Hi,

 Signal delay is dependant of the relative electric permitivity
of the insulating materials sourounding the conductor.
Sometime this material constant is refered to as the 'relative
dielectricity constant' I'ts not really a constant since it
is slightly frequency dependant but for normal use we can regard it as
being a static constant.

The value is about 4.5 for a normal FR-4 laminate but you can check it
in the laminate data sheet.

The value for air is about 1.0

Teflon has about 2 while ceramic may have up to 10.


Now, the signal speed is ideally the same as the speed of light.
-But that's in vacuum only.

On a PCB, the 'light speed' is degraded with the square root of the
relative dielectricity constant.
PCBspeed = speed of light / sqrt( Er )

(Er =  relative dielectricity constant)

-The width or thickness of the conductor has no influence.

Put into some (approximate) formulas you can use, you'll get:

Delaytime = 1,017 * sqrt( 0,475*Er + 0,67 )  nanoseconds per foot
Er= the relative dielectricity constant

This value is fairly accurate for a trace on the outside of a PCB

For an embedded trace you'll get:

Delaytime = 1,017 * sqrt( Er ) nanoseconds per foot


The reason for the difference in the two formulas is that in the
last case, the conductor sees the same Er on top and bottom side of
itself while in the first case the top side is air
(or very thin solder mask) having Er appr =1.0 and the bottom side
being the laminate of Er around 4.5
Unfortunately the resulting Er is not easily calculated so
these formulae are easier to use if not extremely accurate
results are needed -in which case you will need a so called field solver
such as XTK from Quad or similar tools from other vendors.

Hope this helps you. If not, you are welcome to email me for more
assistance.

Best regards

Per Viklund
Dansk Data Elektronik AS



Mark Radley wrote:
>
> I am thinking of using a long signal trace to control some timing.
> Can someone tell me how much delay will be added to a signal due to the length of the signal trace on the board?
>  The Trace width will be .006  - 1/2 oz copper.
> Is this delay dependent on  internal / external layers ?
> Is this delay dependent on impedance control ?
> What kind of tolerance can be exepcted from one board to the next?
>
> Thank You for your help.
>
> Mark Radley
>
> ##############################################################
> IPC Designers Council Mail List provided as a free service by IPC using LISTSERV 1.8c
> ##############################################################
> To subscribe/unsubscribe, send a message to [log in to unmask] with following text in the body:
> To subscribe:   SUBSCRIBE DESIGNERCOUNCIL <your full name>
> To unsubscribe:   SIGNOFF DESIGNERCOUNCIL
> ##############################################################
> Please visit IPC web site (http://www.ipc.org/html/forum.htm) for additional information.
> For the technical support contact Dmitriy Sklyar at [log in to unmask] or 847-509-9700 ext.311
> ##############################################################

##############################################################
IPC Designers Council Mail List provided as a free service by IPC using LISTSERV 1.8c
##############################################################
To subscribe/unsubscribe, send a message to [log in to unmask] with following text in the body:
To subscribe:   SUBSCRIBE DESIGNERCOUNCIL <your full name>
To unsubscribe:   SIGNOFF DESIGNERCOUNCIL
##############################################################
Please visit IPC web site (http://www.ipc.org/html/forum.htm) for additional information.
For the technical support contact Dmitriy Sklyar at [log in to unmask] or 847-509-9700 ext.311
##############################################################