--- In LTspice@yahoogroups.com, Peter Erasmus <wenkoswissauto@y...>
> wrote:
>
> Hallo Helmut.
> I am sorry to ask so many questions.
> the four symbols should I install them in the Lib file for LT

Hello Peter,

There is no need to install any symbol. I recommend to save
the required symbol in the the schematic folder.
You also save your ".lib"-file from FilterLab and the opamp
model file into this directory.

Example:

1.
You make a new design let's say a 3-pole MFB(Multi FeedBack)
lowpass filter. You have named this design "mfb_3pole_1khz_hp".

2.
Filterlab can generate a Spice netlist file with a ".lib"
extension. It will automatically name this netlist file
"mfb_3pole_1khz_hp.lib".

3.
Copy this "mfb_3pole_1khz_hp.lib" and the symbol file
"hp_block.asy" into your working directory. Also copy your
real opamp model file into this directory.

4.
Add an instance of this HighPass-symbol onto your schematic.
Change the value "HP" on this symbol to "mfb_3pole_1khz_hp" .
This name has to be the name of your subcircuit generated by
Filterlab. It's in the file "mfb_3pole_1khz_hp.lib" and looks
like
.subckt mfb_3pole_1khz_hp .....

5.
Take a text editor and replace the "MCPxxxx" in the subcircuit
file "mfb_3pole_1khz_hp.lib" with the name of your real opamp model.

X1 ..... MCPxxxx
-->
X1 ..... TL072A

6.
I assume now that the TL072A model is in the file TI.lib.
Add a SPICE-line at the beginning of "mfb_3pole_1khz_hp.lib"
to include the model file for the opamp.
.include TI.lib



Btw, this is all pure SPICE. It's just about the syntax of the
".subckt ..." and the ".include" comamnd.

7.
Finally you should have the following files in your working
directory.

my_schematic.asc
hp_block.asy
mfb_3pole_1khz_hp.lib
TI.lib

Best regards,
Helmut
