spice model for incandescent lamp

Günter R

unread,

May 28, 2001, 4:41:31 PM5/28/01

to

has someone got a spice model for an incandescent lamp
i.e. 100 W/230 V?

Jim_Thompson

unread,

May 28, 2001, 5:14:16 PM5/28/01

to

On Mon, 28 May 2001 22:41:31 +0200, "Günter R" <gu...@web.de> wrote:

|has someone got a spice model for an incandescent lamp
|i.e. 100 W/230 V?
|

Here's one that works with PSpice. You may need to convert it to
"poly" notation to get it to work with other "Spices".

*VO=NOMINAL OPERATING VOLTAGE
*IO=NOMINAL STEADY STATE OPERATING CURRENT
*RCOLD=FILAMEMT RESISTANCE MEASURED AT ROOM TEMP (300K)
*TAU=CURRENT TIME CONSTANT AFTER A 0 (zero) TO VO STEP IS APPLIED
.SUBCKT LAMP 1 2 PARAMS: VO=28 IO=25m RCOLD=112 TAU=22m TAMB=300
H1 6 0 VML 1
RH1 6 0 1
GP 0 4 VALUE={V(6)*V(1,2)}
*V(4,0) = FILAMENT TEMPERATURE IN KELVINS
RT 4 5 {300*(VO-IO*RCOLD)/(IO*IO*VO*RCOLD)}
CT 4 5 {TAU*IO*IO*VO*RCOLD/(300*(VO-IO*RCOLD))}
VAMB 5 0 {TAMB}
El 7 0 1 2 300
R1 7 0 1
E2 8 0 VALUE={V(4)*RCOLD}
R2 8 0 1
E3 10 0 7 9 10MEG
R3 10 0 1
E4 9 0 VALUE={V(8)*V(10)}
R4 9 0 1
GR 1 3 10 2 1
VML 3 2 0
.ENDS LAMP

(If replying by E-mail please observe obscure method of anti-spam.)

For proper E-mail replies SWAP "-" and "_".

Kevin Aylward

unread,

May 28, 2001, 6:18:12 PM5/28/01

to

"Jim_Thompson" <Jim-T@analog_innovations.com> wrote in message
news:1nf5htsrg3t1k70rn...@4ax.com...

> On Mon, 28 May 2001 22:41:31 +0200, "Günter R" <gu...@web.de> wrote:
>
> |has someone got a spice model for an incandescent lamp
> |i.e. 100 W/230 V?
> |

>

But most other Spices out there are of course, Spice3 or XSpice, which dont
really need/use the poly() statement.

so,

E4 9 0 VALUE={V(8)*V(10)} should be converted to

B4 9 0 V=V(8)*V(10)

i.e. change the E source to a B source
Remove the {}
change VALUE to V.

--
Kevin Aylward , Warden of the Kings Ale
ke...@anasoft.co.uk
http://www.anasoft.co.uk - SuperSpice "Cheap, No Shit!",
GUI xspice, an affordable unlimited component, mixed-mode Windows simulator
with Schematic Capture, waveform display, FFT's and Filter Design.
Opinions of my employer are not necessarily indicative of my own
Oscillators don't, amplifiers do"

Jim_Thompson

unread,

May 29, 2001, 3:23:35 PM5/29/01

to

On Mon, 28 May 2001 22:18:12 GMT, "Kevin Aylward"
<kevinan...@home.com> wrote:

|"Jim_Thompson" <Jim-T@analog_innovations.com> wrote in message
|news:1nf5htsrg3t1k70rn...@4ax.com...
|> On Mon, 28 May 2001 22:41:31 +0200, "Günter R" <gu...@web.de> wrote:
|>
|> |has someone got a spice model for an incandescent lamp
|> |i.e. 100 W/230 V?
|> |
|

|> Here's one that works with PSpice. You may need to convert it to
|> "poly" notation to get it to work with other "Spices".
|>

|> *VO=NOMINAL OPERATING VOLTAGE
|> *IO=NOMINAL STEADY STATE OPERATING CURRENT

[snip]

|> E4 9 0 VALUE={V(8)*V(10)}
|> R4 9 0 1
|> GR 1 3 10 2 1
|> VML 3 2 0
|> .ENDS LAMP
|>
|

|But most other Spices out there are of course, Spice3 or XSpice, which dont
|really need/use the poly() statement.
|
|so,
|
|E4 9 0 VALUE={V(8)*V(10)} should be converted to
|
|B4 9 0 V=V(8)*V(10)
|
|i.e. change the E source to a B source
|Remove the {}
|change VALUE to V.

Hmmm? In PSpice, device "B" is a GaAsFet, so be cautious as to what
flavors of Spice you apply Kevin's suggestion.