The Designer's Guide Community Forum

The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl
Simulators >> Circuit Simulators >> charge pump psrr simulation
https://designers-guide.org/forum/YaBB.pl?num=1236161717

Message started by tempora123 on Mar 4^th, 2009, 2:15am

Title: charge pump psrr simulation
Post by tempora123 on Mar 4^th, 2009, 2:15am

Hello,

I have a Dickson charge pump circuit and would like to simulate the psrr of this block. I have read that pxf analysis can be used for that purpose. Pxf requires pss to be run first and here I have a problem because pss doesn't converge. I set up tstab long enough so that the charge pump output is settled (I checked that from tran analysis) but still I get:
"Conv norm = 33.2e+03, max dV(chargepump.clk_16M.DFF.MP1:int_d) = 3.30005 V"
and this conv norm number doesn't change from pss iteration to iteration. This node is inside a D flipflop where it is perfectly ok to be at either Vdd (3.3V) of GND so dV will be always be 3.3V every half clock period.
Does anyone know how to approach this convergence problem?

Thank you for your help.
BR

Title: Re: charge pump psrr simulation
Post by Frank Wiedmann on Mar 4^th, 2009, 4:32am

First of all, you should verify that you have correctly specified the fundamental frequency of the pss analysis (called "beat frequency" in the ADE form). Next, you should try to change the tstab value by some small amount (some fraction of the pss period). The node probably has a transition close to the beginning or the end of the pss interval. This usually causes convergence problems. Changing tstab should move the transition away from the edges of the interval.

Title: Re: charge pump psrr simulation
Post by Andrew Beckett on Mar 4^th, 2009, 5:48am

You also need to check that the circuit is not oscillating... (save the initial transient, and look around the circuit to see if it is behaving).

Regards,

Andrew.

Title: Re: charge pump psrr simulation
Post by tempora123 on Mar 5^th, 2009, 12:21am

Hello gents,

Thanks for your comment. Replying to your remarks:
- Yes, I have verified that fundamental freq is the same as the clock used in the circuit (I used autocalculate button)
- changing tstab hasn't helped. I saw strange thing though, even my tstab=30.2us, pss will not converge at 31. us so does this mean that my tstab is still not enough and pss extends this period by itself?
- the circuit doesn't oscillate by itself (it has an external clock though). I have checked its behaviour with tran analysis and everything is fine.

BR

Title: Re: charge pump psrr simulation
Post by Visjnoe on Mar 5^th, 2009, 12:29am

Dear,

I you have much trouble evaluating PSRR using PSS analysis, I think you will learn the same from a transient PSRR simulation...perhaps you pay somewhat in simulation time, but from a practical point of view a transient simulation will also allow you to assess the PSRR of your charge pump.

Regards

Peter

Title: Re: charge pump psrr simulation
Post by tempora123 on Mar 5^th, 2009, 3:34am

Hi,

But with tran analysis I would have to run lots of simulations for each disturer's frequency. I think it would take very long (haven't tested though). That is why PSS and PXF analysis are there to speed this up.

Anyway, if I cannot run pss and pxf I will probably do tran for a few frequencies which I'm interested in.

BR

Title: Re: charge pump psrr simulation
Post by Frank Wiedmann on Mar 5^th, 2009, 4:21am

tempora123 wrote on Mar 5^th, 2009, 12:21am:

- Yes, I have verified that fundamental freq is the same as the clock used in the circuit (I used autocalculate button)

There isn't any frequency divider in your circuit by any chance? In such a case, the autocalculate button will not work correctly.

Title: Re: charge pump psrr simulation
Post by tempora123 on Mar 5^th, 2009, 4:44am

Frank Wiedmann wrote on Mar 5^th, 2009, 4:21am:

tempora123 wrote on Mar 5^th, 2009, 12:21am:

- Yes, I have verified that fundamental freq is the same as the clock used in the circuit (I used autocalculate button)

There isn't any frequency divider in your circuit by any chance? In such a case, the autocalculate button will not work correctly.

Yes, there is a divider but after using auto calculate option I see the fundamental freq value is filled with the value from my ideal clock source in the schematic. Which is of course not correct as you mentioned.
Problem solved. Thanks.

Title: Re: charge pump psrr simulation
Post by Ken Kundert on Mar 5^th, 2009, 11:56am

A good way to diagnose these problems is to run a transient analysis with strobing such that the strobe interval is exactly equal to the period of what you specified as being the fundamental frequency to the PSS analysis (also misleadingly called the 'beat frequency'). Then look at all the waveforms. They should all go to constant values. If there is any non-transient repetitive behavior, you will not get PSS to converge because your circuit is not periodic in the period you have specified. This is generally due to some unexpected oscillation or an inappropriate value being specified for the fundamental frequency. In your case, it was the latter. As you found out, you have to account for the divider when setting the fundamental frequency.

-Ken