Ltspice: .Savebias equivalent?

[ldg]

Hi all,

I've been looking for a way to save a dc bias point file at various
times during a transient simulation with LTspice. Does it exist?

I not only use this for .ic conditions, saving time on later runs, but
I use the node list to create a file to limit the number of nodes I
save.

I found that the .save function is similar to the .probe function in
smartspice. It needs a list though which could be time consuming to
type - hence the desire for an automated way to create the file.

Regards,
Larry

 

[Mike Engelhardt]

Larry,

I've been looking for a way to save a dc bias point file at
various times during a transient simulation with LTspice.
Does it exist?

No, but it's on the ToDo list.

--Mike

 

[ldg]

On 14 Oct 2003 15:16:47 GMT, "Mike Engelhardt" <pmte@concentric.net>
wrote:

Larry,

I've been looking for a way to save a dc bias point file at
various times during a transient simulation with LTspice.
Does it exist?

No, but it's on the ToDo list.

--Mike

Great! This is pretty important actually. For instance, I'm running
a full chip similation right now and the first sim basically brings up
the supplies and so forth to steady state. This will take about a
day. At that point I'd like to do a few sims with different inputs
and so forth - without going through the startup sequence again. I
can't do this without a way of saving the dc condition at the end of
the run, then using this as a .ic in the next runs.

I also have a question about the "steady state" usage in the transient
statement. Is this intended for, say finding the dc condition of a dc
circuit, or will it actually try to find a steady state of a circuit
with multiple clocks and so forth? I'm not sure how it would know the
length of a clock pattern to find steady state in a digital circuit.

Of course, you can't save the dc condition at the end of the run
anyway, so there's no way to use the info on later runs right now
anyway.

My next useful feature would be to play some sort of a wav file at the
end of a run. I don't know how much time I waste on long sims when
the computer finishes and I don't notice it for an hour. Even a
toaster noise would be ok.

Regards,
Larry

 

[Jim Thompson]

On Mon, 13 Oct 2003 21:41:17 -0700, ldg <lgipson@ix.netcom.com> wrote:

Hi all,

I've been looking for a way to save a dc bias point file at various
times during a transient simulation with LTspice. Does it exist?

I not only use this for .ic conditions, saving time on later runs, but
I use the node list to create a file to limit the number of nodes I
save.

I found that the .save function is similar to the .probe function in
smartspice. It needs a list though which could be time consuming to
type - hence the desire for an automated way to create the file.

Regards,
Larry

Since you mention .SAVEBIAS you know it can be done in PSpice, but NOT
in LTSpice ;-)

...Jim Thompson
--
| James E.Thompson, P.E. | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC's and Discrete Systems | manus |
| Phoenix, Arizona Voice480)460-2350 | |
| E-mail Address at Website Fax480)460-2142 | Brass Rat |
| http://www.analog-innovations.com | 1962 |

I love to cook with wine. Sometimes I even put it in the food.

 

[Mike Engelhardt]

Larry,

I've been looking for a way to save a dc bias point file
at various times during a transient simulation with
LTspice. Does it exist?

No, but it's on the ToDo list.

Great! This is pretty important actually. For instance, I'm
running a full chip similation right now and the first sim
basically brings up the supplies and so forth to steady state.
This will take about a day.

Yes, it has internal uses also. That being sadi, a day seems like
a very long time for LTspice to find the .op point of even a 10,000
transistor level full chip sim. You might want to make sure you
go right to the correct solution strategy, i.e., noopiter or
gminsteps=0. The .log file will mention if direct Newton
iteration failed(then you can add ".options noopiter" to skip it
next time.) Or if gmin stepping failed(then add ".options
gmin steps=0" to skip that.

I also have a question about the "steady state" usage in the
transient statement. Is this intended for, say finding the
dc condition of a dc circuit, or will it actually try to find
a steady state of a circuit with multiple clocks and so forth?
I'm not sure how it would know the length of a clock pattern to
find steady state in a digital circuit.

The "steady state" option is only of use with the SMPS models
written in LTspice's native HDL. Usually the steady state
condition looks for zero current out of the error amp's
transconductance as averaged over a clock cycle for 10 cycles.
The models specify an edge to use as the the start of clock
cycle, also specify the compliance range of the error amp, and
define a function that specifies what load the error amp had to
drive/bias that should be ignored in this output current. It's of
no use for general SPICE simulations.

My next useful feature would be to play some sort of a wav
file at the end of a run. I don't know how much time I waste
on long sims when the computer finishes and I don't notice it
for an hour. Even a toaster noise would be ok.

The marching waveforms are a pretty good indication of completion
status, but I suppose you could run it from a .bat file:

scad3.exe -b deck.cir
(some command that makes sound)

Notice that if you run it interactively, it will ask you which
waves to plot. That dialog will time out after 5min, but you
can defeat this by saving a valid .plt settings file for the
simulation or by running in batch mode.

--Mike

 

[Mike Engelhardt]

Jim,

I've been looking for a way to save a dc bias point file at various
times during a transient simulation with LTspice. Does it exist?

I not only use this for .ic conditions, saving time on later runs, but
I use the node list to create a file to limit the number of nodes I
save.

I found that the .save function is similar to the .probe function in
smartspice. It needs a list though which could be time consuming to
type - hence the desire for an automated way to create the file.

Regards,
Larry

Since you mention .SAVEBIAS you know it can be done in PSpice, but NOT
in LTSpice ;-)

That's because he's already upgraded to LTspice from PSpice and/or
smartspice.

--Mike

 

[ldg]

On 14 Oct 2003 21:42:39 GMT, "Mike Engelhardt" <pmte@concentric.net>
wrote:

Larry,

I've been looking for a way to save a dc bias point file
at various times during a transient simulation with
LTspice. Does it exist?

No, but it's on the ToDo list.

Great! This is pretty important actually. For instance, I'm
running a full chip similation right now and the first sim
basically brings up the supplies and so forth to steady state.
This will take about a day.

Yes, it has internal uses also. That being sadi, a day seems like
a very long time for LTspice to find the .op point of even a 10,000
transistor level full chip sim. You might want to make sure you
go right to the correct solution strategy, i.e., noopiter or
gminsteps=0. The .log file will mention if direct Newton
iteration failed(then you can add ".options noopiter" to skip it
next time.) Or if gmin stepping failed(then add ".options
gmin steps=0" to skip that.

Well, it would be very nice to reduce the startup time, but
unfortunately there are some long time constants and switching
circuits that have no dc steady state. So I'm using UIC on the end of
my transient statement and guessing a few node voltages in a .ic
statement.

There are also analog and digital one-shots in a sort of Rube Goldberg
configuration that reset this and that on the die at startup (Legacy
stuff.) I have to sim past these things to get to steady state.

I actually started this sim yesterday. It's almost to 200us right now
and things have mostly settled. There's just nothing I can do with it
from here in the way of future sims. The raw file is 23 gigs.

This sim is a little over the top in that there are actually 2 full
die being simulated in a master-slave configuration. There will be 2
micro machine accelerometers that will attach to the die. I just
added the master-slave circuits and wanted to see them work the way
they will be used. I've already tested them with smaller sims.

Regards,
Larry

 

[ldg]

On Tue, 14 Oct 2003 13:39:51 -0700, Jim Thompson
<invalid@invalid.invalid> wrote:

Since you mention .SAVEBIAS you know it can be done in PSpice, but NOT
in LTSpice ;-)

Sad but true.

If I had pspice I'd probably use it once in a while. I have other
simulators here and find reason to use them for various things now and
again. I have nothing against pspice other than I don't own it.

I'd really like to try converting one of my boxes to linux, but hspice
and smartspice are unrealistically $$high for consultants in anything
but win2k. I've thought about Dolphin's Smash since they're
compatible with the CohesionTools schematic capture I use, but they
prefer Bill Gates to Torvolds also.

On the other hand, Mike's effort will let me run spice on any computer
I buy for a very reasonable price. It's hard to beat. I recently
ran corners on a design with LTspice using 4 machines on my lan at
once. I would have to have had four $15k software licenses to do this
with commercial products.

All he needs to do is continue listening to users like he has been and
pretty soon he'll have the corner on spice based simulators. He's
adressing my one largest complaints about simulator developers - the
guys that write the code don't use it.

Very impressive.

Regards,
Larry

 

[Mike Engelhardt]

Larry,

I've been looking for a way to save a dc bias point file
at various times during a transient simulation with LTspice.
Does it exist?

No, but it's on the ToDo list.

Great! This is pretty important actually. For instance, I'm
running a full chip simulation right now and the first sim
basically brings up the supplies and so forth to steady state.
This will take about a day. At that point I'd like to do a few
sims with different inputs and so forth - without going through
the startup sequence again. I can't do this without a way of
saving the dc condition at the end of the run, then using this
as a .ic in the next runs.

OK, released in version 2.06r, available now. The syntax is
similar to PSpice's .savebias's. That is:

..savebias "filename" time=10m
..savebias "anothername" time=55m

You can add the keyword "internal" if you also want device
internal nodes dumped to the file. The keyword "nosub"
will suppress subcircuit node and inductor currents from
being written to the file. Also, you can stipulate a step
number, temperature, or analysis type if you want to limit
the scope of the .savebias statement.

To use it for subsequent simulations, comment out the .savebias
statements referring to files you don't want overwritten and
add the command

..loadbias "filename"

The file is an ASCII file containing a .nodeset statement.
Nodesets are suggestions for the initial operating point to help
in finding the .op point. You can edit this .nodeset to a .ic
statement to be more assertive for the .tran initial condition.
..ic statements are conditions, not suggestions.

--Mike