a question about PSPICE multiple variables simulation

Use a single parameter, say .PARAM Counter = 1, then step it to N in increments of 1.

Express your register and potentiometer as TABLE functions of "Counter"

THIS IS A MAJOR FLAW IN PSPICE, Charlie!!

...Jim Thompson

Hi,

I have to learn a new software....:( I also want to use ORCAD optimizer function to get better performance. Dear Jim, could you please write a simple code for me to follow? e.g. two pots in a closed-loop circuit. Thank you in advance.

I know they upgrade pSpice with a "parametric plotter" in ver. 10.X, but mine is v9.2.

thanksthanks t t t h h h h h a athanksa a a n n n n k k k k k s s s s s

Kev> > > >

Well, if he needed to have these guys vary independently, then he can use Advanced Analysis, and do a multi-parameter simulation. (I know you haven't played with this, Jim, since it is sorta hard to do from Schematics. There have to be a FEW advantages for using Capture and Concept... 8-) ) However, in this case, they need to be linked, since the pot value and the register value are linked, so he needs to just have a defined relationship. I have often had a single parameter defined in a PARAM, and have the second defined as an expression. Since this is a register/counter/pot relationship, this implies an analog to digital conversion, tricky in an expression. I would probably build in a circuit to do the ADC for me, or DAC if setting the register made more sense.

Charlie

That's why I suggested TABLE... avoids an expression between parameters, but I've resorted to that way as well :-(

...Jim Thompson

I only design microchips so I don't use optimizer, though I use sensitivity analysis occasionally.

...Jim Thompson

Indeed. It gives me the opportunity to point out that in SuperSpice you can go:

R1: 10k 3k 8k C2: 1n 2n 5n 6n L1: 5u 7u 10u

and SS will run every combination of all the values and plot them all in one go!

Kevin Aylward snipped-for-privacy@anasoft.co.uk

Werll, heres an A/D

..SUBCKT Analog8BitAtoD_XN _ssi_pin_d8 _ssi_pin_d7 _ssi_pin_d6 _ssi_pin_d5 _ssi_pin_d4 _ssi_pin_d3 _ssi_pin_d2 _ssi_pin_d1 ain_p _ssi_pin_aref _ssi_pin_dref

• _SS_Symbol [C:\Program Files\AnaSoft\SuperSpice\system\MixedMode.ssm] [Analog8BitAtoD]

• d0 is lsb. aref is the +/-vin range. dref is the digital output level e.g. 5V supplies
• output and input is referanced to 0V.
• boffset ain 0 v=v(ain_p)/2 + v(_ssi_pin_aref)/2
• b1 _ssi_pin_d1 0 v=u(v(ain) - v(_ssi_pin_aref)/2 ) * v(_ssi_pin_dref) b2p 2p 0 v=v(ain) - v(_ssi_pin_d1) *v(_ssi_pin_aref)/v(_ssi_pin_dref)/2
• b2 _ssi_pin_d2 0 v=u( v(2p ) - v(_ssi_pin_aref)/4)*v(_ssi_pin_dref) b3p 3p 0 v=v(2p) - v(_ssi_pin_d2) *v(_ssi_pin_aref)/v(_ssi_pin_dref)/4
• b3 _ssi_pin_d3 0 v=u( v(3p ) - v(_ssi_pin_aref)/8)*v(_ssi_pin_dref) b4p 4p 0 v=v(3p) - v(_ssi_pin_d3) *v(_ssi_pin_aref)/v(_ssi_pin_dref)/8
• b4 _ssi_pin_d4 0 v=u( v(4p ) - v(_ssi_pin_aref)/16)*v(_ssi_pin_dref) b5p 5p 0 v=v(4p) - v(_ssi_pin_d4) *v(_ssi_pin_aref)/v(_ssi_pin_dref)/16
• b5 _ssi_pin_d5 0 v=u( v(5p ) - v(_ssi_pin_aref)/32)*v(_ssi_pin_dref) b6p 6p 0 v=v(5p) - v(_ssi_pin_d5) *v(_ssi_pin_aref)/v(_ssi_pin_dref)/32
• b6 _ssi_pin_d6 0 v=u( v(6p ) - v(_ssi_pin_aref)/64)*v(_ssi_pin_dref) b7p 7p 0 v=v(6p) - v(_ssi_pin_d6) *v(_ssi_pin_aref)/v(_ssi_pin_dref)/64 b7 _ssi_pin_d7 0 v=u( v(7p ) - v(_ssi_pin_aref)/128)*v(_ssi_pin_dref) b8p 8p 0 v=v(7p) - v(_ssi_pin_d7)

• b8 _ssi_pin_d8 0 v=u( v(8p ) - v(_ssi_pin_aref)/256)*v(_ssi_pin_dref)
• ..ends

Its a successive approximation without a clock.!

Tyhee is a working example in SS.

and the D/A

..SUBCKT Analog8BitDtoA_XN _ssi_pin_d0 _ssi_pin_d1 _ssi_pin_d2 _ssi_pin_d3 _ssi_pin_d4 _ssi_pin_d5 _ssi_pin_d6 _ssi_pin_d7 aout _ssi_pin_aref _ssi_pin_dref

• _SS_Symbol [C:\Program Files\AnaSoft\SuperSpice\system\MixedMode.ssm] [Analog8BitDtoA]

• d0 is lsb. aref is the +/-vout range. dref is the digital switch point, e.g. 2.5 on 5V supplies
• output and input is referanced to 0V.
• The 1/512 is 1/2 lsb offset to provide for symetrical swings etc...
• b1 aout 0 v= 2*v(_ssi_pin_aref) *
• ( (u( v(_ssi_pin_d0) - v(_ssi_pin_dref)) + u( v(_ssi_pin_d1) - v(_ssi_pin_dref))*2 + u( v(_ssi_pin_d2) - v(_ssi_pin_dref))*4 + u( v(_ssi_pin_d3) - v(_ssi_pin_dref))*8
• + u( v(_ssi_pin_d4) - v(_ssi_pin_dref))*16 + u( v(_ssi_pin_d5) - v(_ssi_pin_dref))*32 + u( v(_ssi_pin_d6) - v(_ssi_pin_dref))*64 + u( v(_ssi_pin_d7) - v(_ssi_pin_dref))*128
• ) /256 - 0.5 + 1/512) ..ends

Kevin Aylward snipped-for-privacy@anasoft.co.uk

there is no such a "look-up table" in ORCAD pspice A/D 9.2. I've spent three days on studing advanced simulation by pspice and draw a conclusion:

....write two sub circuit files and define the two registers as two function of a parameter, e.g. a counter N, respectively, then do simulation. this is silly 'coz I must solve the LMS interpolation to find coefficients of equations by using somekind of maths software package. e.g. IDL, Matlab. then go back to ORCAD.

The ORCAD optimizer is garbage, don't try to learn, it'll waste your time.

okey, it's concluded.

What are you running on, a contraband copy? You'll find Etable, Gtable and just plain "Table" in the PSpice Users Guide.

That's alright, optimizers are for amateurs ;-)

...Jim Thompson

I READ GTABLE/ETABLE BUT I DON'T KNOW HOW TO PLAY IT.

I RUN SVBKSB (I.E. singular value backsubstitution) UP TO 4RD ORDER TO CAL. COEFFICIENTS. IT WORKS WELL. 3RD ORDER IS ENOUGH.

IF YOU HAVE TIME, JUST SHOW US SOME EXAMPLE CODES OF HOW TO USE GTABLE/ETABLE FOR AN ANALOG REGISTER.

THANKS.

No "codes" to it, just fill in the x,y values... "x" = input, "y" = output.

And knock-off the all-caps!

...Jim Thompson