simple RC circuit

 Hi sali,

       According to your RC values I ran the same  simulation. At time =zero the output drops from 10 volt to 0. I dont know why you are getting this results. Here i attached my simulation screenshot.

Regards,

Karthik. 

Sali,

Please post your Netlist (input.scs) as that might then reveal what is wrong.

Thanks,

Andrew 

Hi Mr. Anderew,

This is the netlist

// Generated for: spectre
// Generated on: Mar 31 14:21:43 2014
// Design library name: Chua3
// Design cell name: rc
// Design view name: schematic
simulator lang=spectre
global 0
include "/CMC/kits/cmosp13.V1.8.0.0DM/IBM_PDK/cmrf8sf/V1.8.0.4DM/Spectre/models/design.scs"
include "/CMC/kits/cmosp13.V1.8.0.0DM/IBM_PDK/cmrf8sf/V1.8.0.4DM/Spectre/models/allModels.scs" section=tt

// Library name: Chua3
// Cell name: rc
// View name: schematic
R0 (net03 net04) resistor r=10
C0 (net04 0) capacitor c=10n ic=0
V0 (net03 0) vsource dc=0 type=pulse val0=10 val1=0 period=400n delay=0 \
        rise=1p fall=1p width=200n
simulatorOptions options reltol=1e-3 vabstol=1e-6 iabstol=1e-12 temp=27 \
    tnom=25 scalem=1.0 scale=1.0 gmin=1e-12 rforce=1 maxnotes=5 maxwarns=5 \
    digits=5 cols=80 pivrel=1e-3 sensfile="../psf/sens.output" \
    checklimitdest=psf
tran tran stop=200e-9 errpreset=conservative write="spectre.ic" \
    writefinal="spectre.fc" annotate=status maxiters=5
finalTimeOP info what=oppoint where=rawfile
modelParameter info what=models where=rawfile
element info what=inst where=rawfile
outputParameter info what=output where=rawfile
designParamVals info what=parameters where=rawfile
primitives info what=primitives where=rawfile
subckts info what=subckts  where=rawfile
saveOptions options save=allpub 

 Thanks KarthikJaiho , actually I'm still looking for the reason for this result, I was working in a large circuit that gives me a result different than the manual one, at the end I tested this simple circuit and I found this error which I didn't expect.

Thank you again for your help. 

I've run it through spectre, getting your results. If you think something is strange read your simulation logs:

  Notice from spectre during IC analysis, during transient analysis `tran'.
    C0: Initial condition computed for node net04 is in error by 909.091 mV.
        Decrease `rforce' to reduce error in computed initial conditions.  However, setting rforce too small may
result in convergence difficulties or in the matrix becoming singular.

 Now in your options rforce is set to "1", which is forcing a 1Ohm resistor over the cap to find a DC solution.
Reduce that rforce to smalller values. You still will get some error in the initial condition but not by that magnitude.

What are you trying to simulate? Would be a better idea to have a settled system before hitting it with the pulse.

Marc

 Thanks Marc for your help.

I'm reading now the log file, in the mean while I copied it below:

Cadence (R) Virtuoso (R) Spectre (R) Circuit Simulator
Version 7.2.0.109 64bit -- 6 Dec 2009
Copyright (C) 1989-2009 Cadence Design Systems, Inc. All rights reserved worldwide. Cadence, Virtuoso and Spectre are registered trademarks of Cadence Design Systems, Inc. All others are the property of their respective holders.

Protected by U.S. Patents:
        5,610,847; 5,790,436; 5,812,431; 5,859,785; 5,949,992; 5,987,238;
        6,088,523; 6,101,323; 6,151,698; 6,181,754; 6,260,176; 6,278,964;
        6,349,272; 6,374,390; 6,493,849; 6,504,885; 6,618,837; 6,636,839;
        6,778,025; 6,832,358; 6,851,097; 6,928,626; 7,024,652; 7,035,782;
        7,085,700; 7,143,021; 7,493,240; 7,571,401.

Includes RSA BSAFE(R) Cryptographic or Security Protocol Software from RSA Security, Inc.

Simulating `input.scs' on odin.doe.carleton.ca at 12:14:21 PM, Tue Apr 1, 2014 (process id: 24095).
Environment variable:
    SPECTRE_DEFAULTS=-I/CMC/kits/cmosp13.V1.8.0.0DM/IBM_PDK/cmrf8sf/V1.8.0.4DM/Spectre/models -f psfbin
Command line:
     \
        /CMC/tools/cadence/MMSIM_07.20.109_lnx86/tools.lnx86/spectre/bin/64bit/spectre  \
        input.scs +escchars +log ../psf/spectre.out +inter=mpsc  \
        +mpssession=spectre0_23761_1 -format sst2 -raw ../psf  \
        -I/CMC/kits/cmosp13.V1.8.0.0DM/IBM_PDK/cmrf8sf/V1.8.0.4DM/Spectre/models  \
        +lqtimeout 900 -maxw 5 -maxn 5
spectre pid = 24095

Loading /CMC/tools/cadence/MMSIM_07.20.109_lnx86/tools.lnx86/cmi/lib/64bit/5.0/libinfineon_sh.so ...
Loading /CMC/tools/cadence/MMSIM_07.20.109_lnx86/tools.lnx86/cmi/lib/64bit/5.0/libphilips_sh.so ...
Loading /CMC/tools/cadence/MMSIM_07.20.109_lnx86/tools.lnx86/cmi/lib/64bit/5.0/libsparam_sh.so ...
Loading /CMC/tools/cadence/MMSIM_07.20.109_lnx86/tools.lnx86/cmi/lib/64bit/5.0/libstmodels_sh.so ...
Auto-loading AHDL component.
Finished loading AHDL component in 0 s (elapsed).
Installed AHDL simulation interface.

Circuit inventory:
              nodes 2
          capacitor 1    
           resistor 1    
            vsource 1    

Time for parsing: CPU = 218.965 ms, elapsed = 828.433 ms.
Time accumulated: CPU = 218.965 ms, elapsed = 828.433 ms.
Peak resident memory used = 54.7 Mbytes.

Entering remote command mode using MPSC service (spectre, ipi, v0.0, spectre0_23761_1, ).

*************************************************
Transient Analysis `tran': time = (0 s -> 200 ns)
*************************************************

Notice from spectre during IC analysis, during transient analysis `tran'.
    C0: Initial condition computed for node net04 is in error by 909.091 mV.
        Decrease `rforce' to reduce error in computed initial conditions.  However, setting rforce too small may result in convergence difficulties or in the matrix becoming singular.

Important parameter values:
    start = 0 s
    outputstart = 0 s
    stop = 200 ns
    step = 200 ps
    maxstep = 4 ns
    ic = all
    skipdc = no
    reltol = 1e-03
    abstol(I) = 1 pA
    abstol(V) = 1 uV
    temp = 27 C
    tnom = 25 C
    tempeffects = all
    errpreset = moderate
    method = traponly
    lteratio = 3.5
    relref = sigglobal
    cmin = 0 F
    gmin = 1 pS

    tran: time = 8.095 ns    (4.05 %), step = 4 ns            (2 %)
    tran: time = 16.1 ns     (8.05 %), step = 4 ns            (2 %)
    tran: time = 28.1 ns       (14 %), step = 4 ns            (2 %)
    tran: time = 36.1 ns       (18 %), step = 4 ns            (2 %)
    tran: time = 48.1 ns       (24 %), step = 4 ns            (2 %)
    tran: time = 56.1 ns       (28 %), step = 4 ns            (2 %)
    tran: time = 68.1 ns       (34 %), step = 4 ns            (2 %)
    tran: time = 76.1 ns       (38 %), step = 4 ns            (2 %)
    tran: time = 88.09 ns      (44 %), step = 4 ns            (2 %)
    tran: time = 96.09 ns      (48 %), step = 4 ns            (2 %)
    tran: time = 108.1 ns      (54 %), step = 4 ns            (2 %)
    tran: time = 116.1 ns      (58 %), step = 4 ns            (2 %)
    tran: time = 128.1 ns      (64 %), step = 4 ns            (2 %)
    tran: time = 136.1 ns      (68 %), step = 4 ns            (2 %)
    tran: time = 148.1 ns      (74 %), step = 4 ns            (2 %)
    tran: time = 156.1 ns      (78 %), step = 4 ns            (2 %)
    tran: time = 168.1 ns      (84 %), step = 4 ns            (2 %)
    tran: time = 176.1 ns      (88 %), step = 4 ns            (2 %)
    tran: time = 188.1 ns      (94 %), step = 4 ns            (2 %)
    tran: time = 196.1 ns      (98 %), step = 4 ns            (2 %)
Number of accepted tran steps =             61
Initial condition solution time: CPU = 1 ms, elapsed = 256.062 us.
Intrinsic tran analysis time:    CPU = 2 ms, elapsed = 3.15404 ms.
Total time required for tran analysis `tran': CPU = 4 ms, elapsed = 8.13818 ms.
Time accumulated: CPU = 224.965 ms, elapsed = 1.01592 s.
Peak resident memory used = 59.1 Mbytes.

finalTimeOP: writing operating point information to rawfile.
modelParameter: writing model parameter values to rawfile.
element: writing instance parameter values to rawfile.
outputParameter: writing output parameter values to rawfile.
designParamVals: writing netlist parameters to rawfile.
primitives: writing primitives to rawfile.
subckts: writing subcircuits to rawfile. 

 Dear all,

I have another result when I modified the options under the transient analysis tab, but I need more explination to why the results are different now, please check the file.

This is the netlist file

// Generated for: spectre
// Generated on: Apr  1 14:36:52 2014
// Design library name: Chua3
// Design cell name: rc
// Design view name: schematic
simulator lang=spectre
global 0
include "/CMC/kits/cmosp13.V1.8.0.0DM/IBM_PDK/cmrf8sf/V1.8.0.4DM/Spectre/models/design.scs"
include "/CMC/kits/cmosp13.V1.8.0.0DM/IBM_PDK/cmrf8sf/V1.8.0.4DM/Spectre/models/allModels.scs" section=tt

// Library name: Chua3
// Cell name: rc
// View name: schematic
R0 (net03 net04) resistor r=10
C0 (net04 0) capacitor c=10n
V0 (net03 0) vsource type=pulse val0=10 val1=0 period=400n delay=0 rise=1p \
        fall=1p width=200n
ic net04=0
simulatorOptions options reltol=1e-3 vabstol=1e-6 iabstol=1e-12 temp=27 \
    tnom=25 scalem=1.0 scale=1.0 gmin=1e-12 rforce=1 maxnotes=5 maxwarns=5 \
    digits=5 cols=80 pivrel=1e-3 sensfile="../psf/sens.output" \
    checklimitdest=psf
tran tran stop=200e-9 errpreset=moderate ic=dc skipdc=no \
    write="spectre.ic" writefinal="spectre.fc" annotate=status maxiters=5
finalTimeOP info what=oppoint where=rawfile
modelParameter info what=models where=rawfile
element info what=inst where=rawfile
outputParameter info what=output where=rawfile
designParamVals info what=parameters where=rawfile
primitives info what=primitives where=rawfile
subckts info what=subckts  where=rawfile
save V0:p V0:p
saveOptions options save=allpub 

Thanks

 Dear all,

I tried another example but this time with a DC source it didn't work properly until I changed the options under the transient analysis tab.

The circuit and netlist is attached below.

Thank you in advance,

The netlist:

// Generated for: spectre
// Generated on: Apr  1 14:27:58 2014
// Design library name: Chua3
// Design cell name: rc2
// Design view name: schematic
simulator lang=spectre
global 0
include "/CMC/kits/cmosp13.V1.8.0.0DM/IBM_PDK/cmrf8sf/V1.8.0.4DM/Spectre/models/design.scs"
include "/CMC/kits/cmosp13.V1.8.0.0DM/IBM_PDK/cmrf8sf/V1.8.0.4DM/Spectre/models/allModels.scs" section=tt

// Library name: Chua3
// Cell name: rc2
// View name: schematic
R0 (net03 net04) resistor r=1
V0 (net03 0) vsource dc=8 type=dc
C1 (net04 0) capacitor c=10n ic=0
ic net04=0
simulatorOptions options reltol=1e-3 vabstol=1e-6 iabstol=1e-12 temp=27 \
    tnom=25 scalem=1.0 scale=1.0 gmin=1e-12 rforce=1 maxnotes=5 maxwarns=5 \
    digits=5 cols=80 pivrel=1e-3 sensfile="../psf/sens.output" \
    checklimitdest=psf
tran tran stop=60e-9 errpreset=moderate ic=all skipdc=yes \
    write="spectre.ic" writefinal="spectre.fc" annotate=status maxiters=5
finalTimeOP info what=oppoint where=rawfile
modelParameter info what=models where=rawfile
element info what=inst where=rawfile
outputParameter info what=output where=rawfile
designParamVals info what=parameters where=rawfile
primitives info what=primitives where=rawfile
subckts info what=subckts  where=rawfile
saveOptions options save=allpub 

 Hi Sali,

the simulator works properly in alll the cases you've shown, it just not delivered the results you expected. Ofcourse
their might be bugs from time to time, but when something like this is happening it is a good idea to first question
your expectations.

The last netlist works as you expected since you've pprovided that nodeset to net04, forcing a DC solution onto the simulator. In all other cases the simulator has to find it's own solution. A capacitor is treated as an open when looking for a DC solution, since
that won't work in your circuit  the simulator uses the "rforce" paramater and replaces the cap with a 1 Ohm resistor.  10 Ohm and
1 Ohm in series with a 10V voltage source delivers exactly what you see  as starting point in the simulations.

As circuit designer it is essential to understand your simulator as well as  having an expectations on the results and keep questioning both. 

Regards,

Marc

Thank you so much Marc for your help and support, I'm going to check the "rforce" parameter and do the simulation again.

Best regards,

Sali