ngspice-devel Mailing List for ngspice

Seth,

looks great!

To be honest, I have had to learn a bit about noise simulation, not my
specialty so far.

I have pushed your patch to git branch pre-master-47, will be available
in ngspice-47 (due in summer...).

Holger



A simple test example here:

* noise analysis with analogue code model

aota inn 0 out newota
*.model newota ota (gm=1 rout=1e12 rin=1Meg en=31n enk=100 in_noise=100u ink=10k incm=0 incmk=2k noise_programmatic=TRUE)
*.model newota ota (gm=1m rout=1e12 rin=1Meg en=31n enk=100 noise_programmatic=TRUE)
*.model newota ota (gm=1m rout=1e12 rin=1Meg in_noise=2p ink=500 incm=0 incmk=500 noise_programmatic=TRUE)
.model newota ota (gm=1m rout=1e12 rin=1Meg en=31n enk=100 in_noise=20p ink=2k incm=0 incmk=2k noise_programmatic=TRUE)

Vin in 0 dc 0 ac 1 sin (0 2 1.5k)
Rsource in inn 10k


Rout out 0 1

.control
*tran 1u 10m
*plot out
noise v(out) Vin dec 10 1 10MEG
print inoise_total onoise_total
display
setplot noise1
display
plot  loglog inoise_spectrum
plot  loglog onoise_spectrum
.endc

.end

Hi Holger-

Not to pester you.  But do let me know if you see any issues or would like
modifications

Seth


Seth Hillbrand
*Lead Developer*
+1-530-302-5483‬
Long Beach, CA
www.kipro-pcb.com    in...@ki...


On Sun, Mar 22, 2026 at 3:42 PM Holger Vogt <hol...@un...> wrote:

> Seth,
>
> thanks for the patch.
>
> I have created a git branch hv_noise_2, based on current master, with
> the patch added.
>
> Will have a look at its details later.
>
> Holger
>
>
>
> _______________________________________________
> Ngspice-devel mailing list
> Ngs...@li...
> https://lists.sourceforge.net/lists/listinfo/ngspice-devel
>

Chris,

thanks for the patch.

Uploaded to git branch pre-master-47

If you find more issues, please let us know, or provide another patch :)

Holger

Hello,

I’ve benefitted from open source projects for years, but have never contributed to anything myself. Pardon me if I’m committing any sort of faux pas.

This patch adds a check for a NULL pointer returned by getpwuid() in sharedspice.c and tclspice.c, as well as what looks to be a missing call to tfree() in tclspice.c.

I personally stumbled on the nullptr dereference in sharespice.c, and the tclspice.c looks to be the only other file where this check doesn’t occur.

—
Chris Carreras

Dear ngspice development team,

I recently contributed a small improvement to ngspice 46 (see link below), and I was wondering whether it would be sufficient to have my name added to the AUTHORS file. If not, I completely understand.

https://sourceforge.net/p/ngspice/ngspice/merge-requests/46/

Quote from the AUTHORS file:

If someone helped in the development and has not been inserted in this list
then this omission was unintentional. If you feel you should be on this list
then please write to <ngspice-devel@@lists.sourceforge.net>. Do not be shy, we
would like to make a list as complete as possible.

Best regards,
Enrique Corpa

Seth,

thanks for the patch.

I have created a git branch hv_noise_2, based on current master, with 
the patch added.

Will have a look at its details later.

Holger

Hello Seth,

adding noise support for XSPICE would be a nice feature. This will allow 
not only implement OTA model, but also implement noise for recently 
added XSPICE microstrip lines models: 
https://sourceforge.net/p/ngspice/ngspice/merge-requests/33/ Looking 
forward for feedback from Ngspice maintainers.

Regards,
Vadim

On 3/22/26 18:06, Seth Hillbrand via Ngspice-devel wrote:
> Hi Holger, et al
>
> There was a line in noisean.c that said "/* MIF_NOI is not yet 
> supported by code models, so use their AC capabilities */"
>
> Based on offline discussion, this is required to fully implement the 
> LTSPICE OTA model, which some manufacturers use in their provided models.
>
> The attached patch implements this.  It provides standard noise 
> parameters for simple declarative models and a programmatic interface 
> for code models to define their noise sources.
>
> Let me know if this is acceptable or if you'd like changes.
>
> Seth
>
>
> Seth Hillbrand
> *Lead Developer*
> +1-530-302-5483‬
> Long Beach, CA
> www.kipro-pcb.com <https://www.kipro-pcb.com/> in...@ki...
>
>
>
> _______________________________________________
> Ngspice-devel mailing list
> Ngs...@li...
> https://lists.sourceforge.net/lists/listinfo/ngspice-devel

Hi Holger, et al

There was a line in noisean.c that said "/* MIF_NOI is not yet supported by
code models, so use their AC capabilities */"

Based on offline discussion, this is required to fully implement the
LTSPICE OTA model, which some manufacturers use in their provided models.

The attached patch implements this.  It provides standard noise parameters
for simple declarative models and a programmatic interface for code models
to define their noise sources.

Let me know if this is acceptable or if you'd like changes.

Seth


Seth Hillbrand
*Lead Developer*
+1-530-302-5483‬
Long Beach, CA
www.kipro-pcb.com    in...@ki...

Without knowing which compact model is being called by the hspice model
card, which may provide idsmult as an instance parameters by another name,
I suggest using a subcircuit approach. "Wrap" the transistor in a
subcircuit with an internal drain node. Place a 0V voltage source between
the internal drain node and the external subcircuit drain port. Then place
CCCS between source and the external drain port. Set the gain of the CCCS
to multiply the current of the 0V voltage source to idsmult-1. The final
step is to pass all the same transistor parameters from the subcircuit to
the transistor. Add the extra idsmult parameter to the subcircuit to pass
it into the CCVS.

Regards,
Jim Holmes
*ho...@sh... <ho...@sh...>*






On Tue, Sep 30, 2025, 11:37 AM Brian Degnan <deg...@gm...> wrote:

> M. Vogt,
>
> I look into that too.  HSPICE is basically what I use for everything
> commercial because it's "fab approved", but ngspice has a lot of advantages
> because of my academic overlap, so I have an odd incentive to make
> everything compatible.
> To that end, I still owe you guys some integration examples into verilog.
> I'm trying to make sure that all of the division lines between my projects
> are very bright, and my last foray into making something openly available
> was a bit hazy.
>
> Sincerely,
> Brian Degnan, Ph.D.
>
>
>
> On Tue, Sep 30, 2025 at 6:27 AM Holger Vogt <hol...@un...>
> wrote:
>
>> If you are using BSIM-4.8.3, the current version, you will find instance
>> parameters
>>
>> mult_i "Variability in current"
>> mult_q "Variability in charge"
>> mult_fn "Variability in flicker noise"
>>
>> That may do what you want.
>>
>>
>> _______________________________________________
>> Ngspice-devel mailing list
>> Ngs...@li...
>> https://lists.sourceforge.net/lists/listinfo/ngspice-devel
>>
> _______________________________________________
> Ngspice-devel mailing list
> Ngs...@li...
> https://lists.sourceforge.net/lists/listinfo/ngspice-devel
>

M. Vogt,

I look into that too.  HSPICE is basically what I use for everything
commercial because it's "fab approved", but ngspice has a lot of advantages
because of my academic overlap, so I have an odd incentive to make
everything compatible.
To that end, I still owe you guys some integration examples into verilog.
I'm trying to make sure that all of the division lines between my projects
are very bright, and my last foray into making something openly available
was a bit hazy.

Sincerely,
Brian Degnan, Ph.D.



On Tue, Sep 30, 2025 at 6:27 AM Holger Vogt <hol...@un...> wrote:

> If you are using BSIM-4.8.3, the current version, you will find instance
> parameters
>
> mult_i "Variability in current"
> mult_q "Variability in charge"
> mult_fn "Variability in flicker noise"
>
> That may do what you want.
>
>
> _______________________________________________
> Ngspice-devel mailing list
> Ngs...@li...
> https://lists.sourceforge.net/lists/listinfo/ngspice-devel
>

If you are using BSIM-4.8.3, the current version, you will find instance 
parameters

mult_i "Variability in current"
mult_q "Variability in charge"
mult_fn "Variability in flicker noise"

That may do what you want.

Brain,

Thanks for the additional context. Otherwise I would be suspicious why 
somebody wouldn't "just" use the multiplier :)

I suspect you'll just have to hand hack the model.

The device models are located in: src/spicelib/devices

There are a few BSIM4 directories corresponding to different model 
versions, make sure you're editing the right one.

Add your parameter to b4.c, then edit all of the *ld.c files. (If you're 
not familiar with SPICE, these are the modules that "load" the device 
currents into the circuit matrix, and there are dc/ac/pz analysis 
versions that all need to be consistent).

You'll have to wait for the project maintainer to weigh in to see if a 
model change would be accepted upstream... but of course you can always 
use your own modifications (at your own risk!)

Finally, it sounds like your underlying model is BSIM 4, but if it's 
actually something like PSP you can use ngpsice/OSDI and OpenVAF to run 
VerilogA models.

Regards,
Kevin

Kevin,

I'm sorry, I misspoke. The drain current multiplier that I wanted to add
is MULID0 (idmult is what we call it colloquially).
MULID0 lets me do a sensitivity analysis on bias and gain while holding
Cd/Cs/Cg steady.   It also lets me tweak simulations vs. measured silicon.
I use BSIM models supplied by a "commercially available 2nm" process (as
well as the PSP models depending).
In HSPICE, MULID0 exists for BSIM4, but I suspect it's because it's
supported in PSP103.0, Level=69.

The general syntax for my BSIM4 model is:
Mxxx nd ng ns [nb] mname [L=val] [W=val] [M=val]
+ [AD=val] [AS=val] [PD=val] [PS=val]
+ [RGATEMOD=val] [RBODYMOD=val] [TRNQSMOD=val]
+ [ACNQSMOD=val] [GEOMOD=val] [RGEOMOD=val]
+ [NRS=val] [NRD=val] [RBPB=val] [RBPD=val]
+ [RBPS=val] [RBDB=val] [RBSB=val] [NF=val]
+ [MIN=val] [RDC=val] [RSC=val] [DELVTO=val]
+ [MULU0=val] [DELK1=val] [DELNFCT=val]
+ [DELTOX=val] [OFF] [IC=Vds, Vgs, Vbs]
+ [WNFLAG=val] [MULID0=val]

The fact that MULID0 is the last thing, makes me think that it was
definitely added later.
I can say for sure that it wasn't in HSPICE when I was in grad school, but
it was there in 2015 when I was doing SOI work.

Anyway, I would be excited to get this into the BSIM4 model on ngspice.   I
just have no idea what the level of effort is.  Honestly, I could probably
take a stab at it.

Sincerely,
Brian Degnan, Ph.D.



On Mon, Sep 29, 2025 at 3:58 PM Kevin Zheng <kev...@gm...> wrote:

> Hi Brian,
>
> I'm not sure I've heard of an idmult parameter in HSPICE. Is this a
> standard HSPICE parameter, or a parameter to the particular transistor
> model that you are using?
>
> (Which transistor model are you using? BSIM? EKV?)
>
> I also don't understand what you mean when you say you "don't want to
> change the bias point." It seems to me that setting M would do the same
> as multiplying the drain current.
>
> Regards,
> Kevin
>

Hi Brian,

I'm not sure I've heard of an idmult parameter in HSPICE. Is this a
standard HSPICE parameter, or a parameter to the particular transistor
model that you are using?

(Which transistor model are you using? BSIM? EKV?)

I also don't understand what you mean when you say you "don't want to
change the bias point." It seems to me that setting M would do the same
as multiplying the drain current.

Regards,
Kevin

Hello,

I've been using ngspice concurrently with HSPICE for some of my models.
In HSPICE, I have idmult, which just multiplies the drain current.   I
cannot use "m" as I don't want to change the bias point.  My motivation is
so that my HSPICE/ngspice card decks are the same.

Does anyone have any thoughts on this?  I have no idea the level of effort
for this.

Sincerely,
Brian Degnan, Ph.D.

Marco,

ngspice-44.2 is available.

This is a bug-fix release, fixing some build issues and some recently 
removed source code bugs.

Regards

Holger

On 10/01/2025 19:48, Holger Vogt wrote:
> Marco,
> 
> you may need to build the standard ngspice.exe with
> 
> --with-readline=no
> --with-editline=yes
> 
> I have always tested building on Cygwin with readline. I will check 
> editline as well.
> 
> Holger
> 

build on the bot went fine
https://cygwin.com/cgi-bin2/jobs.cgi?id=9221

and that package is deployed in the distribution

Regards
Marco

On 10/01/2025 16:31, Holger Vogt wrote:
> Concerning the configure options:
> 
> Since ngspice-43 several options are included automatically:
> --enable-xspice, --enable-openmp, --enable-osdi, --enable-klu, --with- 
> readline=yes
> 
> option may be deselected for example by --disable-openmp, with-readline=no
> 
> When the shared ngspice libarary is to be made using --with-ngshared,
> neither readline nor editline options are required, as there is no 
> command input by users.


Cheking the configure --help , I noticed that is NOT obvious that
openmp is enabled by default as two lines are present

   --enable-openmp         Use OpenMP parallel processing
   --disable-openmp        do not use OpenMP

while for the others is more clear

  --disable-xspice        Disable XSPICE enhancements
  --disable-osdi          Disable OSDI integration
  --disable-klu           Use KLU linear systems solver. Default=yes.
                                                         ^^^^^^^^^^^^
partially misleading  default 😉

Regards
Marco

Marco,

you may need to build the standard ngspice.exe with

--with-readline=no
--with-editline=yes

I have always tested building on Cygwin with readline. I will check 
editline as well.

Holger



Am 10.01.2025 um 19:06 schrieb Marco Atzeri:
> On 10/01/2025 16:31, Holger Vogt wrote:
>> Concerning the configure options:
>>
>> Since ngspice-43 several options are included automatically:
>> --enable-xspice, --enable-openmp, --enable-osdi, --enable-klu, --with- 
>> readline=yes
>>
>> option may be deselected for example by --disable-openmp, with- 
>> readline=no
>>
>> When the shared ngspice libarary is to be made using --with-ngshared,
>> neither readline nor editline options are required, as there is no 
>> command input by users.
>>
> 
> Hi Holger,
>   I saw a configure failure for the shared library on the builder bot
> as the readline was not present.
> You may need to check it.
> 
> By long time the cygwin build is using the editline, I never looked to 
> change it until now.
> 
> I patched manually the code along the proposed patch and the shared 
> build worked. The standard one is still running but I expect same result
> 
> Regrds
> Marco
> 

On 10/01/2025 16:31, Holger Vogt wrote:
> Concerning the configure options:
> 
> Since ngspice-43 several options are included automatically:
> --enable-xspice, --enable-openmp, --enable-osdi, --enable-klu, --with- 
> readline=yes
> 
> option may be deselected for example by --disable-openmp, with-readline=no
> 
> When the shared ngspice libarary is to be made using --with-ngshared,
> neither readline nor editline options are required, as there is no 
> command input by users.
> 

Hi Holger,
  I saw a configure failure for the shared library on the builder bot
as the readline was not present.
You may need to check it.

By long time the cygwin build is using the editline, I never looked to 
change it until now.

I patched manually the code along the proposed patch and the shared 
build worked. The standard one is still running but I expect same result

Regrds
Marco

Concerning the configure options:

Since ngspice-43 several options are included automatically:
--enable-xspice, --enable-openmp, --enable-osdi, --enable-klu, 
--with-readline=yes

option may be deselected for example by --disable-openmp, with-readline=no

When the shared ngspice libarary is to be made using --with-ngshared,
neither readline nor editline options are required, as there is no 
command input by users.

The patch is available in the ngspice git master branch.

Do you have a chance to check if it is o.k?

I would then prepare a bug fix release tagged ngspice44.2.

Thanks for the report.

There is already a patch for this bug under way.

diff --git a/src/xspice/verilog/Makefile.am b/src/xspice/verilog/Makefile.am
index cd7674934..262d63384 100644
--- a/src/xspice/verilog/Makefile.am
+++ b/src/xspice/verilog/Makefile.am
@@ -19,11 +19,11 @@ initdata2_DATA = ../../include/ngspice/cosim.h \

  pkglib_LTLIBRARIES = ivlng.la ivlngvpi.la
  ivlng_la_SOURCES = icarus_shim.c icarus_shim.h coroutine_shim.h
-ivlng_la_CFLAGS = -I../../../../src/include
+ivlng_la_CFLAGS = -I$(top_srcdir)/src/include
  ivlng_la_LDFLAGS = -module -shared -avoid-version

  ivlngvpi_la_SOURCES = vpi.c icarus_shim.h vpi_user_dummy.h coroutine.h 
coroutine_cosim.h
-ivlngvpi_la_CFLAGS = -I../../../../src/include
+ivlngvpi_la_CFLAGS = -I$(top_srcdir)/src/include
  ivlngvpi_la_LDFLAGS = -module -shared  -avoid-version

Building on separate tree from source the build stop at:


make[3]: Entering directory 
'/pub/devel/ngspice/ngspice-44-1.x86_64/build/ngshared/src/xspice/verilog'
   CC       ivlng_la-icarus_shim.lo
/pub/devel/ngspice/ngspice-44-1.x86_64/src/ngspice-44/src/xspice/verilog/icarus_shim.c:21:10: 
fatal error: ngspice/cmtypes.h: No such file or directory
    21 | #include "ngspice/cmtypes.h" // For Digital_t
       |          ^~~~~~~~~~~~~~~~~~~
compilation terminated.


configured with

                 --prefix=/usr \
                 --enable-xspice \
                 --enable-cider \
                 --enable-openmp \
                 --enable-osdi \
                 --enable-klu \
                 --with-editline=yes \
                 --with-ngshared


for what I see the file is in an expected location in the source tree

$ find ngspice-44-1.x86_64 -name cmtypes.h
ngspice-44-1.x86_64/origsrc/ngspice-44/src/include/ngspice/cmtypes.h
ngspice-44-1.x86_64/src/ngspice-44/src/include/ngspice/cmtypes.h


but the the Makefile.am of that verilog directory
is not written with proper declaration for separate tree:

marco@LAPTOP-MK4Q85AK 
/pub/devel/ngspice/ngspice-44-1.x86_64/build/ngshared/src/xspice/verilog
x86_64 $ make V=1
/bin/sh ../../../libtool  --tag=CC   --mode=compile gcc -DHAVE_CONFIG_H 
  -I. 
-I/pub/devel/ngspice/ngspice-44-1.x86_64/src/ngspice-44/src/xspice/verilog 
-I../../../src/include  -I../../../../src/include -ggdb -O2 -pipe -Wall 
-Werror=format-security -Wp,-D_FORTIFY_SOURCE=3 -fstack-protector-strong 
--param=ssp-buffer-size=4 
-ffile-prefix-map=/pub/devel/ngspice/ngspice-44-1.x86_64/build=/usr/src/debug/ngspice-44-1 
-ffile-prefix-map=/pub/devel/ngspice/ngspice-44-1.x86_64/src/ngspice-44=/usr/src/debug/ngspice-44-1 
-std=gnu11 -fopenmp -MT ivlng_la-icarus_shim.lo -MD -MP -MF 
.deps/ivlng_la-icarus_shim.Tpo -c -o ivlng_la-icarus_shim.lo `test -f 
'icarus_shim.c' || echo 
'/pub/devel/ngspice/ngspice-44-1.x86_64/src/ngspice-44/src/xspice/verilog/'`icarus_shim.c
libtool: compile:  gcc -DHAVE_CONFIG_H -I. 
-I/pub/devel/ngspice/ngspice-44-1.x86_64/src/ngspice-44/src/xspice/verilog 
-I../../../src/include -I../../../../src/include -ggdb -O2 -pipe -Wall 
-Werror=format-security -Wp,-D_FORTIFY_SOURCE=3 -fstack-protector-strong 
--param=ssp-buffer-size=4 
-ffile-prefix-map=/pub/devel/ngspice/ngspice-44-1.x86_64/build=/usr/src/debug/ngspice-44-1 
-ffile-prefix-map=/pub/devel/ngspice/ngspice-44-1.x86_64/src/ngspice-44=/usr/src/debug/ngspice-44-1 
-std=gnu11 -fopenmp -MT ivlng_la-icarus_shim.lo -MD -MP -MF 
.deps/ivlng_la-icarus_shim.Tpo -c 
/pub/devel/ngspice/ngspice-44-1.x86_64/src/ngspice-44/src/xspice/verilog/icarus_shim.c 
  -DDLL_EXPORT -DPIC -o .libs/ivlng_la-icarus_shim.o
/pub/devel/ngspice/ngspice-44-1.x86_64/src/ngspice-44/src/xspice/verilog/icarus_shim.c:21:10: 
fatal error: ngspice/cmtypes.h: No such file or directory
    21 | #include "ngspice/cmtypes.h" // For Digital_t
       |          ^~~~~~~~~~~~~~~~~~~
compilation terminated.
make: *** [Makefile:538: ivlng_la-icarus_shim.lo] Error 1

Hello Qucs and Ngspice developer,

The Qucs-S v24.3.2 has been released. This version contains no new 
features, only fixed a critical bug: 
https://github.com/ra3xdh/qucs_s/issues/948

The release page is available here: 
https://github.com/ra3xdh/qucs_s/releases/tag/24.3.2
Installation instructions: 
https://github.com/ra3xdh/qucs_s/wiki/Installation

Regards,
Vadim Kuznetsov