How to enter an scr into linear-spice ?

A

Abbie

Guest
I have downloaded the spice program from linear.com ;
I now want to simulated a circuit which contains an scr ;
It seems that there is an scr symbol, but when I try to
simulate the symbol is not recognized. Any ideas ?
Rex
 
"Abbie" <AbbieAbbieAbbie@btinternet.com> schrieb im Newsbeitrag
news:bpqohm$38j$1@sparta.btinternet.com...
I have downloaded the spice program from linear.com ;
I now want to simulated a circuit which contains an scr ;
It seems that there is an scr symbol, but when I try to
simulate the symbol is not recognized. Any ideas ?
Rex
Click to expand...
Hello Rex,
I have added my working oscillator schematic and my
SCR-library file. The simple command line .include mylib.scr
in the schematic tells LTSPICE what file it has to load
to your design. Please put the library file into the same
directory where your schematic is.

Don't spend too much time on this SCR oscillator. It can
never be a good(part tolerant) design.

Take a look to the LTSPICE-YAHOO group too. There is a
detailed explanation about symbols and models in this section.
http://groups.yahoo.com/group/LTspice/files/Tut/


Best Regards,
Helmut



The LTSPICE schematic file: SCR_osc.asc


Version 4
SHEET 1 1832 804
WIRE 128 -112 128 16
WIRE 128 16 -96 16
WIRE 128 -688 128 -720
WIRE 128 -720 -96 -720
WIRE -480 -720 -480 -272
WIRE -480 16 -480 -192
WIRE -480 48 -480 16
WIRE -416 -720 -480 -720
WIRE -288 -288 -288 -720
WIRE -288 -720 -336 -720
WIRE -288 -224 -288 16
WIRE -288 16 -480 16
WIRE -96 -80 -96 -112
WIRE -96 -224 -96 -272
WIRE -96 16 -96 0
WIRE -96 16 -288 16
WIRE 80 -112 -96 -112
WIRE -96 -112 -96 -144
WIRE -96 -336 -96 -720
WIRE -96 -720 -288 -720
WIRE 128 -256 128 -176
WIRE 128 -560 128 -608
WIRE 128 -320 128 -256
WIRE 16 -336 16 -256
WIRE 16 -256 128 -256
WIRE 16 -400 16 -464
WIRE 16 -464 128 -464
WIRE 128 -464 128 -400
WIRE 128 -464 128 -480
WIRE 128 -464 240 -464
WIRE 240 -464 240 -400
WIRE 240 -320 240 -256
WIRE 240 -256 128 -256
WIRE 1088 -112 1088 16
WIRE 1088 16 880 16
WIRE 1088 -688 1088 -720
WIRE 1088 -720 880 -720
WIRE 480 -720 480 -272
WIRE 480 16 480 -192
WIRE 480 48 480 16
WIRE 544 -720 480 -720
WIRE 672 -288 672 -720
WIRE 672 -720 624 -720
WIRE 672 -224 672 16
WIRE 672 16 480 16
WIRE 880 -80 880 -112
WIRE 880 -224 880 -272
WIRE 880 16 880 0
WIRE 880 16 672 16
WIRE 1040 -112 880 -112
WIRE 880 -112 880 -144
WIRE 880 -336 880 -720
WIRE 880 -720 672 -720
WIRE 1088 -256 1088 -176
WIRE 1088 -560 1088 -608
WIRE 1088 -320 1088 -256
WIRE 976 -336 976 -256
WIRE 976 -256 1088 -256
WIRE 976 -400 976 -464
WIRE 976 -464 1088 -464
WIRE 1088 -464 1088 -400
WIRE 1088 -464 1088 -480
WIRE 1088 -464 1200 -464
WIRE 1200 -464 1200 -400
WIRE 1200 -320 1200 -256
WIRE 1200 -256 1088 -256
FLAG -480 48 0
FLAG 480 48 0
SYMBOL Misc\\SCR 112 -176 R0
SYMATTR InstName U1
SYMATTR Value X2N2326
SYMBOL voltage -480 -288 R0
SYMATTR InstName V1
SYMATTR Value 12
SYMBOL res -432 -704 R270
WINDOW 0 32 56 VTop 0
WINDOW 3 0 56 VBottom 0
SYMATTR InstName R1
SYMATTR Value 220
SYMBOL cap -304 -288 R0
SYMATTR InstName C1
SYMATTR Value 2.2ľ
SYMBOL zener -80 -272 R180
WINDOW 0 24 72 Left 0
WINDOW 3 24 0 Left 0
SYMATTR InstName D1
SYMATTR Value BZX84C8V2L
SYMATTR Description Diode
SYMATTR Type diode
SYMBOL res -112 -240 R0
SYMATTR InstName R2
SYMATTR Value 1k
SYMBOL res -112 -96 R0
SYMATTR InstName R3
SYMATTR Value 1k
SYMBOL res 112 -704 R0
SYMATTR InstName R4
SYMATTR Value 5
SYMBOL ind 112 -576 R0
SYMATTR InstName L4
SYMATTR Value 0.2m
SYMBOL ind 112 -416 R0
SYMATTR InstName L5
SYMATTR Value 0.2m
SYMBOL cap 0 -400 R0
SYMATTR InstName C5
SYMATTR Value 10m
SYMBOL res 224 -416 R0
SYMATTR InstName R5
SYMATTR Value 20
SYMBOL Misc\\SCR 1072 -176 R0
SYMATTR InstName U10
SYMATTR Value EC103A
SYMBOL voltage 480 -288 R0
SYMATTR InstName V10
SYMATTR Value 12
SYMBOL res 528 -704 R270
WINDOW 0 32 56 VTop 0
WINDOW 3 0 56 VBottom 0
SYMATTR InstName R10
SYMATTR Value 1k
SYMBOL cap 656 -288 R0
SYMATTR InstName C20
SYMATTR Value 2.2ľ
SYMBOL zener 896 -272 R180
WINDOW 0 24 72 Left 0
WINDOW 3 24 0 Left 0
SYMATTR InstName D10
SYMATTR Value BZX84C6V2L
SYMATTR Description Diode
SYMATTR Type diode
SYMBOL res 864 -240 R0
SYMATTR InstName R20
SYMATTR Value 1k
SYMBOL res 864 -96 R0
SYMATTR InstName R30
SYMATTR Value 10k
SYMBOL res 1072 -704 R0
SYMATTR InstName R40
SYMATTR Value 5
SYMBOL ind 1072 -576 R0
SYMATTR InstName L40
SYMATTR Value 0.2m
SYMBOL ind 1072 -416 R0
SYMATTR InstName L50
SYMATTR Value 0.2m
SYMBOL cap 960 -400 R0
SYMATTR InstName C50
SYMATTR Value 10m
SYMBOL res 1184 -416 R0
SYMATTR InstName R50
SYMATTR Value 20
TEXT -480 -824 Left 0 !.tran 0 20m 0 1u startup
TEXT 248 -816 Left 0 ;SCR Oscillator Circuits
TEXT 1312 -424 VLeft 0 ;LOUDSPEAKER
TEXT 304 -416 VLeft 0 ;LOUDSPEAKER
TEXT -480 -888 Left 0 !.include myscr.lib
RECTANGLE Normal 336 -224 -64 -704
RECTANGLE Normal 1344 -224 944 -704




The library file: myscr.lib


* From www.teccor.com
*SYM=SCR
*SRC=EC103A;EC103A;SCRs;TECCOR; 100V 0.8A
..SUBCKT EC103A 1 2 3
* TERMINALS: A G K
QP 6 4 1 POUT OFF
QN 4 6 5 NOUT OFF
RF 6 4 200K
RR 1 4 133K
RGK 6 5 240
RG 2 6 9.09
RK 3 5 0.112
DF 6 4 ZF
DR 1 4 ZR
DGK 6 5 ZGK
..MODEL ZF D (IS=3.2E-16 IBV=100U BV=100)
..MODEL ZR D (IS=3.2E-16 IBV=100U BV=100)
..MODEL ZGK D (IS=3.2E-16 IBV=100U BV=5)
..MODEL POUT PNP (IS=320F BF=1 CJE=112P TF=85U)
..MODEL NOUT NPN (IS=320F BF=100 RC=0.45 CJE=558P CJC=112P TF=5.95U)
..ENDS
*
*
* From www.duncanamps.com
*Motorola 200V If=1.6A Igt=.2mA Vgt=.8V: A G K
..SUBCKT X2N2326 1 2 3
QP 6 4 1 POUT OFF
QN 4 6 5 NOUT OFF
RF 6 4 40MEG
RR 1 4 26.6MEG
RGK 6 5 2.25k
RG 2 6 51.9
RK 3 5 43.3M
DF 6 4 ZF
DR 1 4 ZR
DGK 6 5 ZGK
..MODEL ZF D (IS=.64F IBV=1U BV=200 RS=6MEG)
..MODEL ZR D (IS=.64F IBV=1U BV=266)
..MODEL ZGK D (IS=.64F IBV=1U BV=5)
..MODEL POUT PNP (IS=640F BF=1 CJE=1.34N)
..MODEL NOUT NPN (IS=640F BF=100 RC=.173
+ CJE=1.34N CJC=268P TF=80.1N TR=11.4U)
..ENDS X2N2326
 
Helmut Sennewald, Abbie wrote:

I have downloaded the spice program from linear.com ;
I now want to simulated a circuit which contains an scr ;
It seems that there is an scr symbol, but when I try to
simulate the symbol is not recognized. Any ideas ?
Click to expand...
To use the scr symbol follow Helmut's excellent instructions.
(Copy and paste from his post to an ascii text editor to create
the two files. Control that the extensions are .asc and .lib
rather than .txt.)

Or - you could skip dealing with the scr symbol altogether and
replace it with a functionally equivalent two transistor circuit.
Place a 2N2222 with its base to the left and its emitter to ground.
Above this place a 2N2907 such that its collector can be connected
to the npn's base and its base can be connected to the npn's
collector. Now place a 100 ohm resistor across the pnp's base and
emitter. The pnp's emitter forms the "scr's" anode, the gate is
the npn's base, and the cathode is the npn's emitter.

For the speaker coil, place an inductor onto the schematic then
right click on it with the mouse and set its inductance to 100uH
or so and its resistance to 5 or 6 ohms.

I have added my working oscillator schematic and my
SCR-library file. The simple command line .include mylib.scr
in the schematic tells LTSPICE what file it has to load
to your design. Please put the library file into the same
directory where your schematic is.

Don't spend too much time on this SCR oscillator. It can
never be a good (part tolerant) design.
Click to expand...
That may be a little harsh, in my opinion.

Take a look to the LTSPICE-YAHOO group too. There is a
detailed explanation about symbols and models in this section.
http://groups.yahoo.com/group/LTspice/files/Tut/
Click to expand...
Yes indeed, it would be well worth the time spent.

Good luck. -- analog
 
"analog" <analog@ieee.org> wrote in message news:3FC157EF.6EB6AD08@ieee.org...
Helmut Sennewald, Abbie wrote:

I have downloaded the spice program from linear.com ;
I now want to simulated a circuit which contains an scr ;
It seems that there is an scr symbol, but when I try to
simulate the symbol is not recognized. Any ideas ?

To use the scr symbol follow Helmut's excellent instructions.
(Copy and paste from his post to an ascii text editor to create
the two files. Control that the extensions are .asc and .lib
rather than .txt.)

Or - you could skip dealing with the scr symbol altogether and
replace it with a functionally equivalent two transistor circuit.
Place a 2N2222 with its base to the left and its emitter to ground.
Above this place a 2N2907 such that its collector can be connected
to the npn's base and its base can be connected to the npn's
collector. Now place a 100 ohm resistor across the pnp's base and
emitter. The pnp's emitter forms the "scr's" anode, the gate is
the npn's base, and the cathode is the npn's emitter.
Click to expand...
Are you sure the resistor is across pnp's base and emitter, I have
a link which shows a configuration with two resistors, see this one:

http://www.uoguelph.ca/~antoon/gadgets/triacs/triacs.html

fig. 1(b)



For the speaker coil, place an inductor onto the schematic then
right click on it with the mouse and set its inductance to 100uH
or so and its resistance to 5 or 6 ohms.

I have added my working oscillator schematic and my
SCR-library file. The simple command line .include mylib.scr
in the schematic tells LTSPICE what file it has to load
to your design. Please put the library file into the same
directory where your schematic is.

Don't spend too much time on this SCR oscillator. It can
never be a good (part tolerant) design.

That may be a little harsh, in my opinion.

Take a look to the LTSPICE-YAHOO group too. There is a
detailed explanation about symbols and models in this section.
http://groups.yahoo.com/group/LTspice/files/Tut/

Yes indeed, it would be well worth the time spent.

Good luck. -- analog
Click to expand...
 
Abbie wrote:

Are you sure the resistor is across pnp's base and emitter, I have
a link which shows a configuration with two resistors, see this one:
Click to expand...
I have tried to give you the simplest model that still captures the
circuit behavior of interest. The pnp's base-emitter resistor is
needed to adjust the holding current. My advice to you is, since the
model is so simple, enter it into LTspice and try it out. Then it is
a simple matter to play with the resistor's value. Don't take my word
or that of someone's web site. Run experiment within the simulator
and come to your own conclusions. Then compare to a real life
breadboard and readjust and/or add detail to your model if and as
required until the two match well enough for your purposes.
 
You must log in or register to reply here.

Welcome to EDABoard.com

Sponsor

Back
Top