spice3f5 under linux

I

Ian Bell

Guest
I am having a problem with dc analysis with spice 3f5 under linux in batch
mode. I get an error which says dc analysis not done because doAnalyses
not found. .ac et al seem to be OK. Any ideas?

Ian
 
Ian Bell <ian@nowhere.com> wrote:
: I am having a problem with dc analysis with spice 3f5 under linux in batch
: mode. I get an error which says dc analysis not done because doAnalyses
: not found. .ac et al seem to be OK. Any ideas?

Download tclspice-0.2.15 and try again. Tclspice is the best
supported port of SPICE 3f5 to Linux.

http://tclspice.sourceforge.net/

Although tclspice has its issues, it does do .dc, .ac, and .tran
analyses without any problem. It incorporates the command-line SPICE
program ngspice, which is probably what you want to use.

Stuart
 
Stuart Brorson wrote:

Ian Bell <ian@nowhere.com> wrote:
: I am having a problem with dc analysis with spice 3f5 under linux in
: batch
: mode. I get an error which says dc analysis not done because doAnalyses
: not found. .ac et al seem to be OK. Any ideas?

Download tclspice-0.2.15 and try again. Tclspice is the best
supported port of SPICE 3f5 to Linux.

http://tclspice.sourceforge.net/

Although tclspice has its issues, it does do .dc, .ac, and .tran
analyses without any problem. It incorporates the command-line SPICE
program ngspice, which is probably what you want to use.

Stuart
Click to expand...
THanks for that. I have downloaded it and will give it a try.

Ian

--
UKFS
 
Ian Bell <ian@nowhere.com> wrote:
: Stuart Brorson wrote:
:> Download tclspice-0.2.15 and try again. Tclspice is the best
:> supported port of SPICE 3f5 to Linux.
:>
:> http://tclspice.sourceforge.net/
:>
: THanks for that. I have downloaded it and will give it a try.

Let us know how you make out! I am keeping a (long and growing) list
of tclspice bugs; I also occasionally submit patches to the keepers of
the code, so if you have a problem I would like to hear about it.

I won't promise that I'll fix anything, or commit to any bugfix
schedule however . . . . :-S

Stuart
 
Stuart Brorson wrote:

Ian Bell <ian@nowhere.com> wrote:
: Stuart Brorson wrote:
:> Download tclspice-0.2.15 and try again. Tclspice is the best
:> supported port of SPICE 3f5 to Linux.
:
:> http://tclspice.sourceforge.net/
:
: THanks for that. I have downloaded it and will give it a try.

Let us know how you make out! I am keeping a (long and growing) list
of tclspice bugs; I also occasionally submit patches to the keepers of
the code, so if you have a problem I would like to hear about it.

I won't promise that I'll fix anything, or commit to any bugfix
schedule however . . . . :-S

Stuart
Click to expand...
Well, apart from installing BLT, dev libs, flex, lex, readlin, tclreadlin
just to get configure to complete without choking, when I finaly got to
make it stops on an error in terminal.c where it can't find a include file
termcaps.h which I could not find either. So I commented out the include
and to my surprise it all compiles and it runs.

First comments - not the worlds best GUI and the usual linux lack of basic
get you started documentation. I'll let you know how I get on.

Ian

--
UKFS
 
Ian Bell wrote:

Stuart Brorson wrote:

Ian Bell <ian@nowhere.com> wrote:
: Stuart Brorson wrote:
:> Download tclspice-0.2.15 and try again. Tclspice is the best
:> supported port of SPICE 3f5 to Linux.
:
:> http://tclspice.sourceforge.net/
:
: THanks for that. I have downloaded it and will give it a try.

Let us know how you make out! I am keeping a (long and growing) list
of tclspice bugs; I also occasionally submit patches to the keepers of
the code, so if you have a problem I would like to hear about it.

I won't promise that I'll fix anything, or commit to any bugfix
schedule however . . . . :-S

Stuart

Well, apart from installing BLT, dev libs, flex, lex, readlin, tclreadlin
just to get configure to complete without choking, when I finaly got to
make it stops on an error in terminal.c where it can't find a include file
termcaps.h which I could not find either. So I commented out the include
and to my surprise it all compiles and it runs.

First comments - not the worlds best GUI and the usual linux lack of basic
get you started documentation. I'll let you know how I get on.

Ian
Click to expand...
I've just tried my simple test circuit and out popped some errors. here's
the orignal spice. maybe you would like to run it with spicewish and see
if it works for you:

First Circuit for Spice
vs 1 0 24V
R1 1 2 10
R2 2 0 1K
R3 2 3 300
R4 3 0 500
*.OPTIONS nopage list nomod
* Operating Point
..op
* DC Analysis
..dc vs 10 24 1
*.PRINT DC I(R1) I(R2) I(R3)
..end


Ian
--
UKFS
 
In article <btpg0t$qg3$2@news.ukfsn.org>, Ian Bell <ian@nowhere.com>
wrote:
I've just tried my simple test circuit and out popped some errors. here's
the orignal spice. maybe you would like to run it with spicewish and see
if it works for you:

First Circuit for Spice
vs 1 0 24V
R1 1 2 10
R2 2 0 1K
R3 2 3 300
R4 3 0 500
*.OPTIONS nopage list nomod
* Operating Point
.op
* DC Analysis
.dc vs 10 24 1
*.PRINT DC I(R1) I(R2) I(R3)
.end
Click to expand...
I wouldn't expect this to run without errors because with the .PRINT commented
out and no .SAVE statement there is nothing for the dc analysis to do.

If you uncomment the print line it still won't work because I(R1) etc
is not valid spice3f4 syntax. The correct syntax would be

..PRINT DC @r1 @r2 @r3

Charles.
 
Charles,

I've just tried my simple test circuit and out popped some errors. here's
the orignal spice. maybe you would like to run it with spicewish and see
if it works for you:

First Circuit for Spice
vs 1 0 24V
R1 1 2 10
R2 2 0 1K
R3 2 3 300
R4 3 0 500
*.OPTIONS nopage list nomod
* Operating Point
.op
* DC Analysis
.dc vs 10 24 1
*.PRINT DC I(R1) I(R2) I(R3)
.end

I wouldn't expect this to run without errors because with
the .PRINT commented out and no .SAVE statement there is
nothing for the dc analysis to do.

If you uncomment the print line it still won't work because I(R1) etc
is not valid spice3f4 syntax. The correct syntax would be

.PRINT DC @r1 @r2 @r3
Click to expand...

If there's no .save statement, I thought 3f4 was
supposed to act as if you had ".save all" in the
deck. Isn't the way the examples that ship with
it were written?

--Mike
 
In article <btpjf3$ji3@dispatch.concentric.net>,
"Mike Engelhardt" <pmte@concentric.net> wrote:

If there's no .save statement, I thought 3f4 was
supposed to act as if you had ".save all" in the
deck. Isn't the way the examples that ship with
it were written?
Click to expand...
Thanks for pointing this out.

You are right about what *should* happen. The spice 3f4 userguide says

http://newton.ex.ac.uk/teaching/CDHW/Electronics2/userguide/sec4.html#4.4.1

"If no .SAVE line is given, then the default set of vectors are saved
(node voltages and voltage source branch currents)."

However, ISTR that, due to a bug in spice, what I described is what *does*
happen for netlists that have .op in them. I may be wrong about this.
I remember thinking about this problem in connection with MacSpice but
never getting roung to fixing it.

Anyway, let's try the OPs netlist in MacSpice, which is similar (but not
identical) in behaviour to Spice 3f5, I find:

----------
MacSpice 1 -> source ianbell

Circuit: First Circuit for Spice

MacSpice 2 -> run
Error: analysis 'D.C. Transfer curve analysis' is being cancelled.
doAnalyses: No valid data saves. Try the 'status' command.

run simulation(s) aborted
MacSpice 3 -> status
1 [OP] save all
MacSpice 4 ->
----------

MacSpice has various modifications over 3f4. Inter alia its error messages are
more informative and the status command prints the ownership of the saves.
MacSpice skipped the DC analysis because there were no applicable saves.
The status command shows that a 'save all' was created, but it was created to
service the .OP command only. The presence of this save inhibits the
default 'save all' behaviour specified in the userguide. Now uncomment the
..PRINT command...

----------
MacSpice 4 -> delete all
MacSpice 5 -> status
MacSpice 6 -> edit
MacSpice 7 -> source ianbell

Circuit: First Circuit for Spice

MacSpice 8 -> run
Warning: can't parse 'r1#branch' in save statement: ignored
Note: use 'status' and 'delete' to deal with obsolete save statements.
Warning: can't parse 'r2#branch' in save statement: ignored
Note: use 'status' and 'delete' to deal with obsolete save statements.
Warning: can't parse 'r3#branch' in save statement: ignored
Note: use 'status' and 'delete' to deal with obsolete save statements.
Error: analysis 'D.C. Transfer curve analysis' is being cancelled.
doAnalyses: No valid data saves. Try the 'status' command.

run simulation(s) aborted
MacSpice 9 -> status
2 [OP] save all
3 [dc] save r1#branch
4 [dc] save r2#branch
5 [dc] save r3#branch
MacSpice 10 ->

----------

Here, MacSpice tried to create the necessary saves to service the .PRINT DC
command, but because I(R1) is a syntax error the were still no valid saves.
However, change the print line so it says '.PRINT DC @r1 ...' and all
is well.

Anyway, I think that Ian should probably try fixing his print statement and/or
add an explicit '.save all' line to his source.

And, I should probably fix MacSpice so that it does what the userguide
says it should...

Charles.
 
Ian Bell <ian@nowhere.com> wrote:
: Ian Bell wrote:
:> Well, apart from installing BLT, dev libs, flex, lex, readlin, tclreadlin
:> just to get configure to complete without choking, when I finaly got to
:> make it stops on an error in terminal.c where it can't find a include file
:> termcaps.h which I could not find either. So I commented out the include
:> and to my surprise it all compiles and it runs.

You only need BLT and much of the other stuff if you want to use the
TCL API stuff. Ngspice alone (which is part of the dist) doesn't need
all that stuff. However, now that you've built it, you've got it!

:> First comments - not the worlds best GUI and the usual linux lack of basic
:> get you started documentation. I'll let you know how I get on.

Hey -- at least it ran! :)

: I've just tried my simple test circuit and out popped some errors. here's
: the orignal spice. maybe you would like to run it with spicewish and see
: if it works for you:

: First Circuit for Spice
: vs 1 0 24V
: R1 1 2 10
: R2 2 0 1K
: R3 2 3 300
: R4 3 0 500
: *.OPTIONS nopage list nomod
: * Operating Point
: .op
: * DC Analysis
: .dc vs 10 24 1
: *.PRINT DC I(R1) I(R2) I(R3)
: .end

This didn't work for me. The issue is that ngspice will only report
current flowing through independent voltage sources:

http://newton.ex.ac.uk/teaching/CDHW/Electronics2/userguide/sec4.html#4.4.2

Perhaps there are some vendor-specific extensions which permit you to
use the above syntax? And as for Charles' suggestion, it didn't work
for me either.

I modified your circuit to incorporate voltage sources. Here is a
session log:

-------------------- Session log ----------------
******
** tclspice-0.2.15 : Circuit level simulation program
** The U. C. Berkeley CAD Group
** Copyright 1985-1994, Regents of the University of California.
** Please submit bug-reports to: ngspice-devel@lists.sourceforge.net
** Creation Date: Sun Dec 21 22:06:36 EST 2003
******

Circuit: First Circuit for Spice

tclspice 380 -> run
Doing analysis at TEMP = 300.150000 and TNOM = 300.150000

No. of Data Rows : 15

No. of Data Rows : 1
tclspice 381 -> listing
First Circuit for Spice

1 : first circuit for spice
2 : vs 1 0 24v
3 : r1 1 2 10
4 : vdc1 2 2a 0v
5 : r2 2a 2b 1k
6 : vdc2 2b 0 0v
7 : r3 2a 3 300
8 : vdc3 3 3a 0v
9 : r4 3a 0 500
12 : .op
14 : .dc vs 10 24 1
15 : .print dc i(vdc1) i(vdc2) i(vdc3)
17 : .end
tclspice 382 -> print dc i(vdc1) i(vdc2) i(vdc3)
Error: dc: no such vector.
tclspice 383 -> print i(vdc1) i(vdc2) i(vdc3)
i(vdc1) = 5.281174e-02
i(vdc2) = 2.347188e-02
i(vdc3) = 2.933985e-02
tclspice 384 ->
-------------------- End session log -----------------

Note that "print dc i(vdc1) i(vdc2) i(vdc3)" didn't work. This is a
bug, since it is apparently correct syntax. I'll add it to the bug
list.

Stuart
 
Stuart Brorson <sdb@cloud9.net> wrote:
: And as for Charles' suggestion, it didn't work
: for me either.

Well, I am a bonehead sometimes. :) I tried the following:

tclspice 384 -> PRINT DC @r1 @r2 @r3
PRINT: no such command available in tclspice
tclspice 385 -> print DC @r1 @r2 @r3
Error: DC: no such vector.
tclspice 386 -> print @r1 @r2 @r3
@r1 = 5.281174e-02
@r2 = 2.347188e-02
@r3 = 2.933985e-02

So Charles is right! Thanks for the suggestion, Charles!

I don't know why tclspice won't do the print when you enter it in the
file itself. It's another bug for the list. . . .

Stuart
 
Charles DH Williams wrote:

In article <btpjf3$ji3@dispatch.concentric.net>,
"Mike Engelhardt" <pmte@concentric.net> wrote:

If there's no .save statement, I thought 3f4 was
supposed to act as if you had ".save all" in the
deck. Isn't the way the examples that ship with
it were written?

Thanks for pointing this out.

You are right about what *should* happen. The spice 3f4 userguide says


http://newton.ex.ac.uk/teaching/CDHW/Electronics2/userguide/sec4.html#4.4.1

"If no .SAVE line is given, then the default set of vectors are saved
(node voltages and voltage source branch currents)."
Click to expand...
Thanks Charles, Stuart and Mike for all your input. The syntax errors are
undoubtedly due to me using an old pspice text book with Berkeley spice3f5.
My justification for this is that the one? area where I have found the
spice docmentation lacking is in the definition (and examples of ) vectors.
I came across the display command in interactive mode so that gave me some
syntactically correct ones to play with plot. Interestingly these use ()
brackets, yet in the examples from you guys [] are common plus the @ prefix
to reference a component. Anyway what this is all leading to is a request
for a pointer to a comprehensive tutorial on vectors.

I have doenloaded umpteen user guides but they are all more or less the help
built into 3f5. Is there some more comprehensive spice documentation
anywhere.

Add to this that I have tried about six variants of linux spice so far and
they all behave differently (the Suse one only accepts lower case commands)
and you can imagine my frustration. Anyway, thanks once again for showing
me the light.

Ian
 
I am making some real progress now - thanks to all who helped. This is my
latest test pack which works fine.

First Circuit for Spice
vs 1 0 24V
R1 1 2 10
R2 2 0 1K
R3 2 3 300
R4 3 0 500
*.OPTIONS nopage list nomod
* Operating Point
..op
* DC Analysis
..dc vs 10 24 1
..PRINT DC @R1 @R2 @R3
..PLOT DC @R1
..PLOT DC V(2)
..end

Though I am still puzzled by the different types of brackets used in
vectors.

Ian
 
Charles,

If there's no .save statement, I thought 3f4 was
supposed to act as if you had ".save all" in the
deck. Isn't the way the examples that ship with
it were written?

Thanks for pointing this out.

You are right about what *should* happen. The spice 3f4 userguide says


http://newton.ex.ac.uk/teaching/CDHW/Electronics2/userguide/sec4.html#4.4.1

"If no .SAVE line is given, then the default set of vectors are saved
(node voltages and voltage source branch currents)."

However, ISTR that, due to a bug in spice...
Click to expand...
Looks like your suggestion fixed the problem, but I've never
seen Berkeley SPICE work that way. The last tape I got from
Berkeley didn't do that. The port I did for Linux didn't do
that. Maybe the error was introduced by whoever compiled
the OP's SPICE.

--Mike
 
In article <1000s823roppmf7@corp.supernews.com>,
Stuart Brorson <sdb@cloud9.net> wrote:

Note that "print dc i(vdc1) i(vdc2) i(vdc3)" didn't work. This is a
bug, since it is apparently correct syntax. I'll add it to the bug
list.
Click to expand...
Not a bug. The 'dc' parameter only applies to the dotcard version of the
command, not the interactive interpreter version where it has been
superceded by 'setplot dc'.

Charles
 
In article <btq54e$r3d$1@news.ukfsn.org>, Ian Bell <ian@nowhere.com>
wrote:

Thanks Charles, Stuart and Mike for all your input. The syntax errors are
undoubtedly due to me using an old pspice text book with Berkeley spice3f5.
Click to expand...
Yes, that would be confusing. Try

Introductory tutorial and exercises:

http://newton.ex.ac.uk/teaching/CDHW/Electronics2/Spice3Quickstart.html
http://newton.ex.ac.uk/teaching/CDHW/Electronics2/SimSheet-01.html

and online Spice 3 manual with corrections, addditions, cross-refs, notes
and search:

http://newton.ex.ac.uk/teaching/CDHW/Electronics2/userguide/

My justification for this is that the one? area where I have found the
spice docmentation lacking is in the definition (and examples of ) vectors.
I came across the display command in interactive mode so that gave me some
syntactically correct ones to play with plot. Interestingly these use ()
brackets, yet in the examples from you guys [] are common plus the @ prefix
to reference a component. Anyway what this is all leading to is a request
for a pointer to a comprehensive tutorial on vectors.
Click to expand...
http://newton.ex.ac.uk/teaching/CDHW/Electronics2/userguide/sec5.html#5.1
http://newton.ex.ac.uk/teaching/CDHW/Electronics2/userguide/secB.html#B

I have doenloaded umpteen user guides but they are all more or less the help
built into 3f5. Is there some more comprehensive spice documentation
anywhere.
Click to expand...
You can either buy a textbook (try amazon) and/or inspect the source code.
If you have specific questions post them here.

Charles.
 
In article <btpva7$jib@dispatch.concentric.net>,
"Mike Engelhardt" <pmte@concentric.net> wrote:

Looks like your suggestion fixed the problem, but I've never
seen Berkeley SPICE work that way. The last tape I got from
Berkeley didn't do that. The port I did for Linux didn't do
that. Maybe the error was introduced by whoever compiled
the OP's SPICE.
Click to expand...
I think the issue only arises with specific combinations
of compile time and runtime options.

Charles.
 
Charles DH Williams wrote:

In article <btq54e$r3d$1@news.ukfsn.org>, Ian Bell <ian@nowhere.com
wrote:

Thanks Charles, Stuart and Mike for all your input. The syntax errors
are undoubtedly due to me using an old pspice text book with Berkeley
spice3f5.

Yes, that would be confusing. Try

Introductory tutorial and exercises:

http://newton.ex.ac.uk/teaching/CDHW/Electronics2/Spice3Quickstart.html
http://newton.ex.ac.uk/teaching/CDHW/Electronics2/SimSheet-01.html

and online Spice 3 manual with corrections, addditions, cross-refs, notes
and search:

http://newton.ex.ac.uk/teaching/CDHW/Electronics2/userguide/
Click to expand...
I had already found and downloaded the quickstart and userguide but did not
realise until last night they were by you. The SimSheet is a useful
addition.

My justification for this is that the one? area where I have found the
spice docmentation lacking is in the definition (and examples of )
vectors. I came across the display command in interactive mode so that
gave me some
syntactically correct ones to play with plot. Interestingly these use ()
brackets, yet in the examples from you guys [] are common plus the @
prefix
to reference a component. Anyway what this is all leading to is a
request for a pointer to a comprehensive tutorial on vectors.

http://newton.ex.ac.uk/teaching/CDHW/Electronics2/userguide/sec5.html#5.1
http://newton.ex.ac.uk/teaching/CDHW/Electronics2/userguide/secB.html#B
Click to expand...
Again this is very similar to the standard user guide but it does have some
aditions so I'll download and read - thanks.

I have doenloaded umpteen user guides but they are all more or less the
help
built into 3f5. Is there some more comprehensive spice documentation
anywhere.

You can either buy a textbook (try amazon) and/or inspect the source code.
Click to expand...
I have a couple of (pspice) books which I suspect will be more of a
hindrance than help. Don't know why I didn't think of Amazon myself.

If you have specific questions post them here.
Click to expand...
Will do and once again many thanks for the help.

ian


--
UKFS
 
You must log in or register to reply here.

Welcome to EDABoard.com

Sponsor

Back
Top