Stats

  • Locked Locked
  • Replies 3
  • Subscribers 143
  • Views 12675
  • Members are here 0
This discussion has been locked.
You can no longer post new replies to this discussion. If you have a question you can start a new discussion

Effective R calculation showing NA

Ymmen

Hi,

We are using IC6.1.8-64b.500.11

which spectre:
/tools/pdk/F01/U130S4/7.2/tools/mmsim18.10.463/tools/bin/spectre

spectre -W:
sub-version  18.1.0.463.isr10

I have been trying to backannotate "my_cell" with effective R value. "my_cell" is schematic with series of 3 resistors and two pins "in" and "out". I made a config view TB using av_extracted_RC(using PVS-Quantus) view of "my_cell" and ran a dc simulation with DC input of 1.2V at "in" pin. I have kept "Save DC Operating Point"  enabled and saving all voltage and current nodes from the Output options in ADEL. After simulation ended I descend into schematic view of "my_cell"(out of context). Then I go to Parasitics->Setup which already had result directory correctly filled under "Results directory for R calculation". When I go for "show parasitics"  option, it gives me capacitance values of each net but R is shown as "NA". Can you help me with where am I going wrong?

List of images/files

1. my_cell schematic

2. Output->save All form of ADEL

3. setup Parasitic form

4. Netlist

Fullscreen input_scs.txt Download 
// Generated for: spectre
// Generated on: Nov 12 15:15:09 2020
// Design library name: BRAZOS_ygoel
// Design cell name: back_annotate
// Design view name: config
simulator lang=spectre
global 0 GND_SUB!
parameters globalSigma=5 SubMod=0
include "/tools/cds2/released_models/RELEASE/internal/U130S4/F01/E5/Vsoi-1.15/modellib.scs" section=Typ
include "/tools/pdk/F01/U130S4/7.2/tools/5LM_BUMP/emxinterface/scalablemodels/emx_inductors.scs"
include "/tools/pdk/F01/U130S4/7.2/tools/cds06.18.110/tools/dfII/etc/cdslib/artist/functional/allFunc.scs"

// Library name: U130S1
// Cell name: gnd_sub
// View name: schematic
// Inherited view list: av_extracted schematic spectre
subckt gnd_sub _GND_SUB
    V0 (GND_SUB! _GND_SUB) vsource dc=0 type=dc
ends gnd_sub
// End of subcircuit definition.

// Library name: analogLib
// Cell name: presistor
// View name: schematic
// Inherited view list: av_extracted schematic spectre
subckt presistor PLUS MINUS
parameters c=0 r=1K a_tc1=0 a_tc2=0
    C1 (PLUS 0) capacitor c=c/2
    C2 (MINUS 0) capacitor c=c/2
    R0 (PLUS MINUS) resistor r=r tc1=a_tc1 tc2=a_tc2
ends presistor
// End of subcircuit definition.

// Inherited view list: av_extracted schematic spectre
// Library name: BRAZOS_ygoel
// Cell name: my_cell
// View name: av_extracted_RC
// View type: maskLayout
subckt my_cell in out
    R2 (\1\:in \2\:net5) pply w=8e-07 l=4.3e-07 ms=1 m=1
    R1 (\3\:net5 \2\:net6) pply w=8e-07 l=4.3e-07 ms=1 m=1
    R0 (\3\:net6 \2\:out) pply w=8e-07 l=4.3e-07 ms=1 m=1
    C1 (\2\:in net5) capacitor c=1.27322e-16
    C2 (\4\:net5 net6) capacitor c=1.22846e-16
    C3 (\4\:net6 \1\:out) capacitor c=1.30186e-16
    C4 (in GND_SUB!) capacitor c=6.93105e-17
    C5 (out GND_SUB!) capacitor c=7.38673e-17
    C6 (\2\:in GND_SUB!) capacitor c=9.23374e-17
    C7 (net5 GND_SUB!) capacitor c=1.38343e-16
    C8 (\4\:net5 GND_SUB!) capacitor c=1.3972e-16
    C9 (net6 GND_SUB!) capacitor c=3.21566e-16
    C10 (\4\:net6 GND_SUB!) capacitor c=3.20097e-16
    C11 (\1\:out GND_SUB!) capacitor c=9.68324e-17
    Rg1 (\2\:in in) presistor c=0 r=0.5381
    Rg2 (\4\:net5 net5) presistor c=0 r=1.9957
    Rg3 (\4\:net6 net6) presistor c=0 r=5.748
    Rg4 (out \1\:out) presistor c=0 r=0.5965
    Rh_1_1 (\1\:in \2\:in) presistor c=0 r=0.0275
    Rh_1_2 (net5 \2\:net5) presistor c=0 r=0.0275
    Rh_1_3 (\3\:net5 \4\:net5) presistor c=0 r=0.0275
    Rh_1_4 (net6 \2\:net6) presistor c=0 r=0.0275
    Rh_1_5 (\3\:net6 \4\:net6) presistor c=0 r=0.0275
    Rh_1_6 (\1\:out \2\:out) presistor c=0 r=0.0275
ends my_cell
// End of subcircuit definition.

// Library name: BRAZOS_ygoel
// Cell name: back_annotate
// View name: schematic
// Inherited view list: av_extracted schematic spectre
V0 (net29 0) vsource dc=1.2 type=dc
I3 (0) gnd_sub
I11 (net29 0) my_cell
simulatorOptions options psfversion="1.1.0" reltol=1e-3 vabstol=1e-6 \
    iabstol=1e-12 temp=27 tnom=27 homotopy=all 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" dochecklimit=yes checklimitdest=both \
    bsimsoi_va=yes 
dcOpCheckLimit checklimit checkallasserts=yes severity=none
dcOp dc write="spectre.dc" save=all maxiters=150 maxsteps=10000 \
    annotate=status
dcOpInfo 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
asserts info what=assert where=rawfile
save net29 I11:1 I11:2 I11.net6 I11.R0:2 I11.R1:1 I11.net5 I11.R1:2 \
    I11.R2:1 I11.R2:2 
saveOptions options save=all currents=all

Parents
  • Andrew Beckett

    I think the issue may be because the presistor has been netlisted as a subckt. I would suggest that you set the view list in your config to have spectre before schematic (normally the default) or at the very least to pick spectre as the View to Use for the presistor.

    Can you try that? You'll need to re-simulate of course.

    Andrew.

  • Ymmen
    in reply to Andrew Beckett

    Yes it worked! It is just presistor which has schematic view. Others like pcapacitor doesn't have schematic view hence it was using spectre view. So capacitance was getting reported but not resistance. It makes sense. Thank you!

Reply
  • Ymmen
    in reply to Andrew Beckett

    Yes it worked! It is just presistor which has schematic view. Others like pcapacitor doesn't have schematic view hence it was using spectre view. So capacitance was getting reported but not resistance. It makes sense. Thank you!

Children
  • Andrew Beckett
    in reply to Ymmen

    The capacitors are shown directly anyway as they can just be summed; to find the effective equivalent resistance needs a solver, which is why simulation is used to find that information.

    Anyway, glad that fixed it!

    Andrew.

Community Guidelines

The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.