Designer’s Guide Community

vivarf

Community Member

Offline

Posts: 35

ac gm simulation
Mar 11^th, 2009, 10:56pm

Hi all

In DC simulation, we can sweep the bias voltage (Vbias), and we can plot the dc I-V characteristics, and gm and gm'... over the large range of sweeping voltage (Vbias).

In "A 2GHz 16dBm IIP3 Low Noise Amplifier in 0.25μm CMOS Technology" paper the authors mentioned about AC characteristics, they can also plot the gm over input voltage range (it is AC Vinput, not Vbias).

Can anyone show me how to do this simulation to get that AC gm plot? Thank you very much.
You can check the paper out at this
http://ieeexplore.ieee.org/stamp/stamp.jsp?arnumber=01234383

Back to top

IP Logged

pancho_hideboo

Senior Fellow

Offline

Posts: 1424
Real Homeless

Re: ac gm simulation
Reply #1 - Mar 13^th, 2009, 8:16am

vivarf wrote on Mar 11^th, 2009, 10:56pm:

Can anyone show me how to do this simulation to get that AC gm plot?

Maybe this is a differential input transconductor. Is it correct ?
Apply swept DC values(-100mV ~ +100mV) as Vin_diff and then evaluate Y21 by executing AC analysis(2.5GHz) under each Vin_diff bias points.

g1 is calculated as g1=real(Y21).
g3 is calculated as g3=d²g1/dVin_diff².

Although I don't see the following, I guess g1=g1₊ + g1_-. Is this correct ?
vivarf wrote on Mar 11^th, 2009, 10:56pm:

http://ieeexplore.ieee.org/stamp/stamp.jsp?arnumber=01234383

Back to top

Kita━━━━━━(ﾟ∀ﾟ)━━━━━━ !!!!!
http://www7.plala.or.jp/ungeromeppa/flash/kita.html
http://www.youtube.com/watch?v=mjIxGh55bMM&feature=related

IP Logged

vivarf Community Member Offline Posts: 35	Re: ac gm simulation Reply #2 - Mar 15^th, 2009, 2:28am Thank you pancho. I may need to spend some time to carry the simulation as you suggested to confirm. About the second figure, I also guess g1 = g1+ + (-) g1-, not sure either :(
Back to top	IP Logged

vivarf

Community Member

Offline

Posts: 35

Re: ac gm simulation
Reply #3 - Mar 17^th, 2009, 4:45am

Hello pancho, sorry to bother you again

Quote:

Maybe this is a differential input transconductor. Is it correct ?
Apply swept DC values(-100mV ~ +100mV) as Vin_diff and then evaluate Y21 by executing AC analysis(2.5GHz) under each Vin_diff bias points.

I carried the AC analysis.
At the result window of AC analysis, as shown below

Quote:

g1 is calculated as g1=real(Y21).
g3 is calculated as g3=d2g1/dVin_diff2.

I supposed Y21 = d[mag(Iout)]/dVin_diff

Is it??

Back to top

IP Logged

pancho_hideboo

Senior Fellow

Offline

Posts: 1424
Real Homeless

Re: ac gm simulation
Reply #4 - Mar 17^th, 2009, 6:11am

vivarf wrote on Mar 17^th, 2009, 4:45am:

I supposed Y21 = d[mag(Iout)]/dVin_diff

No. You are completely misunderstanding.

Show me your netlist regarding
� signal sources statements
� analysis statements
� options statements
� save statements which you observe output currents.

I will correct your netlist.

And show me your definition of Y21 for differential output current.

I define it as Y21=(Iout₊-Iout_-)/(Vin₊-Vin_-).

Also I don't use Direct Plot of Cadence Spectre, since there exist many many unbelievable mistakes in definition.
I use Ocean Script where I write measurement by my own definition.
This is very common in Agilent Tool Environment.

Back to top

Kita━━━━━━(ﾟ∀ﾟ)━━━━━━ !!!!!
http://www7.plala.or.jp/ungeromeppa/flash/kita.html
http://www.youtube.com/watch?v=mjIxGh55bMM&feature=related

IP Logged

vivarf

Community Member

Offline

Posts: 35

Re: ac gm simulation
Reply #5 - Mar 17^th, 2009, 7:08am

Hi pancho, thank you for your quick response !

Here my circuit, I just re-build the one that mentioned in the paper.

The option of the DC bias , one is Vbs2+vin, the other is Vbs2-vin

The option of the port (for AC analysis??)

Those resistors are all 0 just to check the current, and after AC analysis I just take out the current of 1 branch of the circuit at terminal of R (first Fig)

The ac analysis setting

Back to top

IP Logged

pancho_hideboo Senior Fellow Offline Posts: 1424 Real Homeless	Re: ac gm simulation Reply #6 - Mar 17^th, 2009, 7:11am Show me your netlist regarding �signal sources statements �analysis statements �options statements �save statements which you observe output currents. And show me your definition of Y21 for differential output current. Why do you use port ? Anyway show me your netlist.
Back to top	Kita━━━━━━(ﾟ∀ﾟ)━━━━━━ !!!!! http://www7.plala.or.jp/ungeromeppa/flash/kita.html http://www.youtube.com/watch?v=mjIxGh55bMM&feature=related IP Logged

vivarf

Community Member

Offline

Posts: 35

Re: ac gm simulation
Reply #7 - Mar 17^th, 2009, 7:22am

The netlist:

// Generated for: spectre
// Generated on: Mar 17 22:37:31 2009
// Design library name:
// Design cell name:
// Design view name:
simulator lang=spectre
global 0
include "/cadence/IC5141/tools/dfII/samples/artist/ahdlLib/quantity.spectre"
parameters Vbs=.6 Rf_freq=455M Rf_freq2=450M Rf_pwr=-60 vin=0 Vbs2=500m \
� �n1=18 n2=18 xxx=8
include "/tsmc13rf/../models/RF_12_33_FSG.scs"

subckt b_wire _1 _2
parameters length
� �R0 (net5 _2) resistor r=0.2*length
� �L0 (_1 net5) inductor l=0.8n*length
ends b_wire
// End of subcircuit definition.

// Library name:
// Cell name:
// View name: schematic
R28 (net088 net0276 ) rppolyhri l=15.0u w=1u m=1

R6 (net0150 net095 ) rppolyhri l=15.0u w=1u m=1

R2 (net067 net090 ) rppolyhri l=4.05u w=8u m=1

R31 (net069 net068 ) rppolyhri l=15.0u w=1u m=1

R27 (net0276 net093 ) rppolyhri l=15.0u w=1u m=1

R39 (net0162 net072 ) rppolyhri l=15.0u w=1u m=1

R38 (net072 net0274 ) rppolyhri l=15.0u w=1u m=1

R26 (net0274 net076 ) rppolyhri l=15.0u w=1u m=1

R35 (net068 net078 ) rppolyhri l=15.0u w=1u m=1

R36 (net076 net069 ) rppolyhri l=15.0u w=1u m=1

R34 (net078 o\- ) rppolyhri l=15.0u w=1u m=1

R30 (net092 net0275 ) rppolyhri l=15.0u w=1u m=1

R37 (net0275 net0162 ) rppolyhri l=15.0u w=1u m=1

R32 (net089 net088 ) rppolyhri l=15.0u w=1u m=1

R33 (o\+ net089 ) rppolyhri l=15.0u w=1u m=1

R29 (net093 net092 ) rppolyhri l=15.0u w=1u m=1

R45 (net095 net094 ) rppolyhri l=15.0u w=1u m=1

R21 (net097 net0150 ) rppolyhri l=15.0u w=1u m=1

R1 (net099 net0103 ) rppolyhri l=15.0u w=1u m=1

R44 (net0101 net097 ) rppolyhri l=15.0u w=1u m=1

R46 (net0103 net090 ) rppolyhri l=15.0u w=1u m=1

R40 (net066 net0101 ) rppolyhri l=15.0u w=1u m=1

R0 (net0107 net099 ) rppolyhri l=15.0u w=1u m=1

R5 (net094 net0107 ) rppolyhri l=15.0u w=1u m=1

M20 (cmfb cmfb net066 net066) pmos_rf lr=130.0n wr=2u nr=8 m=1
M13 (bias1 net0116 net066 net066) pmos_rf lr=350.0n wr=2u nr=2 m=1
M9 (o\- cmfb net066 net066) pmos_rf lr=130.0n wr=4u nr=64 m=2
M50 (o\+ cmfb net066 net066) pmos_rf lr=130.0n wr=4u nr=64 m=2
M21 (net0160 net0160 net066 net066) pmos_rf lr=130.0n wr=2u nr=8 m=1
M14 (net0116 net0116 net066 net066) pmos_rf lr=350.0n wr=2u nr=2 m=1
I298 (0 net090) b_wire length=2
I296 (0 net062) b_wire length=2
K0 (net0112 0 net215 net025) transformer
C2 (net025 in\-) capacitor c=10p
C1 (net215 in\+) capacitor c=10p
M11 (net0116 bias1 net067 net067) nmos_rf lr=350.0n wr=2u nr=1 m=1
M19 (cmfb net0150 net0156 net0156) nmos_rf lr=130.0n wr=2u nr=4 m=1
M16 (net0156 bias1 net090 net090) nmos_rf lr=350.0n wr=2u nr=4 m=1
M17 (net0156 bias1 net090 net090) nmos_rf lr=350.0n wr=2u nr=4 m=1
M18 (net0160 net0162 net0156 net0156) nmos_rf lr=130.0n wr=2u nr=4 m=1
M15 (net0116 net0116 bias1 bias1) nmos_rf lr=130.0n wr=2u nr=16 m=1
M12 (bias1 bias1 net090 net090) nmos_rf lr=350.0n wr=2u nr=1 m=1
M64 (net018 in\- net043 net043) nmos_rf lr=130.0n wr=2u nr=xxx m=1
M6 (o\- net0132 net074 net074) nmos_rf lr=130.0n wr=2u nr=n1+n2 m=1
M68 (net043 in\+ net062 net062) nmos_rf lr=130.0n wr=2u nr=n2 m=1
M5 (net036 in\- net062 net062) nmos_rf lr=130.0n wr=4u nr=n1 m=1
M3 (net044 in\+ net040 net040) nmos_rf lr=130.0n wr=2u nr=xxx m=1
M4 (net040 in\- net062 net062) nmos_rf lr=130.0n wr=2u nr=n2 m=1
M0 (net014 in\+ net062 net062) nmos_rf lr=130.0n wr=4u nr=n1 m=1
M2 (o\+ net021 net084 net084) nmos_rf lr=130.0n wr=2u nr=n1+n2 m=1
R17 (net0132 net064) resistor r=10K
R7 (net014 net048) resistor r=0
R14 (in\- net070) resistor r=10K
R15 (net044 net096) resistor r=0
R12 (net036 net096) resistor r=0
R19 (net096 net074) resistor r=0
R3 (in\+ net042) resistor r=10K
R4 (net018 net048) resistor r=0
R18 (net048 net084) resistor r=0
R10 (net021 net050) resistor r=10K
V39 (net066 0) vsource dc=1.2 type=dc
V37 (net070 0) vsource dc=Vbs2-vin type=dc
V38 (net064 0) vsource dc=1 type=dc
V26 (net042 0) vsource dc=Vbs2+vin type=dc
V35 (net050 0) vsource dc=1 type=dc
PORT0 (net0112 0) port r=50 num=1 type=sine freq=Rf_freq dbm=Rf_pwr \
�freq2=Rf_freq2 dbm2=Rf_pwr mag=100m fundname="Rf1" fundname2="Rf2"
simulatorOptions options reltol=1e-3 vabstol=1e-6 iabstol=1e-12 temp=27.0 \
� �tnom=27 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
dcOp dc write="spectre.dc" maxiters=150 maxsteps=10000 annotate=status
dcOpInfo info what=oppoint where=rawfile
dc dc param=vin start=-450m stop=2 lin=200 oppoint=rawfile maxiters=150 \
� �maxsteps=10000 annotate=status
ac ac freq=400M param=vin start=-100m stop=100m lin=200 annotate=status
tran tran stop=50n step=10p maxstep=40p 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=all pwr=all currents=all useprobes=yes \
� �saveahdlvars=all

I just check single branch output, because in the paper, I think they use single-ended. And the expression of Y21:

Y21=deriv(i("/R18/MINUS" ?result "ac"))

Back to top

« Last Edit: Mar 17^th, 2009, 8:56am by vivarf »

IP Logged

pancho_hideboo

Senior Fellow

Offline

Posts: 1424
Real Homeless

Re: ac gm simulation
Reply #8 - Mar 17^th, 2009, 8:36am

I don't need full netlist.
Read my requests surely.

You should not use Resistor of 0ohm for observing current.
Instead use vsource of dc=0Volt or iprobe.

Your netlist is too dirty and wrong, so it is laborious to correct.

vivarf wrote on Mar 17^th, 2009, 7:22am:

PORT0 (net0112 0) port r=50 num=1 type=sine freq=Rf_freq dbm=Rf_pwr \
freq2=Rf_freq2 dbm2=Rf_pwr mag=100m fundname="Rf1" fundname2="Rf2"
K0 (net0112 0 net215 net025) transformer
C2 (net025 in\-) capacitor c=10p
C1 (net215 in\+) capacitor c=10p

R3 (in\+ net042) resistor r=10K
V26 (net042 0) vsource dc=Vbs2+vin type=dc

R14 (in\- net070) resistor r=10K
V37 (net070 0) vsource dc=Vbs2-vin type=dc

tran tran stop=50n step=10p maxstep=40p write="spectre.ic" \
� writefinal="spectre.fc" annotate=status maxiters=5
finalTimeOP info what=oppoint where=rawfile

Delete these lines completely. And replace to the followings.

V26 (in\+ 0) vsource type=dc dc=Vbs2+vin/2 mag=0.5 phase=0
V37 (in\- 0) vsource type=dc dc=Vbs2-vin/2 mag=0.5 phase=180

vivarf wrote on Mar 17^th, 2009, 7:22am:

ac ac freq=400M param=vin start=-100m stop=100m lin=200 annotate=status

Modify this line to the following.

ac ac freq=400M param=vin start=-100m stop=100m lin=200 annotate=status restart=yes

vivarf wrote on Mar 17^th, 2009, 7:22am:

Y21=deriv(i("/R18/MINUS" ?result "ac"))

You are misunderstanding completely.

Y21=i("/M2/D" ?result "ac")-i("/M6/D" ?result "ac")
g1=real(Y21), g3=deriv( deriv(g1) )

If you prefer single-ended output, Y21=i("/M2/D" ?result "ac").

I can't find out output terminals for g1₊ and g1_- correctly.
If you specify output terminals correctly for them, you can calculate g1₊ and g1_- by same definition as g1.

I've been very tired due to your unbelievable misunderstanding netlist.

Back to top

« Last Edit: Mar 17^th, 2009, 9:58am by pancho_hideboo »

Kita━━━━━━(ﾟ∀ﾟ)━━━━━━ !!!!!
http://www7.plala.or.jp/ungeromeppa/flash/kita.html
http://www.youtube.com/watch?v=mjIxGh55bMM&feature=related

IP Logged

vivarf Community Member Offline Posts: 35	Re: ac gm simulation Reply #9 - Mar 17^th, 2009, 8:54am My mistake, because I hardly use the script, so netlist is not familiar with me Pancho, thank you very much, I really appreciate.
Back to top	« Last Edit: Mar 17^th, 2009, 6:29pm by vivarf » IP Logged

Ken Kundert Global Moderator Offline Posts: 2384 Silicon Valley	Re: ac gm simulation Reply #10 - Mar 17^th, 2009, 9:36am In Spectre there is nothing wrong with using a zero ohm resistor to measure current, just like it is fine to use a zero volt voltage source. Using the iprobe is actually preferred because it is a very simple and light weight component. -Ken
Back to top	IP Logged

pancho_hideboo Senior Fellow Offline Posts: 1424 Real Homeless	Re: ac gm simulation Reply #11 - Mar 17^th, 2009, 9:55am Ken Kundert wrote on Mar 17^th, 2009, 9:36am: In Spectre there is nothing wrong with using a zero ohm resistor to measure current, just like it is fine to use a zero volt voltage source. I feel it comes to be slow if I use resistor of 0ohm instead of vsource of 0Volt when I run HB analysis of Cadence Spectre.
Back to top	Kita━━━━━━(ﾟ∀ﾟ)━━━━━━ !!!!! http://www7.plala.or.jp/ungeromeppa/flash/kita.html http://www.youtube.com/watch?v=mjIxGh55bMM&feature=related IP Logged

pancho_hideboo Senior Fellow Offline Posts: 1424 Real Homeless	Re: ac gm simulation Reply #12 - Mar 17^th, 2009, 7:17pm vivarf wrote on Mar 17^th, 2009, 8:54am: My mistake, because I hardly use the script, so netlist is not familiar with me Pancho, thank you very much, I really appreciate. Can you understand what is your misunderstanding ?
Back to top	Kita━━━━━━(ﾟ∀ﾟ)━━━━━━ !!!!! http://www7.plala.or.jp/ungeromeppa/flash/kita.html http://www.youtube.com/watch?v=mjIxGh55bMM&feature=related IP Logged

wave

Senior Member

Offline

Posts: 117
Silicon Valley

Re: ac gm simulation
Reply #13 - Mar 17^th, 2009, 7:36pm

Ken Kundert wrote on Mar 17^th, 2009, 9:36am:

In Spectre there is nothing wrong with using a zero ohm resistor to measure current, just like it is fine to use a zero volt voltage source. Using the iprobe is actually preferred because it is a very simple and light weight component.

-Ken

Ken - When I use tiny R's, I find abstol, reltol type of issues.
Usually atleast 100 mOhms is a good compromise.

Vdc=0 works well for me, as it back annotates well. �

I've never understood why iprobe exists. �
Doesn't back annotate that well.

Oddly, the STB analysis can use either device, and I'm curious if there is a tradeoff.
Usually I swap out my STB symbol for Metal R's, so it's always good to have a value that converges Cool

~Wave

Back to top

IP Logged

vivarf Community Member Offline Posts: 35	Re: ac gm simulation Reply #14 - Mar 17^th, 2009, 8:36pm Quote: Can you understand what is your misunderstanding ? I am still a little confused here The original definition: Y21=Id/Vin The result you defined is taken out current: Y21=i("/M2/D" ?result "ac") � (single-ended) From the original definition, I thought Y21 = deriv(i("/M2/D" ?result "ac"))
Back to top	IP Logged