Continue to Site

Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Register Log in

P1dB is greater than IIP3 ! Why?

Status
Not open for further replies.
M

Majid Rafei

Junior Member level 2
Joined
Aug 25, 2011
Messages
20
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Location
Tehran
Activity points
1,463
I am working on a LNA which has an active feedback. P-1dB and IIP3 are simulated using Spectre and results are as follows:
P-1dB:
p1dB_1stage.png
IIP3:
iip3_1stage.png

In addition, these parameters are simulated using HSPICE and results are as follows:
hspice_p1dB_iip3.png

I have two questions:

1) simulation conditions for both Spectre and HSPICE are the same, why results are different?

2) why P-1dB is greater than IIP3 (in normal condition IIP3 is 10 to 15 dBm greater than P1dB)?
 

pancho_hideboo said:
Show me analysis statements and option statements for both Spectre and HSPICE.
I think analysis conditions are different even if you use HB analysis for both Spectre and HSPICE.
Click to expand...

Spectre:
parameters freq2=301e6 Pin=-40 freq1=300e6
simulatorOptions options reltol=1e-3 vabstol=1e-6 iabstol=1e-12 temp=27 \
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
sweepqpss sweep param=Pin start=-50 stop=10 step=1 {
qpss qpss flexbalance=yes oversample=[1 1] funds=["f1" "f2"]
+ maxharms=[5 5] errpreset=conservative annotate=status

}

HSPICE:
.options post=2
.param Pin:dBm=-30.0
.param Pin=Pin:dBm
.param Pin:W='1.0e-3*pwr(10.0,Pin/10.0)' $ Change to Watts for sources
** 50 Ohm input port (incl. bias), 50 Ohm output port.
**
** Two-tone input source (DC blocked at this point)
**
Vin RFin 0 dc=0 power=1 z0=50 $ 50 Ohm src
+ HB Pin:W 0 1 1 $ tone 1
+ HB Pin:W 0 1 2 $ tone 2
Rload RFout 0 R=50
**
** HB test bench to measure IP3 and IP2
**
.HB tones=300e6,301e6 nharms=11 11 intmodmax=7
+SWEEP Pin:dBm -50.0 20 1.0

pancho_hideboo said:
You use exatrapolation point of Pin=-50dBm as post processing of Spectre results.
Do you use same value as post processing of HSPICE results ?
Click to expand...
Yes, I do.

pancho_hideboo said:
IIP3 is small signal distortion measure where Pin v.s. Pout is linear relation.
On the other hand, P1dB is essentially large signal drive distortion.
Click to expand...
So, how can i be sure that results are valid?
 

pancho_hideboo said:
Show me analysis statements and option statements for both Spectre and HSPICE.
I think analysis conditions are different even if you use HB analysis for both Spectre and HSPICE.
Click to expand...
Same results are achieved with hp analysis like qpss in Spectre:
simulatorOptions options reltol=1e-3 vabstol=1e-6 iabstol=1e-12 temp=27 \
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
sweephb sweep param=Pin start=-50 stop=10 step=1 {
hb hb oversample=[1 1] fundfreqs=[freq1 freq2] maxharms=[11
+ 11] errpreset=conservative tstabOpt=yes annotate=status

}
p1db_iip3_1stage.png
 

Majid Rafei said:
1) simulation conditions for both Spectre and HSPICE are the same,
why results are different?
Click to expand...
Show me analysis statements and option statements for both Spectre and HSPICE.
I think analysis conditions are different even if you use HB analysis for both Spectre and HSPICE.

You use exatrapolation point of Pin=-50dBm as post processing of Spectre results.
Do you use same value as post processing of HSPICE results ?

Majid Rafei said:
2) why P-1dB is greater than IIP3
(in normal condition IIP3 is 10 to 15 dBm greater than P1dB)?
Click to expand...
IIP3 is small signal distortion measure where Pin v.s. Pout is linear relation.
On the other hand, P1dB is essentially large signal drive distortion.

See equation, (11) and (14) of https://www.designers-guide.org/Modeling/modeling-rf-systems.pdf
 
Last edited:
Show me versions of Spectre and HSPICE.


Majid Rafei said:
Spectre:
sweepqpss sweep param=Pin start=-50 stop=10 step=1 {
qpss qpss flexbalance=yes oversample=[1 1] funds=["f1" "f2"]
+ maxharms=[5 5] errpreset=conservative annotate=status

}
........................
HSPICE:
.HB tones=300e6,301e6 nharms=11 11 intmodmax=7
+SWEEP Pin:dBm -50.0 20 1.0
Click to expand...
Conditions for HB Analyses are different.

Change HSPICE like following.
Code: 
.HB	tones=300e6,301e6	nharms=5	5	intmodmax=10
+SWEEP	Pin:dBm	-50.0	10	1.0

Majid Rafei said:
So, how can i be sure that results are valid?
Click to expand...
What do you want to mean ?

Majid Rafei said:
sweephb sweep param=Pin start=-50 stop=10 step=1 {
hb hb oversample=[1 1] fundfreqs=[freq1 freq2] maxharms=[11
+ 11] errpreset=conservative tstabOpt=yes annotate=status
Click to expand...
Set "intmodmax=22" for HSPICE.

Show me trace lines, 1st and 3rd using same tool.
I think you use Cadence Wavescan.

Plot Spectre and HSPICE results as over plot using Wavescan.
 
Last edited:
pancho_hideboo said:
Conditions for HB Analyses are different.

Change HSPICE like following.
Code: 
.HB	tones=300e6,301e6	nharms=5	5	intmodmax=10
+SWEEP	Pin:dBm	-50.0	10	1.0

Set "intmodmax=22" for HSPICE.

Show me trace lines, 1st and 3rd using same tool.
I think you use Cadence Wavescan.

Plot Spectre and HSPICE results as over plot using Wavescan.
Click to expand...
I did as you suggested and results are as follows:
Spectre:
p1db_iip3_1stage_new.png
HSPICE:
hspice_p1dB_iip3_new.png
No changes in results! :roll:

pancho_hideboo said:
What do you want to mean ?
Click to expand...
I mean, can i accept these results and report them, although I think that simulation conditions are standard and P1dB should be less than IIP3 by about 10 dBm! But, here IIP3 is less than P1dB! For me, results are strange.
 

Attachments

  • hspice_p1dB_iip3_new.png
    hspice_p1dB_iip3_new.png
    16.7 KB · Views: 103

Overplot results using same tool.

Show me versions of Spectre and HSPICE.

Majid Rafei said:
But, here IIP3 is less than P1dB!
For me, results are strange.
Click to expand...
When distortion is dominant for input characteristics, IIP3 is larger than P1dBin.

However if distortion is fairly occupied by output characteristics, IIP3 could be lesser than P1dBin.
 

pancho_hideboo said:
When distortion is dominant for input characteristics, IIP3 is larger than P1dBin.

However if distortion is fairly occupied by output characteristics, IIP3 could be lesser than P1dBin.
Click to expand...
Excuse me, I am confused. Would you please explain some more or refer me to a reference or paper about this issue?!
 


I think there is a feedback in the circuit.Have you ever checked the stability ?? If there is a stability issue, these results are valid at all.
Because P1dB Compression Point curve is pretty weird.
 

pancho_hideboo said:
No.
Plot Spectre results and HSPICE results using cadence ViVA or Sysnopsys Custom Waveviwer.
Click to expand...
I don't have ViVa and Waveviewer, although i think no changes will be on results!

pancho_hideboo said:
No.
Both don't show version of simulator.

Show me version of simulator.
If you don't know how to know it, see logfile of simulator.
Click to expand...
I looked for log files and find nothing. As I mentioned, I have used HSPICE version 2010 and Cadence version 6.14.

- - - Updated - - -

BigBoss said:
I think there is a feedback in the circuit.Have you ever checked the stability ?? If there is a stability issue, these results are valid at all.
Because P1dB Compression Point curve is pretty weird.
Click to expand...
Yes, as I mentioned in my first post, the circuit has an active feedback. However, I have checked the stability of the LNA by means of K_stability_factor, which is greater than 1 in whole bandwidth (K_stab > 1 is a necessary and sufficient condition for the stability of a LNA).
 

over plot using Cadence wavescan.

Compare results exactly.
I think you have Cadence ViVA since you use Cadence dfII version 6.1.4.

2010 is a version of HSPICE UI not simulator version.

Simulator version is located of head of logfile.
Surely see logfile.

If you use Spectre 6.X, it is too old.
HB-QPSS in Spectre 6.X is very suspicious.

I think you use Spectre 11.X or 14.X.
 
Last edited:

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top