How to simulate a netlist - no schematic available????

S

Samiran

Guest
Hi guys.

I have to simulate a netlist corresponding to a circuit, but I don't
have the schematic of that. How I can correctly simulate the topology
(AC simulation)?

I have tried simulating the netlist by ocean script after creating the
same directory structure as automatically created by cadence inside
the simulation directory [I created:
"/home/samiran/simulation/cell_name/spectre/schematic/netlist"
directories. Inside "netlist" folder, I placed "netlist",
"netlistFooter", "netlistHeader" files, and one more folder named -
"amap" and created all necessary files that should be residing inside
"amap" folder]. But it didn't give me the correct result.

I have independently simulated the correspondent schematic by ocean
script and it gave correct result. I am not sure how to debug it. Is
there any relevant reference doc I can look into?

Please help me asap..I am fighting with it for last three days for
vain!!!!

Thanks & regards
Samiran
 
On Feb 22, 11:00 pm, Samiran <samiran....@gmail.com> wrote:
Hi guys.

I have to simulate a netlist corresponding to a circuit, but I don't
have the schematic of that. How I can correctly simulate the topology
(AC simulation)?

I have tried simulating the netlist by ocean script after creating the
same directory structure as automatically created by cadence inside
the simulation directory [I created:
"/home/samiran/simulation/cell_name/spectre/schematic/netlist"
directories. Inside "netlist" folder, I placed "netlist",
"netlistFooter", "netlistHeader" files, and one more folder named -
"amap" and created all necessary files that should be residing inside
"amap" folder]. But it didn't give me the correct result.

I have independently simulated the correspondent schematic by ocean
script and it gave correct result. I am not sure how to debug it. Is
there any relevant reference doc I can look into?

Please help me asap..I am fighting with it for last three days for
vain!!!!

Thanks & regards
Samiran
Click to expand...
Hi Samiran - what type of netlist do you have? If a CDL, you can
import the
CDL and create a schmatic. If you dont have a CDL, heres a few
workarounds.

1) Ive heard of tools that create a schematic from the layout. There
is probably a
skill routine that will also do this.
2) You could create a schematic from Assura using Solution ID:
11006792 which
shows how to run RCX without a schematic. It generates an Assura
netlist for layout
which can then be used a schematic. Once you have the .sdb file from
above, you
can then run the assura command vldbToCdl and import the
result. Kinda a round
about but it should work

Rick
 
On Feb 23, 10:52 pm, rick <ej...@pacbell.net> wrote:
On Feb 22, 11:00 pm, Samiran <samiran....@gmail.com> wrote:



Hi guys.

I have to simulate a netlist corresponding to a circuit, but I don't
have the schematic of that. How I can correctly simulate the topology
(AC simulation)?

I have tried simulating the netlist by ocean script after creating the
same directory structure as automatically created by cadence inside
the simulation directory [I created:
"/home/samiran/simulation/cell_name/spectre/schematic/netlist"
directories. Inside "netlist" folder, I placed "netlist",
"netlistFooter", "netlistHeader" files, and one more folder named -
"amap" and created all necessary files that should be residing inside
"amap" folder]. But it didn't give me the correct result.

I have independently simulated the correspondent schematic by ocean
script and it gave correct result. I am not sure how to debug it. Is
there any relevant reference doc I can look into?

Please help me asap..I am fighting with it for last three days for
vain!!!!

Thanks & regards
Samiran

Hi Samiran - what type of netlist do you have?   If a CDL, you can
import the
CDL and create a schmatic.  If you dont have a CDL, heres a few
workarounds.

1)  Ive heard of tools that create a schematic from the layout.  There
is probably a
skill routine that will also do this.
2)  You could create a schematic from Assura using Solution ID:
11006792   which
shows how to run RCX without a schematic.  It generates an Assura
netlist for layout
which can then be used a schematic.  Once you have the .sdb file from
above, you
can then run the assura command    vldbToCdl   and import the
result.   Kinda a round
about but it should work

Rick
Click to expand...
Hi Rick,

Its a simple netlist consisting of only passive components.....!!! And
one more thing - why you are talking about generation of schematic -
is the schematic required to simulate the netlist?? I want to simulate
the netlist w/o generating any schematic. Is there any way out?

Thanks,
Samiran
 
Samiran wrote, on 02/23/10 07:00:
Hi guys.

I have to simulate a netlist corresponding to a circuit, but I don't
have the schematic of that. How I can correctly simulate the topology
(AC simulation)?

I have tried simulating the netlist by ocean script after creating the
same directory structure as automatically created by cadence inside
the simulation directory [I created:
"/home/samiran/simulation/cell_name/spectre/schematic/netlist"
directories. Inside "netlist" folder, I placed "netlist",
"netlistFooter", "netlistHeader" files, and one more folder named -
"amap" and created all necessary files that should be residing inside
"amap" folder]. But it didn't give me the correct result.

I have independently simulated the correspondent schematic by ocean
script and it gave correct result. I am not sure how to debug it. Is
there any relevant reference doc I can look into?

Please help me asap..I am fighting with it for last three days for
vain!!!!

Thanks& regards
Samiran
Click to expand...
Hi Samiran,

There's no need to create an "amap" folder - all you need is netlist,
netlistHeader and netlistFooter (the last two can be empty files, but must exist).

You only say "But it didn't give me the correct result". Unfortunately that's
not much for me to go on - what you're doing _ought_ to work, but since you gave
no details as to:

a) what your OCEAN script looked like
b) what the actual problem was

it's virtually impossible for me to guess what you've done wrong. I don't,
unfortunately, have a crystal ball at my disposal.

Regards,

Andrew.
 
On Feb 24, 8:10 pm, Andrew Beckett <andr...@DcEaLdEeTnEcTe.HcIoSm>
wrote:
Samiran wrote, on 02/23/10 07:00:



Hi guys.

I have to simulate a netlist corresponding to a circuit, but I don't
have the schematic of that. How I can correctly simulate the topology
(AC simulation)?

I have tried simulating the netlist by ocean script after creating the
same directory structure as automatically created by cadence inside
the simulation directory [I created:
"/home/samiran/simulation/cell_name/spectre/schematic/netlist"
directories. Inside "netlist" folder, I placed "netlist",
"netlistFooter", "netlistHeader" files, and one more folder named -
"amap" and created all necessary files that should be residing inside
"amap" folder]. But it didn't give me the correct result.

I have independently simulated the correspondent schematic by ocean
script and it gave correct result. I am not sure how to debug it. Is
there any relevant reference doc I can look into?

Please help me asap..I am fighting with it for last three days for
vain!!!!

Thanks&  regards
Samiran

Hi Samiran,

There's no need to create an "amap" folder - all you  need is netlist,
netlistHeader and netlistFooter (the last two can be empty files, but must exist).

You only say "But it didn't give me the correct result". Unfortunately that's
not much for me to go on - what you're doing _ought_ to work, but since you gave
no details as to:

a) what your OCEAN script looked like
b) what the actual problem was

it's virtually impossible for me to guess what you've done wrong. I don't,
unfortunately, have a crystal ball at my disposal.

Regards,

Andrew.
Click to expand...
Due to a little mistake in netlisting the result was wrong. Now I am
getting desired result. But when I run the script w/o the amap folder
the simulation is going on fine, but after the simulation is over I
got an error:
_______________________________________________________________________________________________________________________
*Error* quotient: can't handle (nil / nil)
*Error* load: error while loading file - "testcsa.ocn"
_______________________________________________________________________________________________________________________


This is how the netlist looks like:
_______________________________________________________________________________________________________________________
// Library name: Samiran
// Cell name: TestMyCkt
// View name: schematic
COUTPUT (net9 0) capacitor c=1p
RM2 (0 net9) resistor r=1/gdM2
RM1 (net9 0) resistor r=1/gdM1
VINPUT (net013 0) vsource mag=1m type=sine ampl=1m freq=1K
GM1 (net013 0 net9 0) vccs gm=gmM1
_______________________________________________________________________________________________________________________


And this is how the script ("testcsa.ocn") looks like:
_______________________________________________________________________________________________________________________
ocnWaveformTool( 'wavescan )
simulator( 'spectre )
design( "/home/sdam/simulation/TestMyCkt/spectre/schematic/netlist/
netlist")
resultsDir( "/home/sdam/simulation/TestMyCkt/spectre/schematic" )
modelFile(
'("/usr/local/cadence/umc/UMC_18_CMOS/../Models/Spectre/
core_rf_v2d4.lib.scs" "tt")
'("/usr/local/cadence/umc/UMC_18_CMOS/../Models/Spectre/
io_rf_v2d3.lib.scs" "tt")
'("/usr/local/cadence/umc/UMC_18_CMOS/../Models/Spectre/
l_slcr20k_rf_v2d3.lib.scs" "typ")
'("/usr/local/cadence/umc/UMC_18_CMOS/../Models/Spectre/
mimcapm_rf_v2d3.lib.scs" "typ")
'("/usr/local/cadence/umc/UMC_18_CMOS/../Models/Spectre/
MM180_MIMCAP_V101.lib.scs" "mimcaps_typ")
'("/usr/local/cadence/umc/UMC_18_CMOS/../Models/Spectre/
MM180_REG18BPW_V123.lib.scs" "tt")
'("/usr/local/cadence/umc/UMC_18_CMOS/../Models/Spectre/
MM180_REG18_V124.lib.scs" "tt")
'("/usr/local/cadence/umc/UMC_18_CMOS/../Models/Spectre/
MM180_REG33BPW_V123.lib.scs" "tt")
'("/usr/local/cadence/umc/UMC_18_CMOS/../Models/Spectre/
MM180_REG33_V114.lib.scs" "tt")
'("/usr/local/cadence/umc/UMC_18_CMOS/../Models/Spectre/
MM180_RES_V133.lib.scs" "res_typ")
'("/usr/local/cadence/umc/UMC_18_CMOS/../Models/Spectre/
MM180_ZVT18_V121.lib.scs" "tt")
'("/usr/local/cadence/umc/UMC_18_CMOS/../Models/Spectre/
MM180_ZVT33_V113.lib.scs" "tt")
'("/usr/local/cadence/umc/UMC_18_CMOS/../Models/Spectre/
MM180_LVT33_V113.lib.scs" "tt")
'("/usr/local/cadence/umc/UMC_18_CMOS/../Models/Spectre/
MM180_LVT18_V113.lib.scs" "tt")
'("/usr/local/cadence/umc/UMC_18_CMOS/../Models/Spectre/
pad_rf_v2d3.lib.scs" "typ")
'("/usr/local/cadence/umc/UMC_18_CMOS/../Models/Spectre/
rnhr_rf_v2d3.lib.scs" "typ")
'("/usr/local/cadence/umc/UMC_18_CMOS/../Models/Spectre/
rnnpo_rf_v2d3.lib.scs" "typ")
'("/usr/local/cadence/umc/UMC_18_CMOS/../Models/Spectre/
rnppo_rf_v2d3.lib.scs" "typ")
'("/usr/local/cadence/umc/UMC_18_CMOS/../Models/Spectre/
vardiop_rf_v2d3.lib.scs" "typ")
'("/usr/local/cadence/umc/UMC_18_CMOS/../Models/Spectre/
varmis_18_rf_v2d3.lib.scs" "typ")
'("/usr/local/cadence/umc/UMC_18_CMOS/../Models/Spectre/
MM180_BJT_V112.mdl.scs" "")
'("/usr/local/cadence/umc/UMC_18_CMOS/../Models/Spectre/
MM180_DIODE_V113.mdl.scs" "")
)

gmM1 = 3.038m
gdM1 = 77.86u
gdM2 = 69.09u

p1 = outfile( "/home/sdam/csa.csv" "w" )

analysis('ac ?start "0" ?stop "1" ?annotate "status" )
desVar( "gdM2" gdM2)
desVar( "gmM1" gmM1)
desVar( "gdM1" gdM1)
envOption(
'vcoType ""
'pllPlugin ""
'firstRun nil
'enableArclength nil
'recover ""
'checkpoint ""
'spp ""
'autoDisplay t
'userCmdLineOption ""
'analysisOrder nil
'paramRangeCheckFile ""
)
option( 'reltol "1e-3"
'vabstol "1e-6"
'iabstol "1e-12"
'temp "27"
'tnom "27"
'scalem "1.0"
'scale "1.0"
'gmin "1e-12"
'rforce "1"
'maxnotes "5"
'maxwarns "5"
'digits "5"
'cols "80"
'pivrel "1e-3"
'ckptclock "1800"
'sensfile "../psf/sens.output"
'dochecklimit "no"
'checklimitdest "psf"
)
saveOption('save "allpub" )
saveOption( 'pwr "" )
saveOption( 'nestlvl "" )
saveOption( 'currents "" )
saveOption( 'subcktprobelvl "" )
saveOption( 'useprobes "" )
saveOption( ?saveahdlvars "" )
saveOption( ?modelParamInfo t )
saveOption( ?elementInfo t )
saveOption( ?outputParamInfo t )
temp( 27 )
run()
Av = value(mag((VF("/net9") / VF("/net013"))) 0)
plot( dB20((VF("/net9") / VF("/net013"))) )
fprintf( p1 "%g %g %g" 1/(1000000*gmM1) gdM1*1000000 gdM2*1000000 1/
Av)
newline(p1)
_______________________________________________________________________________________________________________________


Regards,
Samiran
 
Samiran wrote, on 02/25/10 05:30:
Av = value(mag((VF("/net9") / VF("/net013"))) 0)
plot( dB20((VF("/net9") / VF("/net013"))) )
fprintf( p1 "%g %g %g" 1/(1000000*gmM1) gdM1*1000000 gdM2*1000000 1/
Av)
Click to expand...
The problem is that you are referring to net names using "schematic names"
rather than "netlist names". Any name which begins with a "/" is assumed to be
the name in the schematic, and needs to be mapped to the corresponding netlist
name - using spectre's hierarchy delimiters, etc. If it doesn't begin with a
"/", it is assumed to be a netlist name.

So you probably just need:

Av = value(mag(VF("net9") / VF("net013")) 0)
plot( dB20(VF("net9") / VF("net013")) )

Assuming that's what the nets are called in the actual netlist.

Regards,

Andrew.
 
On Feb 25, 1:10 pm, Andrew Beckett <andr...@DcEaLdEeTnEcTe.HcIoSm>
wrote:
Samiran wrote, on 02/25/10 05:30:

Av = value(mag((VF("/net9") / VF("/net013"))) 0)
plot( dB20((VF("/net9") / VF("/net013"))) )
fprintf( p1 "%g %g %g" 1/(1000000*gmM1) gdM1*1000000 gdM2*1000000 1/
Av)

The problem is that you are referring to net names using "schematic names"
rather than "netlist names". Any name which begins with a "/" is assumed to be
the name in the schematic, and needs to be mapped to the corresponding netlist
name - using spectre's hierarchy delimiters, etc. If it doesn't begin with a
"/", it is assumed to be a netlist name.

So you probably just need:

Av = value(mag(VF("net9") / VF("net013")) 0)
plot( dB20(VF("net9") / VF("net013")) )

Assuming that's what the nets are called in the actual netlist.

Regards,

Andrew.
Click to expand...
Thanks!!! It worked!!!!!
 
You must log in or register to reply here.

Welcome to EDABoard.com

Sponsor

Back
Top