The Designer's Guide Community Forum

The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl
Simulators >> Circuit Simulators >> ultrasim v.s. spectre
https://designers-guide.org/forum/YaBB.pl?num=1154797530

Message started by Aigneryu on Aug 5^th, 2006, 10:05am

Title: ultrasim v.s. spectre
Post by Aigneryu on Aug 5^th, 2006, 10:05am

Hi,

I am current using ultrasim to simulate a full chip extracted netlist. I am just wondering that if it is possible to co-simulate the circuit with spectre and ultrasim. Because I need higher accuracy in certain blocks.

Another question is: the hierarchy editor have ultrasim plug-ins for IC5033, but I cannot find it in IC5141, I like the way setting up the simulation accuracy for each block while using ultrasim with IC5033. DOes anybody know how to get the ultrasim plug-ins in HED for IC5141? Right I only get the AMS ones

Title: Re: ultrasim v.s. spectre
Post by sheldon on Aug 5^th, 2006, 3:25pm

Aigneryu,

1) Have you tried using UltraSim's high accuracy settings
on the block?

sim_mode=a or s
speed = 1 or 2

A rough approximation is that the simulator error controls
for speed=1 are similar to Spectre Conservative and
speed=2 are similar to Spectre Moderate

2) In IC5141, there is no plug-in for UltraSim. You need to
set View --> Properties to view the UltraSim simulator
controls.

Best Regards,

Sheldon

Title: Re: ultrasim v.s. spectre
Post by byang on Aug 5^th, 2006, 8:54pm

Hi, Aigneryu,

The difference between sim_mode=a and sim_mode=s is that sim_mode=a uses table model (faster) while sim_mode=s uses analytical model (slower). Other than that, they are the same.

I am very interested in this kind of accuracy problem. It is appreciated that you can tell some more information here. What kind of accuracy problem you have with certain blocks? How big is you full chip extracted netlist? What are the number of RC''s and the number of transistors in the netlist?

Thanks,

Baolin

Title: Re: ultrasim v.s. spectre
Post by Aigneryu on Aug 7^th, 2006, 11:02pm

I tried this setting before, but if I did not set the time step to as small as 1e-11, the lc osc in my pll can not start up correctly, it will damped to zero, much different from what I have seen in full spectre simulation

Title: Re: ultrasim v.s. spectre
Post by byang on Aug 8^th, 2006, 4:45pm

Hi, Aigneryu,

We have a solution to this type of problem. If you are interested, you can drop me a note at

byang@gemini-da.com

I am more than happy to share more information with you.

Regards,

Baolin

Title: Re: ultrasim v.s. spectre
Post by jbdavid on Aug 11^th, 2006, 12:52am

Ultrasim's timestep control is/was quite different than specter's - I had a similar problem a couple of years ago, and the R&D guys just had me add a maxstep to the particular blocks where the inaccuracy was..

Modes s (spice) a(analog) m(mixed) da(digital accurate) df(digital fast) are available in lowest to highest speed.. (if my memory serves me correctly.
each has an accuracy setting of 1-8..

In the Hierachy editor you can set these on a block by block level.. - really helps.
Jonathan

Title: Re: ultrasim v.s. spectre
Post by stefanw on Aug 27^th, 2006, 10:38am

Hi Aigneryu,

here are a few more hint on how to get and to keep the oscillator oscillation:

set the following options locally to the oscillator
- use maxstep to be about 20 point per period
example: .usim_opt maxstep_window = [0 10p] x1.x2.xosc
- use trapezoidal integration method
example: .usim_opt method=trap x1.x2.xosc
- make sure to initialize the oscillator properly, either pull
down one node to the low oscillator level, or inject an inductor
current at time=0

Since you are doing a full chip simulation you may want to
avoid to use maxstep for the entire circuit. Most likely the
rest of the circuit blocks will be fine with the UltraSim default
settings which is sim_mode=ms speed=5.

Best regards, Stefan