SuperSpice and new component

Wed Mar 16, 2005 12:18 pm   

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?

Wed Mar 16, 2005 2:19 pm   

orangeKDS_at_mail.ru wrote:

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

(or should I use

No:-)


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


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.


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_at_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.

Thu Mar 17, 2005 1:23 pm   

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?

Thu Mar 17, 2005 2:22 pm   

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. Its a
'black box' with two wires and I don't wanna know more about it. My
problem is
calculating ONLY power supply of amps, so it should be really simple
to solve it.


yes, (but its not really an 'amp' to me, at least not now)

Thu Mar 17, 2005 2:42 pm   

orangeKDS_at_mail.ru wrote:

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_at_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.

Thu Mar 17, 2005 2:42 pm   

orangeKDS_at_mail.ru wrote:


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.


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


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_at_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.

Thu Mar 17, 2005 5:33 pm   

"Kevin Aylward" <salesEXTRACT_at_anasoft.co.uk> wrote in message
news:cgXZd.68825$Bk7.42294_at_fe1.news.blueyonder.co.uk...

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

Thu Mar 17, 2005 7:57 pm   

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..

Thu Mar 17, 2005 8:10 pm   

On 17 Mar 2005 11:57:56 -0800, orangeKDS_at_mail.ru wrote:


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 Voice:(480)460-2350 | |
| E-mail Address at Website Fax:(480)460-2142 | Brass Rat |
| http://www.analog-innovations.com | 1962 |

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

Thu Mar 17, 2005 8:51 pm   

<orangeKDS_at_mail.ru> schrieb im Newsbeitrag
news:1111089476.424423.76530_at_f14g2000cwb.googlegroups.com...


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

Fri Mar 18, 2005 7:49 am   

Genome wrote:

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_at_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.

Fri Mar 18, 2005 1:10 pm   

you said:


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.

Fri Mar 18, 2005 5:22 pm   

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

Sat Mar 19, 2005 7:58 am   

orangeKDS_at_mail.ru wrote:

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_at_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.

Sat Mar 19, 2005 4:58 pm   

orangeKDS,


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