Continue to Site

Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Register Log in

hspice issue"timestep too small"

Status
Not open for further replies.
T

Tiiu

Junior Member level 1
Junior Member level 1
Joined
Jun 6, 2006
Messages
18
Helped
1
Reputation
2
Reaction score
0
Trophy points
1,281
Activity points
1,397
.options cshunt=1e-13

when I simulate,the report says "timestep too small".
one suspicious warning is because I connected all nodes of one transistor together.
how should I deal with this?

thanks in advance!
 

hspice gshunt ramping

i think you have convergence
when i do the simulate with tran i got the problem too
you can see the hspice help
 
  • Like
Reactions: jren1

    J

    jren1

    Points: 2
    Helpful Answer Positive Rating
timestep too small trouble with node

did u connect source, drain and gate to one node.
 

site:www.edaboard.com tran option trap

Sometimes due to model non-convergence....but this could be improved if use Hspice 2006 version.....
 

spice timestep too small

hai Tiiu
(1)You can set options about convergence.
(2)Set some point's initial voltage
in a word, I think that is a convergece problem.

Perhaps that can help!
 

    T

    Tiiu

    Points: 2
    Helpful Answer Positive Rating
interal timestep too small

Thanks to all
I had added the initial voltages for the circuit and tried some spice options like:convergence=-1 dcon=1 BYPASS=1 CSHUNT=1 dvdt=0

but it doesn't help :cry:

what value I should assign to RELMOS,ABSMOS,DVDT and LVLTIM to get a better convergence?
 

cshunt hspice

Hi,
1. You could add:" .option gshunt=1e-14 and cshunt=1e-14" into the top of sim file. It coukd be useful
2. If it doesn't help, You can look at in the list file (at the end of list file) then see the point that spice announce timestep too small. You could find some thing relative convergence problem, forexample, you have some devices (as fuses) that their nodes are connected togetther.

That is my way to solve the problem that sometimes I got. Good luck!
 

timestep too small spice

harrytrinh said:
Hi,
1. You could add:" .option gshunt=1e-14 and cshunt=1e-14" into the top of sim file. It coukd be useful
2. If it doesn't help, You can look at in the list file (at the end of list file) then see the point that spice announce timestep too small. You could find some thing relative convergence problem, forexample, you have some devices (as fuses) that their nodes are connected togetther.

That is my way to solve the problem that sometimes I got. Good luck!
Click to expand...
hi harrytrinh,
I added the ".option gshunt=1e-14 and cshunt=1e-14"but it doesn't help.
meantime I found 3 nodes claiming non-convergence at the lis file.
Acctually these 3 nodes are the voltage sources within package model.
and yes,there are many devices whose nodes are connected together,but those devices are right be they should,I can't change them.
How should I deal with them?
 

I don't knot about that package model. But if you can remove that voltage source the problem will go away.
 

    T

    Tiiu

    Points: 2
    Helpful Answer Positive Rating
If you add the package model, try to add a small resistor in your power rail , say 1 ohm or 2 ohm, to decrease the Q factor of L of package model. Thease small resistor can be modeled as your metal line resistance, I thank that will not affect your ciecuit simulation accuracy and help your circuits convergence.
 

the non-convergency is a very "irksome" problem, when i simulate the whole circuit system, i encount this problem. who have a detailed experience to share about this?
 

use gmindc and other option to remove the convergance problem
 

Hey try and see if you are trying to ramp up your voltage sources too fast. Internal time step algorithm is used by HSPICE to extrapolate to the next voltage or current. If there is a sudden ramp in the voltage or current in any node, then it will give an internal timestep error.

Rather than changing GMINDC and G/C-SHUNT (which are used in high-frequency) try and type METHOD=GEAR. I think that GEAR method solves better than TRAP(trapezoidal).

I hope that it helps.
 

In your spice file, just add this..

.OPTIONS
+itl4=100

This works.
 

Thanks to all!!!
The issue is sloved by change ".option csdf "to ".option post" and add a statement ".option dcstep=1e-9":D
 

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top