HSPICE to PSPICE Conversion

Thread view:

Enable EMail Alerts

Start New Thread

Thread rating:

Gish - 19 Feb 2005 20:41 GMT

Hi Guys

I have some SPICE code that runs perfectly in HSPICE but will not run
in PSPICE due to issues with "subcircuit expansion." If there's any
experts out there who could take a quick look at this and let me know
what the issue might be I'd appreciate it.

Thanks

******************************************************
**** circuit description
******************************************************
rs in inp 50
r1 inp vss 1K
x1 inp inm out vss my_opamp
rf out inm 100K
r2 inm vss 1K
******************************************************
**** parameters section
******************************************************
******************************************************
**** sources section
******************************************************
v1 in vss sin(0V 60mV 10x 100ps 0)
v2 vss 0 dc 0V
******************************************************
**** specify nominal temperature of circuit in degrees C
******************************************************
.TEMP= 60
******************************************************
**** analysis section
******************************************************
.tran 1ns 200ns
.END

Reply to this Message

Chaos Master - 19 Feb 2005 21:22 GMT

19 Feb 2005 12:41:24 -0800: Gish (----> andrewgish@comcast.net) ---->
sci.electronics.cad @
<1108845684.189581.57660@z14g2000cwz.googlegroups.com> :

> Hi Guys
>
[quoted text clipped - 13 lines]
> rf out inm 100K
> r2 inm vss 1K

What's the model for 'my_opamp' subcircuit (subckt)?

[]s

Signature

Chaos Master®, posting from Canoas, Rio Grande do Sul, Brazil - 29.55° S
/ 51.11° W / GMT-2h / 15m .

"People told me I can't dress like a fairy.
I say, I'm in a rock band and I can do what the hell I want!"
-- Amy Lee

(My e-mail address isn't read. Please reply to the group!)

Reply to this Message

Gish - 20 Feb 2005 04:25 GMT

Ok,

I actually figured everything out except for one line...

E1 out ref in+ in- MAX=5V MIN=-5V opamp_gain

I'm trying to code a VCVS with maximum and minimum output values, but
PSPICE rejects the MAX and MIN parts. Any ideas?

Thanks

> Hi Guys
>
[quoted text clipped - 30 lines]
> .tran 1ns 200ns
> .END

Reply to this Message

Chaos Master - 20 Feb 2005 04:29 GMT

19 Feb 2005 20:25:20 -0800: Gish (----> andrewgish@comcast.net) ---->
sci.electronics.cad @
<1108873520.072521.37120@g14g2000cwa.googlegroups.com> :

> Ok,
>
[quoted text clipped - 4 lines]
> I'm trying to code a VCVS with maximum and minimum output values, but
> PSPICE rejects the MAX and MIN parts. Any ideas?

I think that PSpice doesn't support MAX and MIN values.

[]s

Signature

Reply to this Message

Jim Thompson - 20 Feb 2005 16:57 GMT

>Ok,
>
[quoted text clipped - 15 lines]
>>
>> Thanks

[snip]

Here are a few of the operators in PSpice BEHAVIORAL elements:

LIMIT(x,min,max) result is min if x < min, max if x > max, and x
otherwise

MAX(x,y) maximum of x and y

MIN(x,y) minimum of x and y

In addition you must use the BEHAVIORAL syntax of the E-source

So the correct expression for E1 is:

E1 out ref VALUE = {LIMIT((opamp_gain*V(in+,in-)),MIN,MAX)}

.PARAM MAX=5V MIN=-5V opamp_gain=100K

(Or put the numerics directly in the expression.)

This is convergence risk using mathematical limits, since they are
hard, and derivatives don't exist at the limit points.

I prefer using the TANH expression:

E1 1 0 VALUE {(tanh(A*V(INP,INN))+1)/2}
E2 OUT 0 VALUE {V(1,0)*(VP-VN)+VN}

.PARAM A=100K ; OpAmp Gain
.PARAM VP=+5V ; Positive Limit
.PARAM VN=-5V ; Negative Limit

(Note that exact gain is an interaction between A, VP, and VN (E1
produces 0 ->1), but I'm still too sleepy this morning to make an
exact expression :)

...Jim Thompson

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

Reply to this Message

Jim Thompson - 20 Feb 2005 17:40 GMT

>Ok,
>
[quoted text clipped - 6 lines]
>
>Thanks

[snip]

Are you using PSpice "raw", i.e. without schematic capture?

Both PSpice Schematics and Capture (gag me with a spoon) have the
correct netlist TEMPLATE contained within the symbol.

(Not that I should be one to criticize. I went for MANY years drawing
schematics with pencil and paper, numbering nodes, hand-typing
netlists, and batch-loading into Berkeley Spice 2G6 on an old VAX,
IIRC, 1170. Then I discovered PC's and bought my first 386 for $6K...
cheap because it was a clone :-)

...Jim Thompson

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

Reply to this Message

Chaos Master - 20 Feb 2005 20:01 GMT

Sun, 20 Feb 2005 10:40:10 -0700: Jim Thompson (---->
thegreatone@example.com) ----> sci.electronics.cad @
<78ih11dl5n7vl7ipnvmfc19h6bm1i32d00@4ax.com> :

> (Not that I should be one to criticize. I went for MANY years drawing
> schematics with pencil and paper, numbering nodes, hand-typing
> netlists, and batch-loading into Berkeley Spice 2G6 on an old VAX,
> IIRC, 1170. Then I discovered PC's and bought my first 386 for $6K...
> cheap because it was a clone :-)

I sometimes end up doing this, even though I have 2 schematic editors
here (LTspice and SIMetrix Intro).

[]s

Signature

Reply to this Message

Electronics Forum / CAD / February 2005

HSPICE to PSPICE Conversion