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.

hspice issue"timestep too small"

Status
Not open for further replies.

Tiiu

Junior Member level 1
Joined
Jun 6, 2006
Messages
19
Helped
1
Reputation
2
Reaction score
0
Trophy points
1,281
Activity points
1,410
.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!
 

wjlzhx

Member level 5
Joined
Apr 14, 2005
Messages
82
Helped
4
Reputation
8
Reaction score
1
Trophy points
1,288
Activity points
1,785
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

    jren1

    Points: 2
    Helpful Answer Positive Rating

gharuda

Member level 3
Joined
May 30, 2006
Messages
67
Helped
12
Reputation
22
Reaction score
5
Trophy points
1,288
Location
Bengaluru
Activity points
1,994
timestep too small trouble with node

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

paulux

Advanced Member level 4
Joined
May 16, 2005
Messages
112
Helped
11
Reputation
22
Reaction score
2
Trophy points
1,298
Activity points
2,339
site:www.edaboard.com tran option trap

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

paladinzlp

Full Member level 2
Joined
Feb 2, 2005
Messages
134
Helped
4
Reputation
8
Reaction score
0
Trophy points
1,296
Activity points
916
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!
 

    Tiiu

    Points: 2
    Helpful Answer Positive Rating

Tiiu

Junior Member level 1
Joined
Jun 6, 2006
Messages
19
Helped
1
Reputation
2
Reaction score
0
Trophy points
1,281
Activity points
1,410
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?
 

harrytrinh

Member level 2
Joined
May 21, 2006
Messages
45
Helped
5
Reputation
10
Reaction score
1
Trophy points
1,288
Activity points
1,601
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!
 

Tiiu

Junior Member level 1
Joined
Jun 6, 2006
Messages
19
Helped
1
Reputation
2
Reaction score
0
Trophy points
1,281
Activity points
1,410
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!
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?
 

harrytrinh

Member level 2
Joined
May 21, 2006
Messages
45
Helped
5
Reputation
10
Reaction score
1
Trophy points
1,288
Activity points
1,601
I don't knot about that package model. But if you can remove that voltage source the problem will go away.
 

    Tiiu

    Points: 2
    Helpful Answer Positive Rating

simonkuo

Junior Member level 3
Joined
Nov 2, 2004
Messages
29
Helped
2
Reputation
4
Reaction score
0
Trophy points
1,281
Activity points
276
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.
 

wanily1983

Member level 5
Joined
Mar 22, 2005
Messages
92
Helped
1
Reputation
2
Reaction score
1
Trophy points
1,286
Activity points
2,093
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?
 

manissri

Full Member level 5
Joined
Apr 16, 2005
Messages
279
Helped
9
Reputation
18
Reaction score
3
Trophy points
1,298
Activity points
3,259
use gmindc and other option to remove the convergance problem
 

Vamsi Mocherla

Advanced Member level 1
Joined
Sep 6, 2004
Messages
469
Helped
72
Reputation
144
Reaction score
11
Trophy points
1,298
Activity points
5,136
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.
 

ubetimcool

Newbie level 4
Joined
Jun 13, 2006
Messages
6
Helped
1
Reputation
2
Reaction score
0
Trophy points
1,281
Activity points
1,322
In your spice file, just add this..

.OPTIONS
+itl4=100

This works.
 

Tiiu

Junior Member level 1
Joined
Jun 6, 2006
Messages
19
Helped
1
Reputation
2
Reaction score
0
Trophy points
1,281
Activity points
1,410
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

Top