stuck with table syntax (ltspice)

S

s.d.

Guest
Hello,

I am stuck with table syntax.
I intend to make a step variable frequency, function of time

What's wrong with my approach, how can I fix it?

thanks

d.

WARNING: Can't resolve .param ko=table(time,0, 0,10e-3,0.5,20e-3,1.0)
Questionable use of curly braces in "b2 n003 0 v={ko}"
error: Error: yet unevaluated parameter in: "[ko]"
Circuit: * D:\nour\pll\pll1.asc

Fatal Error: B2: -- Syntax Error --
Unknown symbol: ko


* D:\nour\pll\pll1.asc
A1 N002 N001 0 0 0 0 OUT 0 PHASEDET
V1 N001 0 PULSE(0 1 0.2E-3 0 0 0.5E-3 1E-3)
A2 N003 0 0 0 0 0 b 0 MODULATOR mark=0.5 space=1.5k
B1 N002 0 V=0.5*(sgn(v(B))+1)
B2 N003 0 V=Ko
R1 0 OUT 10k
..tran 5E-2
..param Ko table(time,0, 0,10e-3,0.5,20e-3,1.0)
..backanno
..end

Version 4
SHEET 1 892 692
WIRE 496 304 512 304
WIRE 368 368 368 352
WIRE 368 320 240 320
WIRE 240 320 240 336
WIRE 240 432 240 416
WIRE 368 288 112 288
WIRE 112 384 112 368
WIRE 480 64 560 64
WIRE 336 32 160 32
WIRE 160 32 160 48
WIRE 160 144 160 128
WIRE 336 128 336 144
WIRE 336 128 304 128
WIRE 304 128 304 96
WIRE 304 96 336 96
WIRE 512 304 512 288
WIRE 512 304 528 304
WIRE 512 192 512 208
FLAG 368 368 0
FLAG 528 304 OUT
FLAG 240 432 0
FLAG 112 384 0
FLAG 160 144 0
FLAG 560 64 b
FLAG 336 144 0
FLAG 512 192 0
SYMBOL Digital\\phidet 400 304 R0
SYMATTR InstName A1
SYMBOL voltage 240 320 R0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
SYMATTR InstName V1
SYMATTR Value PULSE(0 1 0.2E-3 0 0 0.5E-3 1E-3)
SYMBOL SpecialFunctions\\modulate 336 32 R0
WINDOW 3 41 120 Left 0
SYMATTR Value mark=0.5 space=1.5k
SYMATTR InstName A2
SYMBOL bv 112 272 R0
WINDOW 0 -64 24 Left 0
WINDOW 3 -58 -14 Left 0
SYMATTR InstName B1
SYMATTR Value V=0.5*(sgn(v(B))+1)
SYMBOL bv 160 32 R0
SYMATTR InstName B2
SYMATTR Value V=Ko
SYMBOL res 496 192 R0
SYMATTR InstName R1
SYMATTR Value 10k
TEXT -470 136 Left 0 !.tran 5E-2
TEXT -488 64 Left 0 !.param Ko table(time,0, 0,10e-3,0.5,20e-3,1.0)
 
On Wed, 07 Jul 2004 15:21:56 +0200, "s.d." <szymik@NOSPAM.univ-lille1.fr> wrote:

Hello,

I am stuck with table syntax.
I intend to make a step variable frequency, function of time

What's wrong with my approach, how can I fix it?

thanks

You must read LTspice help file.
Click to expand...

Damir
 
"s.d." wrote:

I am stuck with table syntax.
I intend to make a step variable frequency, function of time

What's wrong with my approach, how can I fix it?
Click to expand...
LTspice must be able to resolve parameters to one numeric value
before running the simulation. A careful reading of the warnings
and error message reveals that Ko is unresolvable (because "time"
does not have a specific value) which, in turn, leads to fatal
problems with B2.

WARNING: Can't resolve .param ko=table(time,0,0,10e-3,0.5,20e-3,1.0)
....
Error: yet unevaluated parameter in: "[ko]"
....
Fatal Error: B2: -- Syntax Error -- Unknown symbol: ko
....
B2 N003 0 V=Ko
....
.param Ko table(time,0,0,10e-3,0.5,20e-3,1.0)
Click to expand...
"Time" may not be used within an expression for a parameter, but
it is perfectly acceptable directly within a value expression for a
B-source. Your simulation should run fine if your move the table
expression directly over to the B-source in place of "Ko" (and
delete the .param statement).

B2 N003 0 V=table(time,0,0,10e-3,0.5,20e-3,1.0)

Good luck. -- analog
 
Mike Engelhardt a écrit :

Use


B2 N003 0 V=table(time,0, 0,10e-3,0.5,20e-3,1.0)


Alternatively, you can use this syntax:


B2 N003 0 V=Ko()
.func Ko() = { table(time,0, 0,10e-3,0.5,20e-3,1.0)}
Click to expand...
Thanks a lot

d.
 
You must log in or register to reply here.

Welcome to EDABoard.com

Sponsor

Back
Top