| blu_line |
Hello all,
For those simulating with LT_Spice; i have created a DPST realy.
I needed it myself.
Place The following, cut between *'s, in a file called DPST.asy
This is the symbol.
**************************************************
Version 4
SymbolType CELL
RECTANGLE Normal 64 96 -16 -48
SYMATTR Value DPST
SYMATTR Prefix X
SYMATTR SpiceModel DPST.sub
SYMATTR Value2 DPST
SYMATTR Description An DPST model.
PIN -16 -32 LEFT 8
PINATTR PinName 1
PINATTR SpiceOrder 1
PIN -16 0 LEFT 8
PINATTR PinName 2
PINATTR SpiceOrder 2
PIN -16 48 LEFT 8
PINATTR PinName 6
PINATTR SpiceOrder 3
PIN -16 80 LEFT 8
PINATTR PinName 7
PINATTR SpiceOrder 4
PIN 64 80 RIGHT 8
PINATTR PinName 8
PINATTR SpiceOrder 5
PIN 64 -32 RIGHT 8
PINATTR PinName 14
PINATTR SpiceOrder 6
************************************************
Place the file in the misc directory.
The following is the spice model. Paste it into a file called DPST.sub. Put it in the "sub" directory.
************************************************
* Copyright © Linear Technology Corp. 1998, 1999, 2000, 2001, 2002, 2003. All rights reserved.
*
.subckt DPST 1 2 3 4 5 6
S1 1 5 n001 3 SW_NC
S2 5 6 n001 3 SW_NO
R1 4 5 0.1
R2 2 n001 200
.model SW_NC SW(Ron=6 Roff=1G Vt=0.5 Vh=0.4)
.model SW_NO SW(Ron=1G Roff=6 Vt=0.5 Vh=0.4)
.ends DPST
************************************************
The model is like "normal" DPST reed relays.
Pin 1 to Pin 8 (and 7) has a normally closed.
Pin 14 to pin 8 (and 7) is normally open.
Between pin 2 and 6 it has the coil with a resistance of 200 ohms.
grtz
SImon |
|
|
|
