Forums

SPICE help, please

Started by Robert Baer December 17, 2011
   OK, the below listing is accepted by TopSpice (a DOS version) as well 
as LTspice (if the .OPTION card is commented out.
   LTspice takes a while to give a "result" (no curves in plot pane).
   I do not see how one can do an X.. in LTspice so i reverted to TopSpice.

Q#1: How do i get this to work either version)?
Q#2: How could one do this in "plain" LTspice?

CODATRON EMULATION IN TESTING ARRAY
* Codatron (TM) TRADEMARKED BY Oil 4 LESS LLC
.OPTION LIMPTS=1000000 PIVTOL=1D-20 ;LTspice DOES NOT ACCEPT LIMPTS..
.TEMP 25
.dc I1 -200u 200u 0.001u
; Matrix of Codatron "load" resistors first
; 5x5 ARRAY initially ; NO LTSPICE CURVES..??
; TopSpice (dos version) complains no .PRINT output data,
;  maximum entry at step 6 (5D-5) is less than PIVTOL with .OPTION card
RV01 0 101 10E20
RV02 0 102 10E20
RV03 0 103 10E20
RV04 0 104 10E20
RV05 0 105 10E20

RH01 0 201 10E20
RH02 0 202 10E20
RH03 0 203 10E20
RH04 0 204 10E20
RH05 0 205 10E20

X0101 201 101 Codatron
X0102 201 102 Codatron
X0103 201 103 Codatron
X0104 201 104 Codatron
X0105 201 105 Codatron

X0201 202 101 Codatron
X0202 202 102 Codatron
X0203 202 103 Codatron
X0204 202 104 Codatron
X0205 202 105 Codatron

X0301 203 101 Codatron
X0302 203 102 Codatron
X0303 203 103 Codatron
X0304 203 104 Codatron
X0305 203 105 Codatron

X0401 204 101 Codatron
X0402 204 102 Codatron
X0403 204 103 Codatron
X0404 204 104 Codatron
X0405 204 105 Codatron

X0501 205 101 Codatron
X0502 205 102 Codatron
X0503 205 103 Codatron
X0504 205 104 Codatron
X0505 205 105 Codatron

I1  98 0 0              ; UUT TESTING CURRENT
R98 98 0 10E20          ; VOLTAGE LIMIT IF OPEN
R99 98 203 20K          ; CURRENT LIMIT IF SHORT
RG 103 0  1             ; TO TEST X0303

.MODEL DMOD1 D (BV=398)
.MODEL DMOD2 D (BV=3840)
.SUBCKT Codatron 1 2    ; HT-400
  DZ1 1 3 DMOD1
  DZ2 2 3 DMOD2
.ENDS Codatron

.PRINT DC V(203,103) V(201,103) V(201,101) V(103,0)
.PLOT  DC V(203,103) V(201,103) V(201,101) V(103,0)
.SAVE     V(203,103) V(201,103) V(201,101) V(103,0)
.END
On Sat, 17 Dec 2011 17:43:13 -0800, Robert Baer
<robertbaer@localnet.com> wrote:

> OK, the below listing is accepted by TopSpice (a DOS version) as well >as LTspice (if the .OPTION card is commented out.
Is it LIMPTS or the syntax? PIVTOL should be 1E-20, though that seems ridiculously small.
> LTspice takes a while to give a "result" (no curves in plot pane). > I do not see how one can do an X.. in LTspice so i reverted to TopSpice.
I don't understand the "X" problem?
> >Q#1: How do i get this to work either version)?
You need to make it a file that ends in .cir, and all directives AND netlist must be contained in that file. Some "Spice" variants may not accept ; at the beginning of a line, use * instead.
>Q#2: How could one do this in "plain" LTspice?
Should work, I see no gross violations. What error messages do you get?
> >CODATRON EMULATION IN TESTING ARRAY >* Codatron (TM) TRADEMARKED BY Oil 4 LESS LLC >.OPTION LIMPTS=1000000 PIVTOL=1D-20 ;LTspice DOES NOT ACCEPT LIMPTS.. >.TEMP 25 >.dc I1 -200u 200u 0.001u >; Matrix of Codatron "load" resistors first >; 5x5 ARRAY initially ; NO LTSPICE CURVES..?? >; TopSpice (dos version) complains no .PRINT output data, >; maximum entry at step 6 (5D-5) is less than PIVTOL with .OPTION card >RV01 0 101 10E20 >RV02 0 102 10E20 >RV03 0 103 10E20 >RV04 0 104 10E20 >RV05 0 105 10E20 > >RH01 0 201 10E20 >RH02 0 202 10E20 >RH03 0 203 10E20 >RH04 0 204 10E20 >RH05 0 205 10E20 > >X0101 201 101 Codatron >X0102 201 102 Codatron >X0103 201 103 Codatron >X0104 201 104 Codatron >X0105 201 105 Codatron > >X0201 202 101 Codatron >X0202 202 102 Codatron >X0203 202 103 Codatron >X0204 202 104 Codatron >X0205 202 105 Codatron > >X0301 203 101 Codatron >X0302 203 102 Codatron >X0303 203 103 Codatron >X0304 203 104 Codatron >X0305 203 105 Codatron > >X0401 204 101 Codatron >X0402 204 102 Codatron >X0403 204 103 Codatron >X0404 204 104 Codatron >X0405 204 105 Codatron > >X0501 205 101 Codatron >X0502 205 102 Codatron >X0503 205 103 Codatron >X0504 205 104 Codatron >X0505 205 105 Codatron > >I1 98 0 0 ; UUT TESTING CURRENT >R98 98 0 10E20 ; VOLTAGE LIMIT IF OPEN >R99 98 203 20K ; CURRENT LIMIT IF SHORT >RG 103 0 1 ; TO TEST X0303 > >.MODEL DMOD1 D (BV=398) >.MODEL DMOD2 D (BV=3840) >.SUBCKT Codatron 1 2 ; HT-400 > DZ1 1 3 DMOD1 > DZ2 2 3 DMOD2 >.ENDS Codatron > >.PRINT DC V(203,103) V(201,103) V(201,101) V(103,0) >.PLOT DC V(203,103) V(201,103) V(201,101) V(103,0) >.SAVE V(203,103) V(201,103) V(201,101) V(103,0) >.END
...Jim Thompson -- | James E.Thompson, CTO | mens | | Analog Innovations, Inc. | et | | Analog/Mixed-Signal ASIC's and Discrete Systems | manus | | Phoenix, Arizona 85048 Skype: Contacts Only | | | Voice:(480)460-2350 Fax: Available upon request | Brass Rat | | E-mail Icon at http://www.analog-innovations.com | 1962 | I love to cook with wine. Sometimes I even put it in the food.
On Sat, 17 Dec 2011 17:43:13 -0800, Robert Baer wrote:

> OK, the below listing is accepted by TopSpice (a DOS version) as well > as LTspice (if the .OPTION card is commented out.
No need to ditch the whole .option card, just delete the "LIMPTS" statement. Maybe this is similar to "plotwinsize, in LTSpice.
> LTspice takes a while to give a "result" (no curves in plot pane). I > do not see how one can do an X.. in LTspice so i reverted to TopSpice.
AFAIK, LTSpice does not honor .plot statements, *maybe it should*. You need to run the netlist, then go into the plot pane, right click, and select visible traces.
> > Q#1: How do i get this to work either version)?
If it won't work in TopSpice without the .LIMPTS, you can't
> Q#2: How could one do> this in "plain" LTspice?
Make a symbol for your codatron subckt, draw the schematic, and include the subckt. Or, alternatively, just run the existing netlist, like you already did. -- "For a successful technology, reality must take precedence over public relations, for nature cannot be fooled." (Richard Feynman)
Jim Thompson wrote:
> On Sat, 17 Dec 2011 17:43:13 -0800, Robert Baer > <robertbaer@localnet.com> wrote: > >> OK, the below listing is accepted by TopSpice (a DOS version) as well >> as LTspice (if the .OPTION card is commented out. > > Is it LIMPTS or the syntax? PIVTOL should be 1E-20, though that seems > ridiculously small.
* The syntax is correct for TopSpice; LTspice complains, as i said.
> >> LTspice takes a while to give a "result" (no curves in plot pane). >> I do not see how one can do an X.. in LTspice so i reverted to TopSpice. > > I don't understand the "X" problem?
* You know, when you need a widget that is not simple-minded; it is a sub-circuit call..
> >> Q#1: How do i get this to work either version)? > > You need to make it a file that ends in .cir, and all directives AND > netlist must be contained in that file.
* That is EXACTLY what i have..the listing i gave is the contents of Codatron.CIR .
> > Some "Spice" variants may not accept ; at the beginning of a line, use > * instead.
* For example LTspice??
> >> Q#2: How could one do this in "plain" LTspice? > > Should work, I see no gross violations. What error messages do you > get?
* Read what i said..look at end here for more info.
> >> CODATRON EMULATION IN TESTING ARRAY >> * Codatron (TM) TRADEMARKED BY Oil 4 LESS LLC >> .OPTION LIMPTS=1000000 PIVTOL=1D-20 ;LTspice DOES NOT ACCEPT LIMPTS.. >> .TEMP 25 >> .dc I1 -200u 200u 0.001u >> ; Matrix of Codatron "load" resistors first >> ; 5x5 ARRAY initially ; NO LTSPICE CURVES..?? >> ; TopSpice (dos version) complains no .PRINT output data, >> ; maximum entry at step 6 (5D-5) is less than PIVTOL with .OPTION card >> RV01 0 101 10E20 >> RV02 0 102 10E20 >> RV03 0 103 10E20 >> RV04 0 104 10E20 >> RV05 0 105 10E20 >> >> RH01 0 201 10E20 >> RH02 0 202 10E20 >> RH03 0 203 10E20 >> RH04 0 204 10E20 >> RH05 0 205 10E20 >> >> X0101 201 101 Codatron >> X0102 201 102 Codatron >> X0103 201 103 Codatron >> X0104 201 104 Codatron >> X0105 201 105 Codatron >> >> X0201 202 101 Codatron >> X0202 202 102 Codatron >> X0203 202 103 Codatron >> X0204 202 104 Codatron >> X0205 202 105 Codatron >> >> X0301 203 101 Codatron >> X0302 203 102 Codatron >> X0303 203 103 Codatron >> X0304 203 104 Codatron >> X0305 203 105 Codatron >> >> X0401 204 101 Codatron >> X0402 204 102 Codatron >> X0403 204 103 Codatron >> X0404 204 104 Codatron >> X0405 204 105 Codatron >> >> X0501 205 101 Codatron >> X0502 205 102 Codatron >> X0503 205 103 Codatron >> X0504 205 104 Codatron >> X0505 205 105 Codatron >> >> I1 98 0 0 ; UUT TESTING CURRENT >> R98 98 0 10E20 ; VOLTAGE LIMIT IF OPEN >> R99 98 203 20K ; CURRENT LIMIT IF SHORT >> RG 103 0 1 ; TO TEST X0303 >> >> .MODEL DMOD1 D (BV=398) >> .MODEL DMOD2 D (BV=3840) >> .SUBCKT Codatron 1 2 ; HT-400 >> DZ1 1 3 DMOD1 >> DZ2 2 3 DMOD2 >> .ENDS Codatron >> >> .PRINT DC V(203,103) V(201,103) V(201,101) V(103,0) >> .PLOT DC V(203,103) V(201,103) V(201,101) V(103,0) >> .SAVE V(203,103) V(201,103) V(201,101) V(103,0) >> .END > > ...Jim Thompson
A snip from output file: CODATRON EMULATION IN TESTING ARRAY **** TEMPERATURE-ADJUSTED VALUES TEMPERATURE = 25.000 DEG C *********************************************************************** 0**** DIODE MODEL PARAMETERS 0NAME IS VJ CJO DMOD1 7.350D-15 1.002D+00 0.000D+00 DMOD2 7.350D-15 1.002D+00 0.000D+00 0*ERROR*: MAXIMUM ENTRY IN THIS COLUMN AT STEP 12 (5.000000D-05) IS LESS THAN PIVTOL 0*ERROR*: MAXIMUM ENTRY IN THIS COLUMN AT STEP 12 (5.000000D-05) IS LESS THAN PIVTOL 0*ERROR*: MAXIMUM ENTRY IN THIS COLUMN AT STEP 12 (5.000000D-05) IS LESS THAN PIVTOL 0*ERROR*: MAXIMUM ENTRY IN THIS COLUMN AT STEP 12 (5.000000D-05) IS LESS THAN PIVTOL 0*ERROR*: MAXIMUM ENTRY IN THIS COLUMN AT STEP 12 (5.000000D-05) IS LESS THAN PIVTOL 0*ERROR*: MAXIMUM ENTRY IN THIS COLUMN AT STEP 12 (5.000000D-05) IS LESS THAN PIVTOL 0*ERROR*: MAXIMUM ENTRY IN THIS COLUMN AT STEP 12 (5.000000D-05) IS LESS THAN PIVTOL 0 SOURCE STEPPING METHOD FAILED Number of steps = 7 Power supplies at .781% 1*ERROR*: NO CONVERGENCE IN DC TRANSFER CURVES AT I1 = -2.000D-04 0LAST NODE VOLTAGES: NODE VOLTAGE NODE VOLTAGE NODE VOLTAGE (101 ) .0000 (102 ) .0000 (103 ) .0000 (104 ) .0000 (105 ) .0000 (201 ) .0000 (202 ) .0000 (203 ) .0000 (204 ) .0000 (205 ) .0000 (98 ) .0000 (3.X0101 ) .0000 (3.X0102 ) .0000 (3.X0103 ) .0000 (3.X0104 ) .0000 (3.X0105 ) .0000 (3.X0201 ) .0000 (3.X0202 ) .0000 (3.X0203 ) .0000 (3.X0204 ) .0000 (3.X0205 ) .0000 (3.X0301 ) .0000 (3.X0302 ) .0000 (3.X0303 ) .0000 (3.X0304 ) .0000 (3.X0305 ) .0000 (3.X0401 ) .0000 (3.X0402 ) .0000 (3.X0403 ) .0000 (3.X0404 ) .0000 (3.X0405 ) .0000 (3.X0501 ) .0000 (3.X0502 ) .0000 (3.X0503 ) .0000 (3.X0504 ) .0000 (3.X0505 ) .0000 0 ***** JOB ABORTED TOTAL JOB TIME .05
Fred Abse wrote:
> On Sat, 17 Dec 2011 17:43:13 -0800, Robert Baer wrote: > >> OK, the below listing is accepted by TopSpice (a DOS version) as well >> as LTspice (if the .OPTION card is commented out. > > No need to ditch the whole .option card, just delete the "LIMPTS" > statement. Maybe this is similar to "plotwinsize, in LTSpice. > > >> LTspice takes a while to give a "result" (no curves in plot pane). I >> do not see how one can do an X.. in LTspice so i reverted to TopSpice. > > AFAIK, LTSpice does not honor .plot statements, *maybe it should*. > > You need to run the netlist, then go into the plot pane, right click, and > select visible traces.
* "run the netlist" ?? in LTspice, how? There are NO visible traces (yet).
> >> Q#1: How do i get this to work either version)? > > If it won't work in TopSpice without the .LIMPTS, you can't > > >> Q#2: How could one do> this in "plain" LTspice? > > Make a symbol for your codatron subckt, draw the schematic, and include > the subckt.
* In LT spice, how is this done (fake a symbol), and how does one refer to the subcircuit,as there seems to be no X..
> > Or, alternatively, just run the existing netlist, like you already did. >
Well if i did that, then why do i get nothing?
On Mon, 19 Dec 2011 00:12:49 -0800, Robert Baer
<robertbaer@localnet.com> wrote:

>Jim Thompson wrote: >> On Sat, 17 Dec 2011 17:43:13 -0800, Robert Baer >> <robertbaer@localnet.com> wrote: >> >>> OK, the below listing is accepted by TopSpice (a DOS version) as well >>> as LTspice (if the .OPTION card is commented out. >> >> Is it LIMPTS or the syntax? PIVTOL should be 1E-20, though that seems >> ridiculously small. >* The syntax is correct for TopSpice; LTspice complains, as i said. > >> >>> LTspice takes a while to give a "result" (no curves in plot pane). >>> I do not see how one can do an X.. in LTspice so i reverted to TopSpice. >> >> I don't understand the "X" problem? >* You know, when you need a widget that is not simple-minded; it is a >sub-circuit call.. > >> >>> Q#1: How do i get this to work either version)? >> >> You need to make it a file that ends in .cir, and all directives AND >> netlist must be contained in that file. >* That is EXACTLY what i have..the listing i gave is the contents of >Codatron.CIR . > >> >> Some "Spice" variants may not accept ; at the beginning of a line, use >> * instead. >* For example LTspice?? > >> >>> Q#2: How could one do this in "plain" LTspice? >> >> Should work, I see no gross violations. What error messages do you >> get? >* Read what i said..look at end here for more info. > >> >>> CODATRON EMULATION IN TESTING ARRAY >>> * Codatron (TM) TRADEMARKED BY Oil 4 LESS LLC >>> .OPTION LIMPTS=1000000 PIVTOL=1D-20 ;LTspice DOES NOT ACCEPT LIMPTS.. >>> .TEMP 25 >>> .dc I1 -200u 200u 0.001u >>> ; Matrix of Codatron "load" resistors first >>> ; 5x5 ARRAY initially ; NO LTSPICE CURVES..?? >>> ; TopSpice (dos version) complains no .PRINT output data, >>> ; maximum entry at step 6 (5D-5) is less than PIVTOL with .OPTION card >>> RV01 0 101 10E20 >>> RV02 0 102 10E20 >>> RV03 0 103 10E20 >>> RV04 0 104 10E20 >>> RV05 0 105 10E20 >>> >>> RH01 0 201 10E20 >>> RH02 0 202 10E20 >>> RH03 0 203 10E20 >>> RH04 0 204 10E20 >>> RH05 0 205 10E20 >>> >>> X0101 201 101 Codatron >>> X0102 201 102 Codatron >>> X0103 201 103 Codatron >>> X0104 201 104 Codatron >>> X0105 201 105 Codatron >>> >>> X0201 202 101 Codatron >>> X0202 202 102 Codatron >>> X0203 202 103 Codatron >>> X0204 202 104 Codatron >>> X0205 202 105 Codatron >>> >>> X0301 203 101 Codatron >>> X0302 203 102 Codatron >>> X0303 203 103 Codatron >>> X0304 203 104 Codatron >>> X0305 203 105 Codatron >>> >>> X0401 204 101 Codatron >>> X0402 204 102 Codatron >>> X0403 204 103 Codatron >>> X0404 204 104 Codatron >>> X0405 204 105 Codatron >>> >>> X0501 205 101 Codatron >>> X0502 205 102 Codatron >>> X0503 205 103 Codatron >>> X0504 205 104 Codatron >>> X0505 205 105 Codatron >>> >>> I1 98 0 0 ; UUT TESTING CURRENT >>> R98 98 0 10E20 ; VOLTAGE LIMIT IF OPEN >>> R99 98 203 20K ; CURRENT LIMIT IF SHORT >>> RG 103 0 1 ; TO TEST X0303 >>> >>> .MODEL DMOD1 D (BV=398) >>> .MODEL DMOD2 D (BV=3840) >>> .SUBCKT Codatron 1 2 ; HT-400 >>> DZ1 1 3 DMOD1 >>> DZ2 2 3 DMOD2 >>> .ENDS Codatron >>> >>> .PRINT DC V(203,103) V(201,103) V(201,101) V(103,0) >>> .PLOT DC V(203,103) V(201,103) V(201,101) V(103,0) >>> .SAVE V(203,103) V(201,103) V(201,101) V(103,0) >>> .END >> >> ...Jim Thompson > > A snip from output file: > CODATRON EMULATION IN TESTING ARRAY > > **** TEMPERATURE-ADJUSTED VALUES TEMPERATURE = 25.000 DEG C > > *********************************************************************** > > > > >0**** DIODE MODEL PARAMETERS >0NAME IS VJ CJO > > > DMOD1 7.350D-15 1.002D+00 0.000D+00 > DMOD2 7.350D-15 1.002D+00 0.000D+00 >0*ERROR*: MAXIMUM ENTRY IN THIS COLUMN AT STEP 12 (5.000000D-05) IS >LESS THAN PIVTOL >0*ERROR*: MAXIMUM ENTRY IN THIS COLUMN AT STEP 12 (5.000000D-05) IS >LESS THAN PIVTOL >0*ERROR*: MAXIMUM ENTRY IN THIS COLUMN AT STEP 12 (5.000000D-05) IS >LESS THAN PIVTOL >0*ERROR*: MAXIMUM ENTRY IN THIS COLUMN AT STEP 12 (5.000000D-05) IS >LESS THAN PIVTOL >0*ERROR*: MAXIMUM ENTRY IN THIS COLUMN AT STEP 12 (5.000000D-05) IS >LESS THAN PIVTOL >0*ERROR*: MAXIMUM ENTRY IN THIS COLUMN AT STEP 12 (5.000000D-05) IS >LESS THAN PIVTOL >0*ERROR*: MAXIMUM ENTRY IN THIS COLUMN AT STEP 12 (5.000000D-05) IS >LESS THAN PIVTOL >0 SOURCE STEPPING METHOD FAILED > Number of steps = 7 Power supplies at .781% >1*ERROR*: NO CONVERGENCE IN DC TRANSFER CURVES AT I1 = -2.000D-04 >0LAST NODE VOLTAGES: > > NODE VOLTAGE NODE VOLTAGE NODE VOLTAGE > > (101 ) .0000 (102 ) .0000 (103 ) .0000 > (104 ) .0000 (105 ) .0000 (201 ) .0000 > (202 ) .0000 (203 ) .0000 (204 ) .0000 > (205 ) .0000 (98 ) .0000 (3.X0101 ) .0000 > (3.X0102 ) .0000 (3.X0103 ) .0000 (3.X0104 ) .0000 > (3.X0105 ) .0000 (3.X0201 ) .0000 (3.X0202 ) .0000 > (3.X0203 ) .0000 (3.X0204 ) .0000 (3.X0205 ) .0000 > (3.X0301 ) .0000 (3.X0302 ) .0000 (3.X0303 ) .0000 > (3.X0304 ) .0000 (3.X0305 ) .0000 (3.X0401 ) .0000 > (3.X0402 ) .0000 (3.X0403 ) .0000 (3.X0404 ) .0000 > (3.X0405 ) .0000 (3.X0501 ) .0000 (3.X0502 ) .0000 > (3.X0503 ) .0000 (3.X0504 ) .0000 (3.X0505 ) .0000 >0 ***** JOB ABORTED > > TOTAL JOB TIME .05
Maybe you got snagged by LTspice's "diode" ;-) Set all options back to default, and try it again. ...Jim Thompson -- | James E.Thompson, CTO | mens | | Analog Innovations, Inc. | et | | Analog/Mixed-Signal ASIC's and Discrete Systems | manus | | Phoenix, Arizona 85048 Skype: Contacts Only | | | Voice:(480)460-2350 Fax: Available upon request | Brass Rat | | E-mail Icon at http://www.analog-innovations.com | 1962 | I love to cook with wine. Sometimes I even put it in the food.
On Mon, 19 Dec 2011 00:18:09 -0800, Robert Baer
<robertbaer@localnet.com> wrote:

>Fred Abse wrote: >> On Sat, 17 Dec 2011 17:43:13 -0800, Robert Baer wrote: >> >>> OK, the below listing is accepted by TopSpice (a DOS version) as well >>> as LTspice (if the .OPTION card is commented out. >> >> No need to ditch the whole .option card, just delete the "LIMPTS" >> statement. Maybe this is similar to "plotwinsize, in LTSpice. >> >> >>> LTspice takes a while to give a "result" (no curves in plot pane). I >>> do not see how one can do an X.. in LTspice so i reverted to TopSpice. >> >> AFAIK, LTSpice does not honor .plot statements, *maybe it should*. >> >> You need to run the netlist, then go into the plot pane, right click, and >> select visible traces. >* "run the netlist" ?? in LTspice, how? > There are NO visible traces (yet). > >> >>> Q#1: How do i get this to work either version)? >> >> If it won't work in TopSpice without the .LIMPTS, you can't >> >> >>> Q#2: How could one do> this in "plain" LTspice? >> >> Make a symbol for your codatron subckt, draw the schematic, and include >> the subckt. >* In LT spice, how is this done (fake a symbol), and how does one refer >to the subcircuit,as there seems to be no X.. >> >> Or, alternatively, just run the existing netlist, like you already did. >> > Well if i did that, then why do i get nothing?
ESTO ?:-) ...Jim Thompson -- | James E.Thompson, CTO | mens | | Analog Innovations, Inc. | et | | Analog/Mixed-Signal ASIC's and Discrete Systems | manus | | Phoenix, Arizona 85048 Skype: Contacts Only | | | Voice:(480)460-2350 Fax: Available upon request | Brass Rat | | E-mail Icon at http://www.analog-innovations.com | 1962 | I love to cook with wine. Sometimes I even put it in the food.
On Mon, 19 Dec 2011 00:18:09 -0800, Robert Baer wrote:

> Well if i did that, then why do i get nothing?
Because, as I said, LTSPice does not honor .plot statements directly in netlists. A blank plot window should have automatically opened, however. Go into that window (click on its title bar). Left click, or alternatively select "Plot Settings", then "Visible Traces". You'll be offered V(101), V(103), V(201), V(203). For a start, select V(203). A plot will appear of V(203). Right click on the "V(203)" header, an edit box will appear. Edit "V(203)2 to read (V203,103). Click OK, the plot will then change itself. Do the same for the rest. You can then save those plot settings. LTSpice is GUI-oriented. You're expected to probe the circuit voltages and currents directly from a schematic. From someone else's netlist, it's a PITA. IMO, it should support .plot and .print statements, however. Polar and Smith plots would be nice, too. Even Berkeley Spice 3 could do those. The .net directive is probably the most useful LTSpice innovation to me, Zin, Zout, Yin, Yout, s-parameters, h-parameters, automatically. -- "For a successful technology, reality must take precedence over public relations, for nature cannot be fooled." (Richard Feynman)
On Mon, 19 Dec 2011 08:41:47 -0800, Fred Abse
<excretatauris@invalid.invalid> wrote:

>On Mon, 19 Dec 2011 00:18:09 -0800, Robert Baer wrote: > >> Well if i did that, then why do i get nothing? > >Because, as I said, LTSPice does not honor .plot statements directly in >netlists. > >A blank plot window should have automatically opened, however. >Go into that window (click on its title bar). >Left click, or alternatively select "Plot Settings", then "Visible Traces". >You'll be offered V(101), V(103), V(201), V(203). >For a start, select V(203). A plot will appear of V(203). >Right click on the "V(203)" header, an edit box will appear. >Edit "V(203)2 to read (V203,103). >Click OK, the plot will then change itself. >Do the same for the rest. You can then save those plot settings. > >LTSpice is GUI-oriented. You're expected to probe the circuit voltages >and currents directly from a schematic. From someone else's netlist, it's >a PITA. IMO, it should support .plot and .print statements, however. Polar >and Smith plots would be nice, too. Even Berkeley Spice 3 could do those. >The .net directive is probably the most useful LTSpice innovation to me, >Zin, Zout, Yin, Yout, s-parameters, h-parameters, automatically.
LTspice follows the PSpice approach... .PROBE [V(Node) List] or wild card... .PROBE V(*) I(*) W(*) D(*) NOISE(*) You still have to pick from a list ...Jim Thompson -- | James E.Thompson, CTO | mens | | Analog Innovations, Inc. | et | | Analog/Mixed-Signal ASIC's and Discrete Systems | manus | | Phoenix, Arizona 85048 Skype: Contacts Only | | | Voice:(480)460-2350 Fax: Available upon request | Brass Rat | | E-mail Icon at http://www.analog-innovations.com | 1962 | I love to cook with wine. Sometimes I even put it in the food.
On Mon, 19 Dec 2011 10:26:49 -0700, Jim Thompson
<To-Email-Use-The-Envelope-Icon@On-My-Web-Site.com> wrote:

>On Mon, 19 Dec 2011 08:41:47 -0800, Fred Abse ><excretatauris@invalid.invalid> wrote: > >>On Mon, 19 Dec 2011 00:18:09 -0800, Robert Baer wrote: >> >>> Well if i did that, then why do i get nothing? >> >>Because, as I said, LTSPice does not honor .plot statements directly in >>netlists. >> >>A blank plot window should have automatically opened, however. >>Go into that window (click on its title bar). >>Left click, or alternatively select "Plot Settings", then "Visible Traces". >>You'll be offered V(101), V(103), V(201), V(203). >>For a start, select V(203). A plot will appear of V(203). >>Right click on the "V(203)" header, an edit box will appear. >>Edit "V(203)2 to read (V203,103). >>Click OK, the plot will then change itself. >>Do the same for the rest. You can then save those plot settings. >> >>LTSpice is GUI-oriented. You're expected to probe the circuit voltages >>and currents directly from a schematic. From someone else's netlist, it's >>a PITA. IMO, it should support .plot and .print statements, however. Polar >>and Smith plots would be nice, too. Even Berkeley Spice 3 could do those. >>The .net directive is probably the most useful LTSpice innovation to me, >>Zin, Zout, Yin, Yout, s-parameters, h-parameters, automatically. > >LTspice follows the PSpice approach... > >.PROBE [V(Node) List] > >or wild card... > >.PROBE V(*) I(*) W(*) D(*) NOISE(*) > >You still have to pick from a list > > ...Jim Thompson
I should have also mentioned... .PRINT [V(Node) List] Puts the data in the .OUT file as a numeric list. I do that all the time in PSpice to get numeric data into Excel, etc. In PSpice you have to use a symbol to force that .PRINT statement, PSpice has removed it from the "directives" list. ...Jim Thompson -- | James E.Thompson, CTO | mens | | Analog Innovations, Inc. | et | | Analog/Mixed-Signal ASIC's and Discrete Systems | manus | | Phoenix, Arizona 85048 Skype: Contacts Only | | | Voice:(480)460-2350 Fax: Available upon request | Brass Rat | | E-mail Icon at http://www.analog-innovations.com | 1962 | I love to cook with wine. Sometimes I even put it in the food.