[SI-LIST] Re: Rs in W-element
- From: jan.vercammen1@xxxxxxxx
- To: TerenceHsieh@xxxxxxxxxxxx
- Date: Thu, 22 Dec 2005 15:48:14 +0100
Terence,
it is possible to plot the series (L and Rs) and shunt (C and Y) PUL
parameters.
For example, to find the series elements use a short-circuited
transmission line
and excite it with a 1Amp AC current source. To extract Rs one should plot
the
real part of the voltage measured at the excited port. To plot the
inductance
L just plot the expression vi(port_voltage)/(2*pi*frequency).
To find the shunt parameters use an open ended transmission line. The real
part reveals Y
and the reactive part the capacitance C.
Below is an example of a Spice file to extract L and Rs. I have used an
.alter to change the rs
value (doubled it). The plot reveals that Rs changes also. So the Spice
W-element is just
doing what it should do.
One word of caution. As the line becomes electrically "long" there will be
standing waves.
So I have used a very short line of length 0.0025 (1/400). So if you want
to plot
the unit lengt parameters multiply by 1/0.0025=400. You can make the
length shorter if you whish.
For this example I used:
400*ac2.vr(1) 400*ac2.vi(1)/(2*pi*frequency)
to plot the unit length resistance and inductance respectively
Kind regards,
Jan Vercammen
************************
w-element test
.param rs=1.166330e-03
.MODEL singleline W MODELTYPE=RLGC, N=1
+ Lo = 3.149855e-07
+ Co = 1.061570e-10
+ Ro = 2.745859e+00
+ Go = 0.000000e+00
+ Rs = rs
+ Gd = 6.225371e-12
iac 0 1 ac 1
w1 1 0 0 0 singleline len=0.0025
.ac dec 25 0.1meg 2e9
.save vr(1) vi(1)
*** double Rs
.alter
.param rs='2*1.166330e-03'
.end
<TerenceHsieh@xxxxxxxxxxxx>
Sent by: si-list-bounce@xxxxxxxxxxxxx
22/12/2005 08:37
Please respond to TerenceHsieh
To: <si-list@xxxxxxxxxxxxx>
cc: (bcc: Jan Vercammen/AMEMV/AGFA)
Subject: [SI-LIST] Rs in W-element
Dear all
I have a question about W-element in Hspice. When I use
W-element presented by RLGC Matrix,
the matrix parameter looks as below
.MODEL singleline W MODELTYPE=RLGC, N=1
+ Lo = 3.149855e-07
+ Co = 1.061570e-10
+ Ro = 2.745859e+00
+ Go = 0.000000e+00
+ Rs = 1.166330e-03
+ Gd = 6.225371e-12
In Hspice manual description, the resistance with skin effect is
R(f)=Ro+(square_root f)(1+j)Rs
For different frequency there should be different resistance
performance.
However, even I simulate with very high frequency (several Ghz), the
loss of the transmission line is the same.
I have set the INCLUDERSIMAG=YES, and also modify Rs to a big value. The
loss never changes.
How could this happen? Is there some setting I missed?
terence
------------------------------------------------------------------
To unsubscribe from si-list:
si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field
or to administer your membership from a web page, go to:
//www.freelists.org/webpage/si-list
For help:
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
List FAQ wiki page is located at:
http://si-list.org/wiki/wiki.pl?Si-List_FAQ
List technical documents are available at:
http://www.si-list.org
List archives are viewable at:
//www.freelists.org/archives/si-list
or at our remote archives:
http://groups.yahoo.com/group/si-list/messages
Old (prior to June 6, 2001) list archives are viewable at:
http://www.qsl.net/wb6tpu
------------------------------------------------------------------
To unsubscribe from si-list:
si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field
or to administer your membership from a web page, go to:
//www.freelists.org/webpage/si-list
For help:
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
List FAQ wiki page is located at:
http://si-list.org/wiki/wiki.pl?Si-List_FAQ
List technical documents are available at:
http://www.si-list.org
List archives are viewable at:
//www.freelists.org/archives/si-list
or at our remote archives:
http://groups.yahoo.com/group/si-list/messages
Old (prior to June 6, 2001) list archives are viewable at:
http://www.qsl.net/wb6tpu
Other related posts:
