HSPICE to PSPICE Conversion

[Gish]

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

 

[Chaos Master]

19 Feb 2005 12:41:24 -0800: Gish (----> [email protected]) ---->
sci.electronics.cad @

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

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

[]s
--
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!)

 

[Gish]

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

 

[Chaos Master]

19 Feb 2005 20:25:20 -0800: Gish (----> [email protected]) ---->
sci.electronics.cad @

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?

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

[]s
--
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!)

For spammers: [email protected] , or [email protected] .
Those await for your spams!

 

[Jim Thompson]

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

[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

 

[Jim Thompson]

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

[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

 

[Chaos Master]

Sun, 20 Feb 2005 10:40:10 -0700: Jim Thompson (---->
[email protected]) ----> sci.electronics.cad @

(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
--
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!)

For spammers: [email protected] , or [email protected] .
Those await for your spams!