Spectre netlist with ADE

Guest
Hi,
I have created a spectre netlist (no schematic, just a netlist text
file) and I want to know if is it possible to use this netlist file as
input to run a simulation with ADE.

The other possibility is to run the simulation directly from the
command line (spectre my_netlist.scs). I tried this, but a lot of
error related to library files appear.

Thank you,
Pedro
 
I tried this, but a lot of
error related to library files appear.
You should use -I to specify path to the libraries. The other useful
Click to expand...
option is -E (preprocessing).
Take runSpectre script as a prototype.
 
Hi,

1. Passing through ADE is for any use in your case
2. It seems that you are missing the include of your Spectre Model
Cards. Your input netlist should come with an include of Spectre Model
files for each used model, something like:
include "PATH_TO_MODELS/yourModelFile.scs"
or
include "PATH_TO_MODELS/yourModelFile.scs" section=typ
if the section is needed (typ in here but could be else)

If you run spectre with the '-I' option as said before, something
like:
spectre -I/PATH_TO_MODELS ... input.scs (no blank after the -I)
then you don't need to write:
include "PATH_TO_MODELS/youModelFile.scs" but
include "yourModelFile.scs" is good enough since the -I option runs
the C preprocessor and searches the
directory dir for include files.

You can have one or more include files, depends how your models are
structured.
FYI:
UNIX> spectre -h include
or read the spectre User/Ref docs.

3. As explained by Andrew in a previous post :
" ... runSpectre is what the script is called if you're using the old
(obsolete, and
dropped in releases after IC5141) spectreS interface". So look at the
'runSimulation' from Spectre Direct rather.

4. It would helpful for the future if you post your error messages,
this is very handy for the community to help and debug ;-)

Hope it helps !

Riad.
 
Thank you very much for your answers,
I think I should explain a little bit more what my problem is (you are
right, the output with errors always help :) ). I created an schematic
that contains just a few vdc sources and a subcircuit that is repeated
6 times (this subcircuit contains 2 pmos and 3 nmos transistors). I
simulate this circuit using ADE and everything works fine. But, the
case is that I need to repeat this subciruit 1024 times (a matrix of
32x32 for a vision chip). So, I made a very simple c++ program that
writes my netlist (fullciruit.scs) containing 1024 subcircuits with
the corresponding 1024 vdc sources with different values simulating
different stimulus from different pixels.

The header of fullcircuit.scs (my c++ generated netlist), with its
corresponding includes and so, is exactly the same as the one in the
netlist that ADE created for the schematic I created first
(input.scs). As no other elements are added to the circuit (except for
the repetition of the same subcircuit) I guess that the included files
should be the same for both circuits (the models for the nmos and pmos
transistors are the same for the elements in input.scs and
fullcircuit.scs).

To run the simlation of fullcircuit.scs I put it in the same directory
as input.scs. Then I edit the runSimulation file (that is in the same
directory as input.scs and fullcircuit.scs) and replace the name of
the schematic file (input.scs) for the new schematic
(fullcircuit.scs). Then I type ./runSimulation in the command line,
and the following error appears:

Error found by spectre in `modp':`WTA31_310_0.MP1', in
`WTA':`WTA31_310_0',
during hierarchy flattening.
"/ic_tools/ams_v3.70/spectre/c35/cmos53.scs" 556: parameter
`dvthmat':
Unknown parameter name `mv_modp53' found in expression.

"/ic_tools/ams_v3.70/spectre/c35/cmos53.scs" 556: parameter
`dumat':
Unknown parameter name `mu_modp53' found in expression.


This error repeats several times.

As the simulations goes ok with ADE I thought that maybe the ADE
environment could accept a netlist as input, so I could try this
option, but it looks like I will have to look for another solution...

Thanks,
Pedro
 
pezuc@alumni.uv.es wrote, on 06/04/08 16:11:
Thank you very much for your answers,
I think I should explain a little bit more what my problem is (you are
right, the output with errors always help :) ). I created an schematic
that contains just a few vdc sources and a subcircuit that is repeated
6 times (this subcircuit contains 2 pmos and 3 nmos transistors). I
simulate this circuit using ADE and everything works fine. But, the
case is that I need to repeat this subciruit 1024 times (a matrix of
32x32 for a vision chip). So, I made a very simple c++ program that
writes my netlist (fullciruit.scs) containing 1024 subcircuits with
the corresponding 1024 vdc sources with different values simulating
different stimulus from different pixels.

The header of fullcircuit.scs (my c++ generated netlist), with its
corresponding includes and so, is exactly the same as the one in the
netlist that ADE created for the schematic I created first
(input.scs). As no other elements are added to the circuit (except for
the repetition of the same subcircuit) I guess that the included files
should be the same for both circuits (the models for the nmos and pmos
transistors are the same for the elements in input.scs and
fullcircuit.scs).

To run the simlation of fullcircuit.scs I put it in the same directory
as input.scs. Then I edit the runSimulation file (that is in the same
directory as input.scs and fullcircuit.scs) and replace the name of
the schematic file (input.scs) for the new schematic
(fullcircuit.scs). Then I type ./runSimulation in the command line,
and the following error appears:

Error found by spectre in `modp':`WTA31_310_0.MP1', in
`WTA':`WTA31_310_0',
during hierarchy flattening.
"/ic_tools/ams_v3.70/spectre/c35/cmos53.scs" 556: parameter
`dvthmat':
Unknown parameter name `mv_modp53' found in expression.

"/ic_tools/ams_v3.70/spectre/c35/cmos53.scs" 556: parameter
`dumat':
Unknown parameter name `mu_modp53' found in expression.


This error repeats several times.

As the simulations goes ok with ADE I thought that maybe the ADE
environment could accept a netlist as input, so I could try this
option, but it looks like I will have to look for another solution...

Thanks,
Pedro
Click to expand...
Well, there must be some difference in the files - the error suggests that it's
expecting to have a parameter mu_modp53 defined. Either the input.scs had this
parameter defined, or it included a file with that parameter definition with in.

Fundamentally ADE runs spectre with an input file - nothing particularly magic
about that. So if you're getting errors in a batch simulation, it's because you
have an error in your netlist or command line to spectre.

Regards,

Andrew.
 
Hi,

Since You've got this running from ADE, why don't you give a look at
the generated files in your run directory:
1. The 'input.scs' file is the main netlist, make sure that all the
'include' statements in this file are also in there with your stand
alone netlist
2. the 'runSimulation' shell script for any -I option and make sure
you do so in your own stand alone run.

Regards,

Riad.
 
You must log in or register to reply here.

Welcome to EDABoard.com

Sponsor

Back
Top