Post-layout simulation problem

[jalinmes]

Transient post-layout simulation- Is this reliable- Option/ Analog setup

Hi everyone,

I am now doing a post-layout simulation for my buck converter. everything worked fine and I started adding additional two comparators as over voltage & over current protection purpose.

The whole thing worked fine even after adding those in schematic level simulation but couldnt run and seemed like frozen and not proceeding to anything, not even show me any error sign. It simply couldnt run.


Because of the problem above, I modified the analog setup in option / analog in analog environment and again the simulation can run but I am not sure how reliable this is.

Can anyone please tell me how big the iabstol can it go and how small gmin can it go.

The attached image is the important setup parameters. Is there any problem for this? and how reliable of this simulation is.

it is done in " homotype=dptran"
maxstep 2us
skipdc =no
reltol=10e-3
abstolV=1uV
abstolI=1mA
errpreset=liberal
method gear2
lteratio=3.5
relref=sigglobal
cmin=0F
gim=1pS
mos_vre=50mV

 

[wdssll]

for chartered 018 process, the minimum iabstol is about 4E-16, same for vabstol. gmin can be set to 0. it is used to provide a very small conductance for non linear devices, in case it is turned off. i think by setting gmin to 0 will solve the problem.

---------- Post added at 01:22 AM ---------- Previous post was at 01:21 AM ----------

you should set gmin to 0 if your circuit is sensitive to leakage current.

 

[jalinmes]

setting gmin = 0 , didnt work. I changed the parameters to as follow. It worked. Do you know how accurate this can be if I run by tran conservative but set iabstol to 1uA. And where can I find the definition of those parameters? such as vabstol, gmin, iabstol, pivrel, reltol, etc. Thank you.

it is done in " homotype=dptran"
maxstep 2us
skipdc =no
reltol=10e-3
abstolV=1uV
abstolI=1uA
errpreset=conservative
method gear2
lteratio=3.5
relref=sigglobal
cmin=0F
gim=1pS
mos_vre=50mV

 

[wdssll]

Here is the instructions from cadence manual.

Suggestions for Improving Transient Analysis Accuracy

Verify that the circuit biased up properly. If it did not, there might be a problem in the topology, the models, or the power supplies.

Be sure you are using appropriate models and that the model parameters are consistent and correct. Check the operating point of each device.

Set the transient analysis parameter errpreset to conservative.

If there is a charge conservation problem, use only charge-conserving models if you are not already doing so. Then tighten reltol to increase accuracy. (With the Spectre simulator, only customer-installed models might not be charge conserving.)

Be sure that gmin is not influencing the solution. If possible, set gmin to 0 (in an options or set statement).

If a solution exhibits point-to-point ringing, set the integration method in the transient analysis to Gear’s second-order backward-difference formula (method=gear2only).

If a low-loss resonator exhibits too much loss, set the integration method in the transient analysis to the trapezoidal rule (method=traponly).

If the initial conditions used by the Spectre simulator are not the same as the ones you specified, decrease the rforce parameter in the options or set statements until the initial conditions are correct.

If the Spectre simulator does not accurately follow the turn-on transient of an oscillator, set the maxstep parameter of the transient analysis to one-tenth the size of the expected period of oscillation or less.