A question about ADS Trans simulation

[guoluren]

ads tran

In ADS, can I use P1tone as input with trans simulation?

Since time domain source like Vtsine does not have source impedance, so do they give correct result when source impedance is important?

 

[kspalla]

tran simulation with ads

It will not be correct result impedance matching is important.
To simplify the problem, let say if the impedance is 50 ohm then just place a resistor with 50 ohm in series.

 

[fujian]

trans simulator 2009

Impendance matching is a difficult thing

 

[guoluren]

ads polar(dbmtow(10),90)

Thanks.

I also think source impedance should be included in trans simulation.

It is just in one of my simulations, the results with either a power source(P1tone, of course with source impedance) or a time source + 50 ohms resistor in series are different. It seems that the one with P1tone could be wrong. I have checked all the bias, nothing wrong. Really confused.

So has anybody compared these two cases? Or is there any documentation validating transient simulation with power source?

 

[pancho_hideboo]

trans simulator 09

It is just in one of my simulations,
the results with either a power source(P1tone, of course with source impedance) or a time source + 50 ohms resistor in series are different.
It seems that the one with P1tone could be wrong. I have checked all the bias, nothing wrong. Really confused.

"V_1Tone" with Series Resistor of 50ohm or "P_1Tone" with Z=50ohm always gives same results as "VtSine" with Series Resistor of 50ohm in Transient Analysis unless you do wrong setting in simulation.

Difference of them are phase.
"V_1Tone" and "P_1Tone" are Cosine Waveform(Oriented for HB Analysis orginally).
On the other hand, "VtSine" is Sine Waveform(Conventional SPICE Compatible).
http://edocs.soco.agilent.com/display/ads2009/P+1Tone+(Power+Source,+Single+Frequency)

So if you want to set "V_1Tone" or "P_1Tone" as Sine Waveform, you have to set their phase as -90degree.

Also see http://www.designers-guide.org/Forum/YaBB.pl?num=1231076499/8#8

Show me your netlists of ADS especially regarding signal sources, analysis statements and loads.

The followings are my netlist of ADS. Here all voltages at nodes, "a", "b" and "c" are completely same.

Options ResourceUsage=yes UseNutmegFormat=no \
　　　　TopDesignName="./aho.ds"

V_Source:SRC1 _net49 0 Type="V_1Tone" SaveCurrent=0 \
V[1]=polar(2,-90) V Freq[1]=1 GHz Vac=polar(1,0) V
R:R1 _net49 a R=50 Ohm Noise=yes
R:R2 a 0 R=50 Ohm Noise=yes

V_Source:SRC2 _net52 0 Type="VtSine" SaveCurrent=0 \
V[1]=if (_tr_state == 0) \
then (2 V)*exp(j*2*pi*((0)/360-(0 nsec)*(1 GHz)-.25)-(time-(0 nsec))*(0))*step((time-(0 nsec))+tinyreal) else 0 endif \
Freq[1]=1 GHz Vdc=0 V \
V_Tran=if (_tr_state == 1) \
then damped_sin(time,0,2 V,1 GHz,max(0,0 nsec),0,0) else (2 V)*step(((0 nsec)-time)-tinyreal)*sin(pi*(0)/180) endif
R:R3 _net52 b R=50 Ohm Noise=yes
R:R4 b 0 R=50 Ohm Noise=yes

PortORT1 c 0 Num=1 Z=50 Ohm P[1]=polar(1**2/(2*50),-90) Freq[1]=1 GHz Noise=yes Pac=polar(dbmtow(0),0)
R:R5 c 0 R=50 Ohm Noise=yes

Tran:Tran1 StartTime=0.0 nsec StopTime=3 nsec MaxTimeStep=1n/20 \
LimitStepForTL=yes TimeStepControl=2 TruncTol=7.0 ChargeTol=1.0e-14 IntegMethod=0 MaxGearOrder=2 \
Mu=0.5 MaxOrder=4 Freq[1]=1.0 GHz Order[1]=3 HB_Window=no \
HB_Sol=no ImpApprox=no ShortTL_Delay=1.0 psec ImpMode=1 UseInitCond=no \
LoadGminDC=no CheckKCL=yes CheckOnlyDeltaV=yes OverloadAlert=no DeviceBypass=no \
MaxIters=10 MaxItersDC=200 DevOpPtLevel=0 StatusLevel=2 OutputAllPoints=yes \
NoiseScale=1 ImpEnforcePassivity=yes \
OutputPlan="Tran1_Output"

OutputPlan:Tran1_Output \
Type="Output" \
UseNodeNestLevel=yes \
NodeNestLevel=2 \
UseEquationNestLevel=yes \
EquationNestLevel=2 \
UseSavedEquationNestLevel=yes \
SavedEquationNestLevel=2 \
UseDeviceCurrentNestLevel=no \
DeviceCurrentNestLevel=0 \
DeviceCurrentDeviceType="All" \
DeviceCurrentSymSyntax=yes \
UseCurrentNestLevel=yes \
CurrentNestLevel=999