How to fix "timestep too small" error in hspice si

internal timestep too small in transient analysis

Anyone know which options will help to solve this problem?

timestep too small

What exactly are you doing? What does your forcefile look like?

internal timestep too small

Hughes said:

Anyone know which options will help to solve this problem?

Click to expand...

relv=2 ...
or change the voltage or temperature in minor

hspice internal timestep too small

If i am not mistaken, what it means is the timestep specified in the spice simulation file is too small.

Example (for transient analysis):

.tran 0.01ns 360ns

The "0.01ns" is your timestep to run the transient analysis till 360ns. Perhaps you should increase it to 0.1ns.

spice timestep too small

Thanks all.
My problem should be "internal timestep too small".
Transient analysis timestep has little effect to this problem.
Simetimes I made a small change to the circuit and the problem dispeared. But when circuits arelarge, it is hard to find a solution by this way. So I want to know which spice options will help to solve this problem.

I will try kfy's solution next time I encounter this problem. Thank you.

time step too small

I also meet this problem in orcad (pspice).
After increase the default convergence times (maybe K4 in orcad9) from 10 too 200, many Transient analysis can run but the speed is slow.

timestep too small spice

"timestep too small"-- Transient Convergence Problem:

Solution:
0. Check circuit topology and connectivity.
This item is the same as item 0 in the DC analysis.

1. Set RELTOL=.01 in the .OPTIONS statement.
Example: .OPTIONS RELTOL=.01

2. Reduce the accuracy of ABSTOL/VNTOL if current/voltage levels allow it.
Example: . OPTION ABSTOL=1N VNTOL=1M

3. Set ITL4=500 in the .OPTIONS statement.
Example: .OPTIONS ITL4=500

4. Realistically Model Your Circuit; add parasitics, especially stray/junction capacitance.

5. Reduce the rise/fall times of the PULSE sources.
Example: VCC 1 0 PULSE 0 1 0 0 0
becomes VCC 1 0 PULSE 0 1 0 1U 1U

6. Use the .OPTIONS RAMPTIME=xxx statement to ramp up all of the sources.
Example: .OPTIONS RAMPTIME=10NS

7. Add UIC (Use Initial Conditions) to the .TRAN line.
Example: .TRAN .1N 100N UIC

8. Change the integration method to Gear (See also Special Cases below).
Example: .OPTIONS METHOD=GEAR


Regards,

tran timestep too small

to solve convergence problems

hspice timestep too small

Internal timestamp too small is usually due to the fact that hspice cannot find the derivative of a waveform. (Usuallly means that the derivative is inifinity) Hspice calculates (I think) the running derivative of the signal and adjusts the timestep accordingly. If it cannot find the derivative, it barfs. I have found that taking the time to check the initialization of all nodes usually helps.

Just a thought,

altium timestep too small

crystal said:

If i am not mistaken, what it means is the timestep specified in the spice simulation file is too small.

Example (for transient analysis):

.tran 0.01ns 360ns
*the "0.01ns" is not your timestep to run the transient analysis, it is print step
The "0.01ns" is your timestep to run the transient analysis till 360ns. Perhaps you should increase it to 0.1ns.

Click to expand...

spice time step too small

Hi, rambus_ddr. I don't know what you mean by quoting crystal's input. But internal timestep is definitely not the same as the step in transient analysis statement. The latter is just a step for output. I think rambus_ddr and srik's solution is very helpful.

hspice internal timestep too small#

ITL4 is limited to 100 now in the new versions of HSPICE.

OkGuy

timestamp too small

The timestep used by HPSPICE when making a transient simulation is changed dynamically, i.e., HSPICE always tries to find the maximum timestep that still guarantees a given precision. Several different algorithms can be selected to determine the timestep to use - for details refer to HSPICE manual.

The timestep specified in the .tran line (TSTEP) serves two main purposes:
1. Print step (used by .print statements)
2. Helps to define that MAXIMUM and MINIMUM internal timestep used in the simulation.

The "internal timestep too small" error happens when HSPICE tries to use an internal timestep bellow a certain threshold. This threshold is given by:
MIN TIMESTEP=TSTEP*RMIN
where RMIN is an option that can be set by the user (default=1e-9).

For example if one specifies
.tran 0.01ns 360ns

we have TSTEP=0.01ns and the default internal timestep is 0.01ns*1e-9=1e-20 s

So, one solution to the problem is to specify a smaller RMIN (I think that the minimum value is 1e-15...). This solved the problem most of the times I faced it.

If you still have this problem you can try to play with the others parameters that control the internal timestep (see the manual).

Regards

"timestep too small"-- Transient Convergence Problem:

I have done all of the above advices, but it did not work.
Now, I try to use ".options accurate=1 gmin=1e-9" and it's work well.

Two main things.

One, every active device must have realistic capacitances between
all nodes. Too low a capacitance lets voltage swing crazy with a
tiny charge error.

Two, every device must be well behaved at abnormal terminal
bias conditions. There can be no singularities (BSIMSOI is very
bad about this) anywhere and no blowups when you take a
pin voltage well outside normal range. Modeling dudes don't
have data for that and don't check it. But by 1kV pin-pin
or 1kA forced current you had better still look like a
finte valued resistor. When 1kV gets you 1MA by some
bullschnitzel square law approximation you are in trouble
anytime the numerical algorithm steps off into the weeds.
You need the device to be solvable over a much, much
wider range than you will ever use it.

If tweaking settings doesn't work that's a pretty good
sign that it isn't a settings problem. Sacrificing accuracy
to get convergence means your model is numerically
bad (accuracy aside). And some models depend on the
alignment of a lot of parameters to "cover up" some
fundamental singularities (like where region of operation
and equations transition). When you get to Monte Carlo
and start random-messing parameters around you can
expose "unexplored territory".

hiii shiowjyh

can u plz tell some more information regarding transient convergence problems?? how to overcome those??

Hello all,

"time step specified too small"

I have been getting this error even when I tried all your above mentioned comments.
The interesting point about my circuit is I didn't mention any timestep or timestop for my transient analysis.
I am doing optimization and so I wrote the command based on the information in this link:

**broken link removed**

So my netlist includes this line:

.Tran Data=frq Sweep optimize=opt1 results=comp1 model=optmodel

What do you think?

Thanks in advance
Analogstudent