem of these higher frequencies is the radiated power. If
you have to pass an EMC test, this can be critical. Much CPU's can lower
the sharpness of their signals, this can help. Another possibility is to take
a metal housing...

Bye
 

juggernaut7

Member level 1
Joined
May 10, 2001
Messages
39
Helped
3
Reputation
6
Reaction score
3
Trophy points
1,288
Location
USA
Activity points
291
You may be selling yourself short by limiting your discussions to 50MHz. The clock frequency may be low, but it isn't the clock freq that causes a design to be considered high speed, it is the rise time of the device. A fast device (which pretty much all new builds are) will create a signal transition that propagates down the line much faster than 50MHz. You should evaluate your design based on the parts, not the clock frequency.
 

binu G

Advanced Member level 2
Joined
Jan 9, 2003
Messages
501
Helped
12
Reputation
24
Reaction score
3
Trophy points
1,298
Location
Bangalore
Activity points
3,782
help

where i can get more information about the high speed design?
 

wilson

Member level 3
Joined
Jul 24, 2002
Messages
54
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,286
Activity points
478
High Speed Design

Hello Binu
Here is a file which will give you a brief intro about High Speed Board Design.
Other Then this you can visit

https://www.signalintegrity.com/

a nice site to look at...

regards

Wilson
 

tarakesava

Newbie level 6
Joined
Jan 28, 2007
Messages
14
Helped
2
Reputation
4
Reaction score
2
Trophy points
1,283
Activity points
1,356
when ever trace behaves as a transmission line in pcb,by the time we consider as high spped design.

1)whenever trace exceeds criticl length,by the time we consider trace behaves as a transimission line.
2)when rise time of signal is less than twice of the propagation delay of the signal to travel trace ,then we conisider trace exceed the critical length.

pls inform if any thing is wrong.

thx u

Added after 18 minutes:

Signal_Integrity_Issues_And_Printed_Circuit_Board_Design.rar by dougals brooks
 

venkat_kvr

Banned
Joined
Jan 24, 2007
Messages
208
Helped
32
Reputation
64
Reaction score
16
Trophy points
1,298
Activity points
0
if the length of the trace is grater than the rise time length,then u can consider ur board as highspeed
 

hidelove

Newbie level 3
Joined
Feb 13, 2007
Messages
3
Helped
1
Reputation
2
Reaction score
1
Trophy points
1,283
Activity points
1,293
I've questions for it , Does the trace length are really relate for EMI , becuase I seem many trace has equal the 1/4 lumda,but I can't see anything happening ,please explain why ~? Thanks !!
 

AlexTien

Newbie level 3
Joined
Sep 20, 2006
Messages
3
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Activity points
1,293
I think this book is great to read.



Signal Integrity - Simplified (Prentice Hall Modern Semiconductor Design Series' Sub Series: PH Signal Integrity Library) (Hardcover)
by Eric Bogatin (Author)
 

panda14

Newbie level 4
Joined
Jun 14, 2007
Messages
7
Helped
1
Reputation
2
Reaction score
1
Trophy points
1,283
Activity points
1,310
it depends on your rise time also, normally exceed 5% or 10% of lamba we can see the TL effects
 

Thomson

Full Member level 3
Joined
Oct 15, 2004
Messages
181
Helped
4
Reputation
8
Reaction score
1
Trophy points
1,298
Activity points
2,400
AlexTien said:
I think this book is great to read.



Signal Integrity - Simplified (Prentice Hall Modern Semiconductor Design Series' Sub Series: PH Signal Integrity Library) (Hardcover)
by Eric Bogatin (Author)



Five Star book on amazon and tells your much about signal integrity!
 

Fom

Advanced Member level 2
Joined
Mar 10, 2004
Messages
633
Helped
84
Reputation
168
Reaction score
31
Trophy points
1,308
Location
Taiwan
Activity points
4,451
From "Electromagnetics explained" book:

5/5 rule
If any signal has a frequency greater than 5MHz or has edges faster than 5 nsec you should use ground plane.
 

prasad5551

Newbie level 6
Joined
Apr 16, 2008
Messages
12
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Activity points
1,339
hi
all concepts are given in the EMC and the printed circuit board by mark.I.montrose from ieee press,u can download from ebookee.com
 

Timgonghe

Newbie level 1
Joined
Apr 26, 2008
Messages
1
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Activity points
1,284
If 1/3 or more of your digital circuit speed excced 40~50MHz, we generally call it high speed.
 

ar_m_in

Junior Member level 2
Joined
Jun 20, 2006
Messages
23
Helped
0
Reputation
6
Reaction score
0
Trophy points
1,281
Activity points
1,384
Nice info from diff people
thanks
 

Status
Not open for further replies.

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Top