(P)Spice / LT Spice param ? & high side firing circuit

[Active8]

Hi:

Two examples here. One in LT Spice and one in another CAD, I'm not
sure which.

Field Strength Meter.gif by analog

It uses a parameter called "Rser" for the meter inductor, V1, and
the batts. and "Cpar" and "Rpar" for L1 and L2.

I see those parameters are part of LT Spice's part properties.
Impressive. I bet that means that SS has those, too.

but then there's the

High side firing circuit.jpg from a disscussion under various
subject lines including "High side firing circuit".

It has a line "C1 = 0.014 ESR" which may be just text. If that's a
PSpice program then the braces are missing and there's no .param
line on the schem.

I can put a parameter in PSpice and/or a special part property for
ESR and stuff like that, but how do I get it to actually count? A
cap's a cap in PSpice AFAIK and I've been just adding coil
resistances and such as separate parts.

Is there a way to make a param like that count in PSpice, or do I
have to define a subcircuit for a symbol and pass the param to the
parasitic while dealing with whichever schem capture app I'm using?
Something tells me that's what really happens in LT Spice - a
subcircuit, but the param is called a symbol attribute or SYMATTR.

--
Best Regards,
Mike

 

[analog]

Active8 wrote:

uses a parameter called
"Rser" for the meter inductor, V1, and the batts and "Cpar" and
"Rpar" for L1 and L2.

These optional parameters enable the special model extensions for
these elements that LTspice has over standard plain vanilla spice.
The LTspice engine handles them using dedicated solver code in
multiple parallel threads such that the extra model elements do not
increase the size of the circuit matrix. This improves speed, not
only by minimizing matrix bloat, but also by avoiding many near
singularities that might otherwise throttle back step size.

Adding this capability to a switching power electronics simulator
was a pure stroke of genius on Mike Engelhardt's part. All the
parasitic elements important to accurate simulation of switch mode
power supplies can be included without cluttering up the schematic
(and are automatically included if one selects these components
from the convenient drop down menu to the extensive built-in
library of passives).

If you have LTspice, just refer to the help file sections detailing
inductors and capacitors - it (and lots more goodies) are all there.
_____________

"It is possible to specify an equivalent series resistance, series
inductances, parallel resistance and parallel shut capacitance."
--from the LTspice help file section on inductive circuit elements.

 

[Mike Engelhardt]

Mike,

...It uses a parameter called "Rser" for the meter inductor,
V1, and the batts. and "Cpar" and "Rpar" for L1 and L2.

I see those parameters are part of LT Spice's part properties.
Impressive. I bet that means that SS has those, too...

Unlikely. LTspice can solve, e.g, a series LCR circuit as
a single circuit element without internal nodes. It's a
method I originated. Whereas every other SPICE I know of
only has one integrator for integrating a reactance, LTspice
has about 17 different integrators for special cases of two
terminal linear networks. The technique improves solution
accuracy by solving some numerical difficulties and speeds
up the overall simulation speed.

--Mike

 

[Paul Burridge]

On Tue, 06 Jan 2004 05:31:03 GMT, analog <analog@ieee.org> wrote:

These optional parameters enable the special model extensions for
these elements that LTspice has over standard plain vanilla spice.
The LTspice engine handles them using dedicated solver code in
multiple parallel threads such that the extra model elements do not
increase the size of the circuit matrix. This improves speed, not
only by minimizing matrix bloat, but also by avoiding many near
singularities that might otherwise throttle back step size.

Adding this capability to a switching power electronics simulator
was a pure stroke of genius on Mike Engelhardt's part. All the
parasitic elements important to accurate simulation of switch mode
power supplies can be included without cluttering up the schematic
(and are automatically included if one selects these components
from the convenient drop down menu to the extensive built-in
library of passives).

Hi Analogue,

Thanks for the circuit you designed, BTW. I'm going to build it some
time this week - if you're happy with it as it stands on the last
revision, of course.
Just a couple of questions on the LT schematic. You've entered a
value of 50u for time delay. Is there any advantage in that? You've
also given the batteries one ohm of Rseries - is that really
necessary? And how did you arrive at the paracitic properties for L1
and L2?

thanks,

p

--

"I expect history will be kind to me, since I intend to write it."
- Winston Churchill

 

[Mike Engelhardt]

...It uses a parameter called "Rser" for the meter inductor,
V1, and the batts. and "Cpar" and "Rpar" for L1 and L2.

I see those parameters are part of LT Spice's part properties.
Impressive. I bet that means that SS has those, too...

Unlikely. LTspice can solve, e.g, a series LCR circuit as
a single circuit element without internal nodes. It's a
method I originated. Whereas every other SPICE I know of
only has one integrator for integrating a reactance, LTspice
has about 17 different integrators for special cases of two
terminal linear networks. The technique improves solution
accuracy by solving some numerical difficulties and speeds
up the overall simulation speed.

This question comes up often enough that I've prepared
a couple of trivial examples to demonstrate LTspice's
numerical improvement in accuracy over any other SPICE
due to its ability to solve an RC circuit as a single
intrinsic SPICE device with no internal nodes instead
of separate R's and C's. I introduced this method years
ago so that the circuit matrix would be better formulated
for short time steps in the interest of reducing
convergence problems in transient analysis. But the
problem can also be demonstrated in a .AC analysis and
it's easier to compare SPICE's there because there's no
timestep size that can be chosen differently between
SPICE's.

Here is an AC voltage divider circuit:

* Using LTspice's internally nodeless RC
C1 N001 A 10 Rser=1Meg
C2 A 0 10 Rser=1Meg
V1 N001 0 ac 2
..ac oct 100 10Meg 10G
..probe V([a])
..end

The voltage on A should be exactly 1V AC and it is
in LTspice. The circuit can not be simulated as
formulated in any other SPICE because no other SPICE
has an intrinsic SPICE device of a series RC.

Here's the same circuit, but using two components
for the R and C's. This version can be run in most
any standard SPICE. In PSpice, you will see that
node A can not always be solved for correctly:

* Using an internal node(N002 and N003) for RC components
R1 N001 N002 1Meg
C1 N002 A 10
R3 N002 A 1T
R2 A N003 1Meg
C2 N003 0 10
R4 N003 0 1T
V1 N001 0 ac 2
..ac oct 100 10Meg 10G
..probe V([a])
..end

LTspice also has the same trouble with this circuit
because of the formulation of the circuit matrix.
But, as a separate matter, the alternate solver of
LTspice reduces the problem by about 1000x because
it uses a sparse matrix solver that runs typically
1000 times more accurately than any other commercial
SPICE's.

These decks demonstrate two unique advantages of LTspice.
The integrated solvers for RC's improves the accuracy
and avoid certain convergence problems while increasing
simulation speed. The alternate solver uses a numerical
brute force method to run the simulation about 1000x more
accurately but at about half the simulation speed.

--Mike

 

[Active8]

On 06 Jan 2004 13:23:20 EST, pmte@concentric.net said...

...It uses a parameter called "Rser" for the meter inductor,
V1, and the batts. and "Cpar" and "Rpar" for L1 and L2.

I see those parameters are part of LT Spice's part properties.
Impressive. I bet that means that SS has those, too...

Unlikely. LTspice can solve, e.g, a series LCR circuit as
a single circuit element without internal nodes. It's a
method I originated. Whereas every other SPICE I know of
only has one integrator for integrating a reactance, LTspice
has about 17 different integrators for special cases of two
terminal linear networks. The technique improves solution
accuracy by solving some numerical difficulties and speeds
up the overall simulation speed.

Hi Mike, analog. Thanks, both.

Ok. Good feature.

Adding a property ESR to an SS or PSpice cap doesn't do a thing to
the net list.

--
Best Regards,
Mike

This question comes up often enough that I've prepared
a couple of trivial examples to demonstrate LTspice's
numerical improvement in accuracy over any other SPICE
due to its ability to solve an RC circuit as a single
intrinsic SPICE device with no internal nodes instead
of separate R's and C's. I introduced this method years
ago so that the circuit matrix would be better formulated
for short time steps in the interest of reducing
convergence problems in transient analysis. But the
problem can also be demonstrated in a .AC analysis and
it's easier to compare SPICE's there because there's no
timestep size that can be chosen differently between
SPICE's.

Here is an AC voltage divider circuit:

* Using LTspice's internally nodeless RC
C1 N001 A 10 Rser=1Meg
C2 A 0 10 Rser=1Meg
V1 N001 0 ac 2
.ac oct 100 10Meg 10G
.probe V([a])
.end

The voltage on A should be exactly 1V AC and it is
in LTspice. The circuit can not be simulated as
formulated in any other SPICE because no other SPICE
has an intrinsic SPICE device of a series RC.

Here's the same circuit, but using two components
for the R and C's. This version can be run in most
any standard SPICE. In PSpice, you will see that
node A can not always be solved for correctly:

* Using an internal node(N002 and N003) for RC components
R1 N001 N002 1Meg
C1 N002 A 10
R3 N002 A 1T
R2 A N003 1Meg
C2 N003 0 10
R4 N003 0 1T
V1 N001 0 ac 2
.ac oct 100 10Meg 10G
.probe V([a])
.end

LTspice also has the same trouble with this circuit
because of the formulation of the circuit matrix.
But, as a separate matter, the alternate solver of
LTspice reduces the problem by about 1000x because
it uses a sparse matrix solver that runs typically
1000 times more accurately than any other commercial
SPICE's.

These decks demonstrate two unique advantages of LTspice.
The integrated solvers for RC's improves the accuracy
and avoid certain convergence problems while increasing
simulation speed. The alternate solver uses a numerical
brute force method to run the simulation about 1000x more
accurately but at about half the simulation speed.

--Mike

 

[Jim Thompson]

On Wed, 07 Jan 2004 10:17:35 GMT, Active8
<mTHISREMOVEcolasono@earthlink.net,invalid> wrote:

On 06 Jan 2004 13:23:20 EST, pmte@concentric.net said...
...It uses a parameter called "Rser" for the meter inductor,
V1, and the batts. and "Cpar" and "Rpar" for L1 and L2.

I see those parameters are part of LT Spice's part properties.
Impressive. I bet that means that SS has those, too...

Unlikely. LTspice can solve, e.g, a series LCR circuit as
a single circuit element without internal nodes. It's a
method I originated. Whereas every other SPICE I know of
only has one integrator for integrating a reactance, LTspice
has about 17 different integrators for special cases of two
terminal linear networks. The technique improves solution
accuracy by solving some numerical difficulties and speeds
up the overall simulation speed.

Hi Mike, analog. Thanks, both.

Ok. Good feature.

Adding a property ESR to an SS or PSpice cap doesn't do a thing to
the net list.

If it ain't mentioned in the resultant subcircuit, it ain't a
"property". You need to edit the template.

...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.

 

[Jim Thompson]

On 07 Jan 2004 11:34:24 EST, "Mike Engelhardt" <pmte@concentric.net>
wrote:

Jim,

Adding a property ESR to an SS or PSpice cap doesn't do
a thing to the net list.

If it ain't mentioned in the resultant subcircuit, it ain't a
"property". You need to edit the template.

But real problem is that you *have* to use a subcircuit for
an RC circuit in PSpice. LTspice does not and that improves
the accuracy, robustness, and simulation speed.

--Mike

Don't you end up with too many "special cases/parts"?

What you really have is an RC part/device-model.

...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]

Jim,

Adding a property ESR to an SS or PSpice cap doesn't do
a thing to the net list.

If it ain't mentioned in the resultant subcircuit, it ain't a
"property". You need to edit the template.

But real problem is that you *have* to use a subcircuit for
an RC circuit in PSpice. LTspice does not and that improves
the accuracy, robustness, and simulation speed.

--Mike

 

[Mike Engelhardt]

Jim,

Adding a property ESR to an SS or PSpice cap doesn't do
a thing to the net list.

If it ain't mentioned in the resultant subcircuit, it ain't a
"property". You need to edit the template.

But real problem is that you *have* to use a subcircuit for
an RC circuit in PSpice. LTspice does not and that improves
the accuracy, robustness, and simulation speed.

Don't you end up with too many "special cases/parts"?

What you really have is an RC part/device-model.

There's presently 18 special cases of linear, two-terminal
reactances that handled internally by their own integrator in
LTspice(in contrast to all other SPICE's which use a single
integrator multiple times for everything and then have more
nodes, less accuracy, less solver robosity and run slower).

All these devices are special cases of L's and C's. You just
specify the parasitics and LTspice picks the right integrator
for the job. About the only tricky thing is that if you
want to simulate a Xtal with one of these integrators, you would
use a symbol that actually netlists as a capacitor with the Xtal's
series resonance capacitance being the C device's capacitance,
and the parallel resonant's capacitance being the device's Cpar.
There's an example circuit, Pierce.asc, that shows this technique
in the directory examples/Educational.

Otherwise it's pretty straightforward and just takes care of
itself. It's really not that complicated and described in
the help documentation.

--Mike