Instead, you should fix the frequency in s-parameters simulation in Spectre ( single point) then change the Line Length.
Also, look at Zm ( Port Input Impedance ) instead of s-parameters.
Beautiful. I am not really good with ADS, as I never worked on it. Well, now I will try it in ADS.
Both 1 and 2 are possible in any simulator.Beautiful. I am not really good with ADS, as I never worked on it. Well, now I will try it in ADS.
Yes, for sure, I still don't understand not only about tline but also many other things. That's why I am here to learn from experts like you.Simply still you can not understand parameters of tline.
Yes, for sure, I still don't understand not only about tline but also many other things. That's why I am here to learn from experts like you.
I was not sweeping the frequency parameter in the TLINE. Should I need to do that
I use Synopsys HSPICE from Cadence ADE.2.I have tried to sweep the Frequency of TLINE keeping length constant
for the open circuit case and short circuit case
** Generated for: hspiceD
** Generated on: Jun 17 11:47:47 2019
** Design library name: My_RFDE_Test
** Design cell name: test_circuitslave
** Design view name: schematic
.PARAM f0=1G nl0=0.25
.PROBE AC
+ I(v1) IP(v1)
+ I(v0) IP(v0)
.AC LIN 1001 1e-3 4e9
.TEMP 25.0
.OPTION
+ ACCURATE
+ ACOUT=0
+ LIST=3
+ ARTIST=2
+ INGOLD=2
+ INTERP
+ METHOD=GEAR
+ NOMOD
+ PARHIER=LOCAL
+ PROBE
+ PSF=2
+ RUNLVL=6
** Library name: My_RFDE_Test
** Cell name: test_circuitslave
** View name: schematic
t1 net03 0 net02 0 ZO=50 F=f0 NL=nl0 IC=0 , 0 , 0 , 0
t0 net08 0 0 0 ZO=50 F=f0 NL=nl0 IC=0 , 0 , 0 , 0
v1 net03 0 AC 1
v0 net08 0 AC 1
.END
simulator( 'hspiceD )
design( "/AHO/simulation/test_circuitslave/hspiceD/schematic/netlist/netlist" )
resultsDir( "/AHO/simulation/test_circuitslave/hspiceD/schematic" )
analysis('ac ?sweepType "linear" ?numPoints "1001" ?fstart "1e-3"
?fstop "4G" ?points "1G" )
desVar( "f0" 1G )
desVar( "NL0" 0.25 )
option( 'TEMPDC "25.0" )
save( 'i "/V0/PLUS" "/V1/PLUS" )
temp( 25.0 )
run()
Xin_short = imag((-1 / getData("/i(v0)" ?result "frequencySweep")))
Xin_open = imag((-1 / getData("/i(v1)" ?result "frequencySweep")))
plot( Xin_short ?expr '( "Xin_short" ) )
plot( Xin_open ?expr '( "Xin_open" ) )
I used Cadence Spectre from Cadence ADE.1.I have tried to sweep the length of TLINE keeping frequency constant
for the open circuit case and short circuit case
// Generated for: spectre
// Generated on: Jun 17 11:59:19 2019
// Design library name: My_RFDE_Test
// Design cell name: test_circuitslave
// Design view name: schematic
simulator lang=spectre
global 0
parameters f0=1G NL0=0.25
// Library name: My_RFDE_Test
// Cell name: test_circuitslave
// View name: schematic
T1 (net03 0 net02 0) tline z0=50 f=f0 nl=NL0
T0 (net08 0 0 0) tline z0=50 f=f0 nl=NL0
V1 (net03 0) vsource mag=1 type=dc
V0 (net08 0) vsource mag=1 type=dc
simulatorOptions options psfversion="1.1.0" reltol=1e-3 vabstol=1e-6 \
iabstol=1e-12 temp=25.0 tnom=25.0 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
ac ac freq=1G param=NL0 start=1e-3 stop=1 lin=1001 save=all \
annotate=status
save V0:p V1:p
saveOptions options save=selected saveahdlvars=all
simulator( 'spectre )
design( "/AHO/simulation/test_circuitslave/spectre/schematic/netlist/netlist" )
resultsDir( "/AHO/simulation/test_circuitslave/spectre/schematic" )
analysis('ac ?freq "1G" ?param "NL0" ?start "1e-3"
?stop "1" ?lin "1001" ?dec "" )
desVar( "f0" 1G )
desVar( "NL0" 0.25 )
envOption(
'analysisOrder list("ac")
)
save( 'i "/V0/PLUS" "/V1/PLUS" )
temp( 25.0 )
run()
Xin_short = imag((-1 / getData("/V0/PLUS" ?result "ac")))
Xin_open = imag((-1 / getData("/V1/PLUS" ?result "ac")))
plot( Xin_short ?expr '( "Xin_short" ) )
plot( Xin_open ?expr '( "Xin_open" ) )
"test_circuitslave_2.scs"Code:// Generated for: spectre // Generated on: Jun 17 11:59:19 2019 // Design library name: My_RFDE_Test // Design cell name: test_circuitslave // Design view name: schematic simulator lang=spectre global 0 parameters f0=1G NL0=0.25 // Library name: My_RFDE_Test // Cell name: test_circuitslave // View name: schematic T1 (net03 0 net02 0) tline z0=50 f=f0 nl=NL0 T0 (net08 0 0 0) tline z0=50 f=f0 nl=NL0 V1 (net03 0) vsource mag=1 type=dc V0 (net08 0) vsource mag=1 type=dc simulatorOptions options psfversion="1.1.0" reltol=1e-3 vabstol=1e-6 \ iabstol=1e-12 temp=25.0 tnom=25.0 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 ac ac freq=1G param=NL0 start=1e-3 stop=1 lin=1001 save=all \ annotate=status save V0:p V1:p saveOptions options save=selected saveahdlvars=all
What do you want to mean ?Which editior do you use to write these codes.
No.Also does connecting to "NoConn" instance means it is open circuited?
Surely see netlist.
Nothing.As pet T1 (net03 0 net02 0), net02 is connected to T1 on one side.
Where is the other side of net02 connected?.
What do you want to mean ?In the image you added, it is connected to "NoConn" instance.
How did you get that?
"basic/NoConn" is a symbol, that's all.does connecting a net to NoConn also mean leaving it as open?
We use cookies and similar technologies for the following purposes:
Do you accept cookies and these technologies?
We use cookies and similar technologies for the following purposes:
Do you accept cookies and these technologies?