spectre captab?

Spectre has the option to print all the node capacitance values with
an option called captab in the DC analysis options form. I specified
node to node capacitance. The circuit consists of 1 diode connected
npn. In my spectre.out file I see the following:

Q1:int_b : 0 variable=0 0
Q1:int_b : Q1:int_b variable=536.081f 536.081f
Q1:int_b : Q1:int_c variable=201.324f 201.324f
Q1:int_b : Q1:int_e variable=334.757f 334.757f
Q1:int_b : net24 variable=0 -0
Q1:int_c : 0 variable=98.8871f 98.8871f
Q1:int_c : Q1:int_b variable=201.559f 201.559f
Q1:int_c : Q1:int_c variable=300.446f 300.446f
Q1:int_c : Q1:int_e variable=0 -0
Q1:int_c : net24 variable=0 -0
Q1:int_e : 0 variable=0 0
Q1:int_e : Q1:int_b variable=334.522f 334.522f
Q1:int_e : Q1:int_c variable=234.671a 234.671a
Q1:int_e : Q1:int_e variable=334.757f 334.757f

Questions:
1. Why is the b-c and c-b capacitance slightly different?
2. What is the meaning of the b-b, c-c, and e-e capacitance?
3. It is diode connected so why do I have a b-c capacitance?
4. Can I use the b-c and b-e cap values as Cmu and Cpi in the
hybrid-pi SS model?
5. Is there a way that I can output the captab results to a separate
file other than spectre.out for postprocessing?

 

Erik,

Don't have time to check out the other questions, but spectre itself can
output the captab to an arbitrary file. Add an include file (or a model file)
with:

mycaptab info what=captab where=file ...

Andrew.

 

Hi Erik,

Your question 1 is tricky.

I believe the user manual answers questions 2

(formulas are a bit messed up, here, you can better look at the pdf.)
_______________________________________________________________________<rtfm>
Printing the Node Capacitance Table

The Spectre simulator allows you to print node capacitance to an output
file. This can help
you in identifying possible causes of circuit performance problems due
to capacitive loading.

The capacitance between nodes x and y is defined as


July 2002 194
Product Version 5.0


Spectre Circuit Simulator
User Guide
Control Statements




q
x
C = ­
xy --------
vy


where q is the sum of all charges in the terminal connected to node
is the voltage
x
x, and vy
at node y.

The total capacitance at node x is defined as


q
x
C =
xx v
--------x


where charge q and voltage are at the same node
x vx
x.

You may use the captab analysis to display the capacitance between the
nodes in your
circuit. This is an option in the info statement. Here is an example of
the info settings you
would set to perform a captab analysis:


Parameter Setting Action Taken

what=captab Performs captab analysis.
The default value is
oppoint.

where=logfile Prints the parameters to
a logfile. Other possible values
are nowhere, screen, and
file. The value rawfile is
not supported for node
capacitance.

title=captab Prints captab as the
title of the analysis in the output
file.

threshold=0 Specifies the threshold
capacitance value. The nodes for
which the total node
capacitance is below the threshold
value will not be
printed in the output table.

detail=node Displays the total node
capacitances. Other possible
values are nodetoground
and nodetonode.

sort=value Sorts the captab output
according to value. The other
possible value is name.


For a complete list of captab parameters and values, consult the Spectre
online help
(spectre -h).


July 2002 195
Product Version 5.0


Spectre Circuit Simulator User Guide
Control Statements



You may use the infotimes option of the transient analysis when you bind
the captab
analysis to a transient analysis. This runs the captab analysis at
specified time intervals. The
syntax for the infotimes option is

infotimes=[x1, x2...]

where x1 and x2 are time points for which the info analysis should be
performed. The
following is an example of binding a captab analysis to a transient
analysis.

tran1 tran stop=1 µ infotimes=[0.1 µ 0.5 µ ]infoname=capInfo
capInfo info what=captab where=file file='capNodes'
detail=nodetonode



Output Table

The output for the captab analysis is printed in the following format:

n The first column displays the names of the two nodes
(From_node:To_Node).

n The second column displays the fixed (linear) capacitance between
the two nodes.

n The third column is the variable (non-linear) capacitance between
the two nodes.

n The last column displays the total capacitance between the nodes.

Table 7-1 displays the output for the circuit below when detail=nodetonode:



C3=1p


0.5p
n1
n3

C2=2p
n2
1p


1p


C1=2p





July 2002 196
Product Version 5.0


Spectre Circuit Simulator User Guide
Control Statements



In this circuit, the total capacitance at node 2 (n2:n2 in the table) is:
C1+C2+C3=5p

The total capacitance between node 2 and node 1 (n2:n1) is:
C2(Linear)+C3(Non-Linear)=3p

Table 7-1 Node Capacitance Table Sorted by Value



n2:n2 Fixed=2p Variable=3p
Sum=5p

n2:n1 Fixed=2p Variable=1p
Sum=3p



n1:n1 Fixed=3.5p Variable=1p
Sum=4.5p

n1:0 Fixed=1p Variable=0
Sum=1p

n1:n2 Fixed=2p Variable=1p
Sum=3p

n1:n3 Fixed=0.5p Variable=0
Sum=0.5p

n3:n3 Fixed=1.5p Variable=0
Sum=1.5p

n3:0 Fixed=1p Variable=0
Sum=1p

n3:n1 Fixed=0.5p Variable=0
Sum=0.5p



The total node capacitance at nodes 1, 2, and 3 is represented by the
rows n1:n1, n2:n2,
and n3:n3 respectively.

There is no entry for n3:n2, which means there is no capacitance between
these two nodes.

Table 7-1 is sorted by value. The rows are first grouped according to
node names - the rows
with the same From_Node are kept in a group. The row depicting the total
capacitance at
each node is always displayed first in the group, and the row displaying
the node-to-ground
capacitance is second. The remaining rows within each group are sorted
in descending order
of the Sum value.

Note: If the threshold is set to 2p (thresh=2p), the row n1:n3 will not
be printed since the
capacitance between them is less than the threshold. The row n1:0 will
be printed since the
node-to-ground capacitance is always printed. The group n3:n3, n3:0, and
n3:n1 will not
be printed because the total node capacitance at node 3 (n3:n3) is less
than the threshold.

If you sort the table by name (sort=name), it would look as follows:




July 2002 197
Product Version 5.0


Spectre Circuit Simulator User Guide
Control Statements



Table 7-2 Node Capacitance Table Sorted by Name


n1:n1 Fixed=3.5p Variable=1p
Sum=4.5p

n1:0 Fixed=1p Variable=0 Sum=1p

n1:n2 Fixed=2p Variable=1p Sum=3p

n1:n3 Fixed=0.5p Variable=0
Sum=0.5p



n2:n2 Fixed=2p Variable=3p Sum=5p

n2:0 Fixed=0 Variable=2p Sum=2p

n2:n1 Fixed=2p Variable=1p Sum=3p



n3:n3 Fixed=1.5p Variable=0
Sum=1.5p

n3:n0 Fixed=1p Variable=0 Sum=1p

n3:n1 Fixed=0.5p Variable=0
Sum=0.5p



In this case, the From_Node:To_Node column is sorted alpha-numerically.
However, the
row depicting the total capacitance at each node is always displayed
first in the group, and
the row displaying the node-to-ground capacitance is second.
______________________________________________________________________</rtfm>



For question 3: a shorted capacitor is still a capacitor. If you ask for
all the operating point capacitors of a bipolar, you will get them all,
no matter what the network around this bipolar is.

Question 4: It seem Cmu is between intrinsic base and intrinsic
collector, what you print also. That should be OK.

(question 5 : answered by Andrew, and documented by "spectre -h info")


When you get an answer about Q1, please post it.

 

FYI

I opened SR 32715538 to allow me to specify a captab output file in
the captab section of the DC options form.