Converge problem? how to solve it?

[savithru]

eldo convergence problem

hi all,

I am simulating the PLL (trans). But I am unable to do it as I am facing with convergence problem.

Spectre is giving some repost like "No DC solution found (no convergence)"..

Can you please tell me how to overcome the convergence problem..

Also It will be great if you can tell me why thse convergence problems comes ..

pls reply

Thanks
SavithRu

 

[watersky]

spectre gshunt

perhaps somewhere need to be set initial condition. for example some line is set to 0V as an initial condition.

 

[gte582w]

how to solve dc solution

try break it down to pieces, it would be easier to
understand which one gives you the trouble.

 

[sriramachandra]

converge problem

If u r using eldo then try to use .ic statements to initialise the VCO, then it will be fine

 

[020170]

iteratio steadyratio

In Hspice, Some option command solve this problem.

example )

.Option Gshunt = 1e-12

If you want more information, read Hspice manual.

Remenber : Example I represented is not always appropriate answer.

Designer Always thinks about How To Optimize Hspice Option Command Case by Case.

 

[srieda]

gshunt spectre

hi all,

I am simulating the PLL (trans). But I am unable to do it as I am facing with convergence problem.

Spectre is giving some repost like "No DC solution found (no convergence)"..

Can you please tell me how to overcome the convergence problem..

Also It will be great if you can tell me why thse convergence problems comes ..

pls reply

Thanks
SavithRu

Simulation is based on mathematical model of devices. When you try to simulate a circuit, the simulator tries to calculate the voltage and current values of all nodes/links by solving mathematical equations. As you know integration and differentiation are carried out by numerical methods. Most of the numerical methods are iterative in nature. i e they derive the solution by plugging in a random value and then try and converge to a single unique solution by manipulating the current input value. Sometimes it can so happen that such a iterative process leads to non-unique solutions or the solution may not converge into a single value at all..
The solution to such a situation is usually, to specify some initial conditions, so that the simulator starts to solve the equation with that particular initial condition.

I use eldo. I think its very efficient in that I have hardly seen any convergence issues at all... I do not know much about convergence in Hspice.

Hope this helps...

 

[RDRyan]

eldo dc convergence option

When I simulate PLL in hspice, I am also faced with the convergence problem. And after adding initional condition in the control line of VCO and the divider (TSPC divider), the hspice begain to work.
So, if you face with a convergent problem. you can consult the error message, find out which node is not convergent. and set a initional condition to the related circuit of that node.

 

[pankajdudulwar]

converge problem

go to the analysis menu and then enter the value for steadyratio to 0.1. Generally this value help in convergence in spectre. Try this if it didn't work let me know.
Pankaj

 

[Areky_qin]

how to solve spectre convergence

when i

Added after 1 minutes:

when I do simulations use hspice, convergence option and innitial condition set have to be added, all of them are important for simulation.

good luck

 

[paladinzlp]

I think you should set value of some floating net voltage.spectre's convergence is good.

 

[seeker137]

Assuming that all the blocks have been simulated and are converging and non-convergence happens only when they are all put together:
I will try the foll:
1.First iteration, relax all the options to low resolutions. Then save the operating point. Start the next simulation with tight resolution and using the previously saved operating point as nodeset conditions.
2. If that doesn't work try changing the integration algorithm.
3. apply initial conditions to known node values from calculations.
4. Ramping up supply and then running dc /tran...
Hope this helps.

 

[FastSpice]

Since it is about DC convergence, integration method doesn't matter. Relaxing reltol may help.

 

[allennlowaton]

use UIC (use initial condition) in the .tran analysis, that is if your on the transient analysis..
just like this: .TRAN .1n 100n UIC