SuperSpice and new component

[Kevin Aylward]

orangeKDS@mail.ru wrote:

I need to analyse VERY simple circuit with SuperSpice

You can always email me direct. Support is all free.

(or should I use

some other program?).

No

Schematics has some resistors and 'special type'
of (coax)amplifiers. All that I know about those amplifiers is that
their U*I=22,5Watt, but that should be all that I need.

This don't seem to mean much. Amps have all sorts of specs, like gain,
bandwidth, noise, slew rate etc.

It is
connected to power supply =63V DC.
I want to know the (DC)current that those amplifiers are using and
their voltage.

How do I add that type of amplifiers to SuperSpice component database?

I presume you mean the specific amp model which is a ".subckt".
".subckt" models are placed in library text files, usually with the
extension .lib. You need to find out what the amp model is.

Adding a file with models is just a matter of drag-dropping the file
from windows explorer to the SS main window. You aslo ope existing files
and past in the model text

When you try and place the ".subckt" it will want to be attached to a
symbol. The GUI will guide you through selecting an existing symbol, or
you can create a block symbol automatically, or draw one from scratch
using the symbol editor.

I do not need any complex analysis, just DC voltages and currents. I
have used Derive for (numerical) solving system of nonlinear
equations, but SuperSpice should be easier for modifying
schematics..etc?

Yes it is. However, I need more specific info though to sort out your
problem. Your amp spec is pretty much meaningless.

Kevin Aylward
salesEXTRACT@anasoft.co.uk
http://www.anasoft.co.uk
SuperSpice, a very affordable Mixed-Mode
Windows Simulator with Schematic Capture,
Waveform Display, FFT's and Filter Design.

 

I need to analyse VERY simple circuit with SuperSpice (or should I use
some other program?). Schematics has some resistors and 'special type'
of (coax)amplifiers. All that I know about those amplifiers is that
their U*I=22,5Watt, but that should be all that I need. It is connected
to power supply =63V DC.
I want to know the (DC)current that those amplifiers are using and
their voltage.

How do I add that type of amplifiers to SuperSpice component database?

I do not need any complex analysis, just DC voltages and currents. I
have used Derive for (numerical) solving system of nonlinear equations,
but SuperSpice should be easier for modifying schematics..etc?

 

you once said:

'To construct a non-linear resistor, one can set up a voltage dependent
current source as a non-linear function of its own terminal voltage.
I've never tried it, but believe a behavioral source's describing
function can include frequency. But even if you could, why would you
wish to model a non realizable component?'


What I need is to 'construct' a nonlinear resistor that has: I=P/U
(P=const.=22.5Watt)

how do I do it?

 

[Kevin Aylward]

orangeKDS@mail.ru wrote:

you once said:

'To construct a non-linear resistor, one can set up a voltage
dependent current source as a non-linear function of its own terminal
voltage. I've never tried it, but believe a behavioral source's
describing function can include frequency. But even if you could,
why would you wish to model a non realizable component?'


What I need is to 'construct' a nonlinear resistor that has: I=P/U
(P=const.=22.5Watt)

how do I do it?

Until you tell us what "U" is, we don't know. Do you want to confirm it
might be "V", for voltage?

Kevin Aylward
informationEXTRACT@anasoft.co.uk
http://www.anasoft.co.uk
SuperSpice, a very affordable Mixed-Mode
Windows Simulator with Schematic Capture,
Waveform Display, FFT's and Filter Design.

 

[Kevin Aylward]

orangeKDS@mail.ru wrote:

Schematics has some resistors and 'special type'
of (coax)amplifiers. All that I know about those amplifiers is that
their U*I=22,5Watt, but that should be all that I need.

This don't seem to mean much. Amps have all sorts of specs, like
gain, bandwidth, noise, slew rate etc.

but I really don't need all that. When I try to solve it manually, I
write down Kirchhoffs rules and equations for componenets, use math
program for numerical solving of system and thats ALL.
I just want program to make it easier for me when for eg. removing one
resistor.
To me, (coax) amplifier is a 'strange' resistor with U=22/I.

An amplifier is not a resister. The problem here, is that you are
essentially, talking gibberish. "U" means nothing, other then as a
referance desigater.

Its a
'black box' with two wires and I don't wanna know more about it.

But *we* need to know what your talking about to help you. You are using
notation that means, essentially, nothing in electronics.

problem is
calculating ONLY power supply of amps, so it should be really simple
to solve it.

Probably is, if you can tell us what you are actualy trying to do.

Do you mean somting to do with

V=IR

or V=P/I

Until you formulate you problem correctly, or explain in more detail
what you are trying to do so we can formulate it for you, no one can
help you.


Kevin Aylward
informationEXTRACT@anasoft.co.uk
http://www.anasoft.co.uk
SuperSpice, a very affordable Mixed-Mode
Windows Simulator with Schematic Capture,
Waveform Display, FFT's and Filter Design.

 

[Genome]

"Kevin Aylward" <salesEXTRACT@anasoft.co.uk> wrote in message
news:cgXZd.68825$Bk7.42294@fe1.news.blueyonder.co.uk...

orangeKDS@mail.ru wrote:

Oi, I happened to be in my registry today. I had a look at your software
once and then uninstalled it. What's that anasoft/superspice crap doing in
my registry?

DNA

 

of course it means the same as V.. I've been using symbol U as voltage
for years in school.. so I thought everyone else used it too, my
mistake., sorry

The 'amplifier' has constant power: V*I=22.5Watt, that is it, nothing
more..

I have been trying to use your users guide and part that describes:
3.2.3. Non-linear Dependent Sources
but as you can see I'm a total newbie and need help badly..

 

[Jim Thompson]

On 17 Mar 2005 11:57:56 -0800, orangeKDS@mail.ru wrote:

of course it means the same as V.. I've been using symbol U as voltage
for years in school.. so I thought everyone else used it too, my
mistake., sorry

The 'amplifier' has constant power: V*I=22.5Watt, that is it, nothing
more..

I have been trying to use your users guide and part that describes:
3.2.3. Non-linear Dependent Sources
but as you can see I'm a total newbie and need help badly..

Just use a G source (behavioral), where G = W/V (W=22.5)

I don't know SuperSpice, but that expression _might_ cause convergence
issues. If so try:

G = W/(abs(V)+0.001)

to avoid a divide by zero.

...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.

 

[Helmut Sennewald]

<orangeKDS@mail.ru> schrieb im Newsbeitrag
news:1111089476.424423.76530@f14g2000cwb.googlegroups.com...

of course it means the same as V.. I've been using symbol U as voltage
for years in school.. so I thought everyone else used it too, my
mistake., sorry

The 'amplifier' has constant power: V*I=22.5Watt, that is it, nothing
more..

I have been trying to use your users guide and part that describes:
3.2.3. Non-linear Dependent Sources
but as you can see I'm a total newbie and need help badly..

Hello orange,
this is an example how you would write it in a netlist.
B1 is a behaviorial current source. The current is
I = const/actual_voltage .

B1 a 0 I=22.5/V(a)

What you see above is SPICE instruction line.
It can be also the result of a schematic containing a B-source.
I have attached a schematic file from another SPICE program.
It's LTspice. This example sweeps the voltage from 20V to 60V.
You can download LTspice with this link.
http://ltspice.linear.com/software/swcadiii.exe

There are many other SPICE programs around, but not all have
behavioral sources.

Best Regards,
Helmut



This is the schematic file "test.asc".

Version 4
SHEET 1 880 680
WIRE 32 208 32 160
WIRE 32 336 32 288
WIRE 32 368 32 336
WIRE 208 160 32 160
WIRE 208 208 208 160
WIRE 208 336 32 336
WIRE 208 336 208 288
FLAG 32 368 0
FLAG 208 160 a
SYMBOL voltage 32 192 R0
SYMATTR InstName V1
SYMATTR Value 63
SYMBOL bi 208 208 R0
SYMATTR InstName B1
SYMATTR Value I=22.5/V(a)
TEXT 32 80 Left 0 !.dc V1 20 100 1
TEXT 40 24 Left 0 ;I = P / V

 

[Kevin Aylward]

Genome wrote:

"Kevin Aylward" <salesEXTRACT@anasoft.co.uk> wrote in message
news:cgXZd.68825$Bk7.42294@fe1.news.blueyonder.co.uk...
orangeKDS@mail.ru wrote:

Oi, I happened to be in my registry today. I had a look at your
software once and then uninstalled it. What's that anasoft/superspice
crap doing in my registry?

Well, it just stays there. It don't do anything. Its completely passive.
You can just delete the whole lot if you want. I did have a go once at
improving the delete on uninstall, but it got to be a bit of pain with
the install/uninstall program I use.

Kevin Aylward
informationEXTRACT@anasoft.co.uk
http://www.anasoft.co.uk
SuperSpice, a very affordable Mixed-Mode
Windows Simulator with Schematic Capture,
Waveform Display, FFT's and Filter Design.

 

you said:

Hello orange,
this is an example how you would write it in a netlist.
B1 is a behaviorial current source. The current is
I = const/actual_voltage .

B1 a 0 I=22.5/V(a)

What you see above is SPICE instruction line.
yes, that is what i need, but how to do it in super spice?

I have tried modifying 'functional' component named COS_XN like this:

..SUBCKT COS_XN _ssi_pin0 1
* _SS_Symbol [C:\Program
Files\AnaSoft\SuperSpice\system\SchematicBlocks.ssm] [2PinBlock]
B1 _ssi_pin0 1 I=22/(V(_ssi_pin0,1))
..ENDS

but it doesn't work. Please tell me how to make it work.


BTW, does ltspice have nice and greatlooking GUI like superspice? Can I
easily draw schematics in it? I don't wanna type in node numbers and
elements like in old spice, ever.

 

it works!! )
where do I set how many digits of precision is needed?

 

[Kevin Aylward]

orangeKDS@mail.ru wrote:

it works!! )
where do I set how many digits of precision is needed?

Not sure what you mean by this. The calculation itself always uses the
full range that the compiler supports, which is something like 12 digits
of accuracy. This never need setting. You can change the number of
digits displayed by clicking on the graph and going to the Options/misc
tab. The default is usually quite adequate.

Kevin Aylward
informationEXTRACT@anasoft.co.uk
http://www.anasoft.co.uk
SuperSpice, a very affordable Mixed-Mode
Windows Simulator with Schematic Capture,
Waveform Display, FFT's and Filter Design.

 

[Mike Engelhardt]

orangeKDS,

Can I easily draw schematics in
it? I don't wanna type in node numbers and elements
like in old spice, ever.

LTspice had integrated schematic capture. It also lets
you add SPICE directives on the schematic and has dialog
boxes that let you mix and match editing the SPICE
syntax in text or checking boxes on a dialog box. You
might want to check it out. More full licenses of
LTspice are distribed per day than, say, PSpice/Schematic/
Orcad does in a year.

--Mike

 

[Jim Thompson]

On Sat, 19 Mar 2005 16:58:47 GMT, "Mike Engelhardt" <nospam@spam.org>
wrote:

orangeKDS,

BTW, does ltspice [...]Can I easily draw schematics in
it? I don't wanna type in node numbers and elements
like in old spice, ever.

LTspice had integrated schematic capture. It also lets
you add SPICE directives on the schematic and has dialog
boxes that let you mix and match editing the SPICE
syntax in text or checking boxes on a dialog box. You
might want to check it out. More full licenses of
LTspice are distribed per day than, say, PSpice/Schematic/
Orcad does in a year.

--Mike

And Wimpows has even more licenses than 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]

Jim,

More full licenses of LTspice are distributed per day than,
say, PSpice/Schematic/ Orcad does in a year.

And Wimpows has even more licenses than LTSpice ;-)

Wrong-Horse-Thompson -- stuck in the wrong simulator
saddle again!

--Mike

 

[Jim Thompson]

On Sat, 19 Mar 2005 17:26:39 GMT, "Mike Engelhardt"
<nospam@nospam.org> wrote:

Jim,

More full licenses of LTspice are distributed per day than,
say, PSpice/Schematic/ Orcad does in a year.

And Wimpows has even more licenses than LTSpice ;-)

Wrong-Horse-Thompson -- stuck in the wrong simulator
saddle again!

--Mike

Could be.

However one of my clients tried LTSpice on a *complex* BiCMOS circuit
and got spurious results, not matching actual performance like PSpice
did.

I suspect that your speed-up algorithms, just ducky for SMPS, can skip
over important stuff in other types of circuits.

...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,

More full licenses of LTspice are distributed per day than,
say, PSpice/Schematic/ Orcad does in a year.

And Wimpows has even more licenses than LTSpice ;-)

Wrong-Horse-Thompson -- stuck in the wrong simulator
saddle again!

Could be.

However one of my clients tried LTSpice on a *complex* BiCMOS
circuit and got spurious results, not matching actual
performance like PSpice did.

I suspect that your speed-up algorithms, just ducky for SMPS,
can skip over important stuff in other types of circuits.

Nothing that speeds up the SMPS stuff would corrupt
the BiCMOS results. The SMPS stuff doesn't impact the
SPICE stuff, its a library of ABM, special devices,
and HDL's w/ some VerilogA-type extensions. Anyway,
people upgrade routinely from PSpice and hspice to
LTspice for it's speed, *accuracy*, and convergence
specifically in BiCMOS full-chip simulation. LTspice
was first a IC simulation tool and second a SMPS
tool. BTW, it now has a new data file format called
Fast Access that allows you to load waveforms from
full chip sims extremely fast, i.e., if you have a
5G file with 2K data traces the load time for a new
trace drops from 5min to 1sec with not one bit loss
of accuracy.

I'd have to see the circuit to tell what happened.
Please feel free to send the files I need to duplicate
the problem and I can tell you what the problem was.
Just to rub it in, last time you sent me a nelist,
LTspice gave the correct result and PSpice gave the
wrong one because it isn't as accurate at integrating
differential equations.

The most effective thing for me would be if you
first make sure you're using the current version(2.13x)
and see if the problem occurs both in the Normal
and Alternate solver(Tools=>Control Panel=>SPICE=>
Solver)

Regards,

--Mike

 

[Jim Thompson]

On Sat, 19 Mar 2005 18:11:13 GMT, "Mike Engelhardt"
<nospam@nospam.org> wrote:

Jim,
[snip]

I'd have to see the circuit to tell what happened.
Please feel free to send the files I need to duplicate
the problem and I can tell you what the problem was.
Just to rub it in, last time you sent me a nelist,
LTspice gave the correct result and PSpice gave the
wrong one because it isn't as accurate at integrating
differential equations.

The most effective thing for me would be if you
first make sure you're using the current version(2.13x)
and see if the problem occurs both in the Normal
and Alternate solver(Tools=>Control Panel=>SPICE=
Solver)

Regards,

--Mike

qrk/Mark, Could you send Mike the circuit? I don't recall now what
was involved.

...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.

 

[ldg]

On Sat, 19 Mar 2005 16:58:47 GMT, "Mike Engelhardt" <nospam@spam.org>
wrote:

More full licenses of
LTspice are distribed per day than, say, PSpice/Schematic/
Orcad does in a year.

And more are deleted

Actually, LTspice seems to be getting slightly better, but is a board
level simulator. If that's you're purpose, then fine. If you're
doing IC's, it will soon disappoint.

It still doesn't seem to be able to handle simple hspice models for
resistors and capacitors. (specified by w/l). These are simple
things, but not needed for board level work.

I haven't tried using a multiplier ( m=) for bipolars, but this didn't
seem to work when I tried it a while back in a bandgap. A multiplier
isn't in the LTspice documentation for bipolars, so it's really not
there anyway. Again, if you're not doing a lot of device level work
using bipolars, this isn't too much of a problem. There are many
things like this you run into when trying to use LTspice for IC's.

So LTspice is a board level simulator with nice graphics. There are
many undocumented features in LTspice that people have reverse
engineered, but a user shouldn't have to do that.

I looked at Simetrix recently and they can't do m= (mutipliers) on
capacitors, so LTspice has them beat there. They have a native linux
version though and that sure is tempting.

Both LTspice and Simetrix run well on my AMD 64 box under SuSE9.2.

Ltspice really does run well under wine. I was impressed. I didn't
do benchmarks, so have no way of knowing at this point how the extra
overhead might affect a long simulation. What impressed me most I
think was the ease with which this software loaded and ran. As a new
linux administrator (used unix for years), I've struggled with getting
other software to run. Loading LTspice was a joy in comparison. 64
bits? No problem.

I tried recently to get ECS/Synario/Cohesion/Lakers_AMS schematic
capture to run under SuSE9.2. It's libraries are dependent on Redhat
V3 and gets glibc errors under SuSE.

Smartspice won't even let you try their software if you tell them you
have anything besides Redhat V3. They don't support anything else.
End of story. They're nice about it though

Looks like I chose the wrong distro for my linux box. I'm going to
have to switch over to Redhat since that's what the engineering
software companies seem to have standardized on. From what I
understand the different distros use the same libraries, but have
arranged them differently? If true it makes one wonder if the word
duh means anything to these folks. Then again, why is it some vendors
seem to be able to write distro independent software for linux and
while others can't?

Regards,
Larry