The Designer's Guide Community Forum

The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl
Simulators >> Circuit Simulators >> Convergence problem! how to solve it?
https://designers-guide.org/forum/YaBB.pl?num=1181642349

Message started by savithru on Jun 12^th, 2007, 2:59am

Title: Convergence problem! how to solve it?
Post by savithru on Jun 12^th, 2007, 2:59am

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

Title: Re: Convergence problem! how to solve it?
Post by Geoffrey_Coram on Jun 12^th, 2007, 4:10am

savithru wrote on Sep 29^th, 1973, 8:23am:

Read the rest of the message from Spectre, which usually tells you which nodes are causing problems ...

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

Because you made a mistake in your circuit. Or you have bad models. Or any of a hundred different reasons, none of which we can even guess at without knowing more about your circuit. Is it transistor-level or behavioral? Do you have any dependent sources? Any "bsource" elements?

Title: Re: Convergence problem! how to solve it?
Post by simon2 on Sep 23^rd, 2007, 3:15am

Hi Geoffrey,
this response is probably too late to help you, so I am posting for the benefit of other latecomers ....

You will find under one of the menu lists in the Analog Design Environment window, something called "Analog ...", open this and you will find the simulator convergence settings. Also, somewhere you will find a menu item called nodeset - think about what voltages should be at strategic nodes like logic totem poles, casccode inputs, diff-pair "tails" and the like, then put in a value on the schematic using the nodeset item.
If you intend to become an analogue designer as a career, I suggest you get hspice - you will find that it is much easier to access these features and can do so with a line or two of text in your scripts. The downside is, hspice's convergence is not quite as stable on large circuits so requires such intervention more often than spectre, however on circuits that converge in neither simulator, hspice is easier to sort out.

Convergence is a large and complex topic but as an experienced spicer, I can make a few general comments that might help:
- Homotopy based simulators seem more stable than others
- Gear method seems better at DC convergence than others, however occasionally
- Backward-Euler may solve transient convergence faster than others
- Gmath and Source-ramping techniques seem to overcome convergence issues more efficently.
- Often a circuit will converge for tran but not DC, so consider using only tran in your design flow (be prepared to do a lot of post simulation processing).
- Make copious use of 1e12 resistors to define bias points. Mostly these resistors should be connected to pull the circuits into the "off" state rather the "on" state.
- Ensure that gmin and gmindc are not too large, that they effect the circuits behaviour (check the run file to see what value the simulator has assigned to these, will give a good indication if the convergence point is correct).
- try altering PIVREL and PIVTOL from default values; these affect how the matrix is solved and can have an enormous effect on the ability of the simulator to find a solution.

Hope this helps.

Cheers,
SimonH.

Title: Re: Convergence problem! how to solve it?
Post by simon2 on Sep 23^rd, 2007, 3:21am

Additional to my previous post, this subject:

- try partitioning your circuit into sub-circuits, then note the time the simulator takes to converge on these, whilst working on the strategic placement of the 1e12 resistors and the simulator settings, should allow you to build a more stable and robust convergence solution. You can also then replace difficult sub-circuit netlists with simpler resistor-controlled source descriptions, to allow you to work through the convergence issues.

Cheers,
SimonH.

Title: Re: Convergence problem! how to solve it?
Post by Geoffrey_Coram on Sep 24^th, 2007, 9:11am

simon2 wrote on Sep 23^rd, 2007, 3:15am:

Hi Geoffrey,
this response is probably too late to help you, so I am posting for the benefit of other latecomers ....

It was savithru who was having trouble ...

Quote:

If you intend to become an analogue designer as a career, I suggest you get hspice - you will find that it is much easier to access these features and can do so with a line or two of text in your scripts. The downside is, hspice's convergence is not quite as stable on large circuits so requires such intervention more often than spectre, however on circuits that converge in neither simulator, hspice is easier to sort out.

Spectre has a command-line interface as well; don't know what your comment is really trying to say.

Quote:

Convergence is a large and complex topic but as an experienced spicer, I can make a few general comments that might help:
- Homotopy based simulators seem more stable than others
- Gear method seems better at DC convergence than others, however occasionally

Gear is an integration method for transient analysis -- what does this have to do with dc convergence? I don't think the transient integration method is used for the pseudo-transient.

Quote:

- Often a circuit will converge for tran but not DC, so consider using only tran in your design flow (be prepared to do a lot of post simulation processing).

If it can converge for tran, then you should be able to generate a nodeset for running dc. Unless your simulator doesn't actually find the time=0 solution (I've heard some of the fast spice simulators don't, they just start running and hope that the problems resolve themselves during the transient).