ELDO SST and chopper amplifiers simulation

Status
Not open for further replies.
B

Braski

Full Member level 3
Joined
Dec 22, 2009
Messages
154
Helped
32
Reputation
64
Reaction score
28
Trophy points
1,308
Location
Florence (ITALY)
Activity points
2,384
does anyone know the SST analysis with the ELDO software? i need it to simulate a chopper amplifier, but i've never used this kind of simulation. Then i'll be able also to make noise simulation with SSTNOISE and transfer function with SSTXF, but i don't know the basis of these simulations.

could someone explain them and give some hints on the application to chopper stabilized amplifiers?
 

Braski said:
does anyone know the SST analysis with the ELDO software?
Click to expand...
It is a "Master Large Signal Steady State Analysis" as same as HB-Analysis of Agilent ADSsim, CR-Analysis of Agilent GoldenGate, (.hb and .sn) of Synopsys HSPICE-RF and PSS-Analysis of Cadence Spectre, etc.

Braski said:
could someone explain them and give some hints on the application to chopper stabilized amplifiers?
Click to expand...
There is no difficulty in simulation at all.
Use ".sst" as master analysis and ".sstac" and ".sstnoise" as slave analysis.
Here input signal is small signal for ".sstac" and clock signal is large signal periodical rectangular pulse wave for ".sst".
The Designer's Guide Community Forum - pss pac in eldo ?
**broken link removed**

See the followings.
https://www.edaboard.com/threads/169169/
The Designer's Guide Community Forum - switched capacitor integrator noise simulation results

Methodolgies of simulation are completely same even if you use any vendor's simulator.
The Designer's Guide Community Forum - ELDO SST Simulations - chopper amplifiers

The Designer's Guide Community Forum - Index is almost Cadence Tool Support Forum,
so you can never expect any helpful reply other than Cadence Tool there.
 
Last edited:
i've tried exactly the same you told. however, i can't manage to deal with convergence.

i've tried this setup:
20 Khz clock to a non overlap phase generator.
AC=1 for the input signal (Vd)

i've tried .sst with fund1=10KHz with 10 harmonics with .sstac, maybe i can try also 20 KHz with harmonics..
but i've got serious convergence issues...the circuit is not a simple chopper amplifier.
it is the right setup and i've to try to fix these issues? or should i try something different?

i really appreciate your advices.
 

pancho_hideboo said:
Show me netlist regarding analysis statements and signal source(clock and input) definitions.
Click to expand...

the analysis statement is:
.SST fund1 = 20K nharm =5
.SSTAC DEC 20 0.01 1Meg

the harmonic number here is a try. i've also tried 10 or more.

the clock is
V1 NETxx 0 DC 0 PULSE (0.0 3.3 0 0 0 25u 50u)

the input now is
V7 VIN 0 DC 0 AC 1

other option i've tried are
.OPTION SST_PRECONDITIONER=TIME_ACCURATE
.OPTION SST_MAXLINITER=500
.OPTION SST_TRAN_NPER=20

however, i've convergence issues.

other setup i've tried are to put input as VSIN with 100 Hz with nharm very large to cover the clock frequency.

---------- Post added at 10:18 ---------- Previous post was at 09:55 ----------

to be more accurate, i can say that my Newton residual dramatically increase after a few linear iterations, also with 20 harmonics
 

Braski said:
however, i've convergence issues.
Click to expand...
Show me log file.

Braski said:
the analysis statement is:
.SST fund1 = 20K nharm =5
the harmonic number here is a try. i've also tried 10 or more.
Click to expand...
Your "nharm" is too few.
".sst" analysis of Mentor eldo is a Harmonic Balance Method.
And you use pulse waveform which have very sharp rise and fall edges.

Simply observe time waveform at "NETxx" with .sst analysis of parallel connection of V1 and dummy resistor alone.
Is waveform of nharm=10 reasonable ?

Generally you have to set nharm=31 at least.

Braski said:
the clock is
V1 NETxx 0 DC 0 PULSE (0.0 3.3 0 0 0 25u 50u)
Click to expand...
It should be
.param tperiod=50u trise='tperiod/100' tfall=trise twidth='(tperiod-(trise+tfall))/2'
V1 NETxx 0 DC 0 PULSE (0.0 3.3 0 trise tfall twidth tperiod)
Click to expand...

Try to set analysis statements like followings.
.SST FUND1=20k NHARM1=31
.SSTAC DEC 20 0.01 1Meg
.OPTION SST_PRECONDITIONER=TIME_ACCURATE
.OPTION SST_MAXLINITER=500
.OPTION SST_TRAN_NPER=20
.OPTION SST_CONVERGENCE_HELP=TRANSIENT
.OPTION SST_OVRSMP=4
Click to expand...

If you can't get convergence success even using these settings, try to increase SST_OVRSMP or NHARM1.

In your case, both much higher harmonics and much time sample points are required.

See the followings.
The Designer's Guide Community Forum - maxstep in shooting-envlp of Cadence Spectre
https://www.edaboard.com/threads/195061/
 
Last edited:
Reactions: Braski

    B

    Braski

    Points: 2
    Helpful Answer Positive Rating
i've to say that on friday i'ìve reached convergence using pretransient convergence help and advanced_newton option. however, the results of SSTAC didn't make me satisfied. tomorrow i'll try again with more than 30 harmonics. ty, i'll let u know
 

Braski said:
however, the results of SSTAC didn't make me satisfied.
Click to expand...
Show me results and log file.

Braski said:
tomorrow i'll try again with more than 30 harmonics. ty, i'll let u know
Click to expand...
In your case, NHARM1=100 might be required for getting reasonable small signal analysis results such as ".sstac" and ".sstnoise".
 
Last edited:
Reactions: Braski

    B

    Braski

    Points: 2
    Helpful Answer Positive Rating
i can't directly show you my results, but i can say that they are reasonable close to what i did expect.

i've performed my last simulations with 40 harmonics, but it took 4 hours to complete the simulation. I'll try again going over with this number, but i am a bit worried about the database size (1.6 giga for 40 harmonics). maybe i'll reduce the number of points for decade (10 are too much i think)
 

Braski said:
i've performed my last simulations with 40 harmonics,
but it took 4 hours to complete the simulation.
Click to expand...
Try to use "Multi-Threading ability of Eldo".

There could be possibility to reduce simulation time also by other methods.

Braski said:
I'll try again going over with this number,
but i am a bit worried about the database size (1.6 giga for 40 harmonics).
Click to expand...
If you set up simulation properly, data size can be never large.

Reduce saving data for followings.
(1) node voltages or pin currents.
Don't save all nodes.
Save as small number of nodes as possible.

(2) harmonics data for ".sst"

(3) sideband data for ".sstac" and ".sstxf"


(1) is also true for ".tran".
But (2) and (3) are peculiar to ".sst", ".sstac" and ".sstxf".

When NHARM1 is large, there are many unnecessary data generated.
So you have to not save unnecessary data for both ".sst" and ".sstac".

For example, data for ".sstac" which you have interest on is only sideband=0, so don't save other sideband dara for ".sstac".
.PLOT SSTAC vdb(out_p).h(0) vdb(out_n).h(0)
Click to expand...
 
Last edited:
thank you again for your precious advices.

however, there's no big difference between 40 and 60 (almost none), so i think to have reached a sufficiently good result.

thank you very much.

i'll continue to study steady state analysis to properly know how it works.
 

Last edited:

you are right at every post! yopu should have great experience. i ran first with 40 harm SSTNOISE, than with 60 harm, and i found the residual flicker noise reduced of 1.5 dB in the second case. tomorrow i'll try among the others a simulation with 100 harms or over, oversampling, and other accuracy options. i ran all the sims with oversampling of 4.
 

there is one problem:

using a command like this:
.PLOT SSTAC vdb(out_p).h(0) vdb(out_n).h(0)

will unexpectly not limit the .wdb to only that wafeform, as you told and as it is written on the ELDORF handbook.
Any ideas?

>>>> SOLVED!
 

i should say that i greatly improve the convergence and the speed of the simulations simply using ideal clock generators, removing the digital gates necessary to realize the non-overlapping clocks. This can be useful for others if someone checks this topic.
 

Reactions: Braski

    B

    Braski

    Points: 2
    Helpful Answer Positive Rating
hi, sorry if i resume this old topic, but i still have a question:

during SSTNOISE and SSTAC (steady state noise analysis and steady state ac analysis) some points are skipped with the comment:

WARNING: noise frequency in SST spectrum: skip point

or similar.

Do you know how to fix this? Is it a problem of the algorithm or a wrong option?

i should add that some strange behaviour happens around these frequencies, like a drop of the response or a peak. i think this is because the plot use the value of the sst analysis to fill the graph, but this is wrong. how to fix?
 
Last edited:

Braski said:
WARNING: noise frequency in SST spectrum: skip point
Click to expand...
I think this means ill-convergence of small signal analysis such as SSTAC and SSTNOISE which are slave analyses for master large signal analysis, SST.

Try to set the followings in ".OPTION" statement.
SST_NOLIMIT_LINITER
SST_NODIVERGENCE=KRYLOV
Click to expand...

Or increase following.
.OPTION SST_MAXLINITER=500
Click to expand...
 
Last edited:

i can directly reply:

i think this is not a convergence issue. this is because when ELDO doesn't converge, it gives feedback about it! in this case, it just says that it skips the point. Other points around that frequency are calculated without problems, but follow the strange trend of the curve.

Max linear iteration limit is never hit. (set to 200)

I have to try only Krilov, but i am almost sure that it is not a convergence issue.

I tried also to look at the tutorial to see some examples. In those cases, the sstnoise band is set under the fundamental. FOr example, fundamental at 900 Mhz and noise band from 1 to 60 Mhz. So, i couldn't manage to figure out what it is doing.

The points skipped are those which coincide with the .sst harmonics. very strange.
 


Status
Not open for further replies.

Similar threads

Menu
Log in
Register
Cookies are required to use this site. You must accept them to continue using the site. Learn more…