LTSpice Math Ops?

[George Steber]

Hi,,

I admit I don't use LTS much but wanted to try the wav file input
feature not available in PSpice student version and try some signal
processing.. But I couldn't find the comparable math blocks like
"integrator", "multiplier" in LTSpice as they are in PSpice. I could
probably cobble something together using Laplace E block. Am I missing
something here with LTSpice and math operations?

George

PS. Yes, I downloaded the latest LTSpice today.

 

[Helmut Sennewald]

Hi,,

I admit I don't use LTS much but wanted to try the wav file input
feature not available in PSpice student version and try some signal
processing.. But I couldn't find the comparable math blocks like
"integrator", "multiplier" in LTSpice as they are in PSpice. I could
probably cobble something together using Laplace E block. Am I missing
something here with LTSpice and math operations?

Hello George
I also don't know why these functions are not documented in the help pages.
The function sdt() or the equivalent idt() are for integration and
ddt() is for the derivative.
These functions can be used only in a .TRAN simulation.

All the other functions are specified in
Help->LTSPICE->Circuit Elements->B. Arbitr....


V1 1 0 SINE(1 1 50)

With E-source, symbol "epoly" in folder "misc" folder

Integration
E1 n1 0 value={idt(V(1))} or E1 n1 0 value={sdt(V(1))}

*Derivative
E2 n2 0 value={ddt(V(1))}

*Multiplication
E3 n3 0 value={V(1)*V(1)}



The same with B-source, symbol "bv" in root folder

B1 n1 0 V=idt(V(1)) or B1 n1 0 V=sdt(V(1))

B2 n2 0 V=ddt(V(1))

B3 n3 0 V=V(1)*V(1)


Best Regards,
Helmut


LTSPICE news group
http://groups.yahoo.com/group/LTspice

 

[Mike Engelhardt]

George,

I admit I don't use LTS much but wanted to try the wav file input
feature not available in PSpice student version and try some signal
processing.. But I couldn't find the comparable math blocks like
"integrator", "multiplier" in LTSpice as they are in PSpice. I could
probably cobble something together using Laplace E block. Am I missing
something here with LTSpice and math operations?

For a multiplier you can use a behavioral source
and give it a value of V=V(x)*V(y), where x and y
are nodes in the circuit. The special fuction
"modulate" might also be of use. See the example
FSK modem in example/Eduational/PLL.asc. For an
integrator, you can also use the a behavioral
source but use the Verilog type functions idt()
or idtmod() in the expression. For integration,
it will understand the PSpice synonym sdt() for
idt(). FYI, there's also an independent users'
group at http://groups.yahoo.com/group/LTspice

--Mike

 

[George Steber]

Hi Mike and Helmut,

Thanks for the info. Last night I found the behavioral source (even before I
saw the email <grin>) and it works fine. I used the Laplace transform to do
integrations and some filtering Very slooooow. Took over an hour to
integrate just over a hundred msec. Finally dropped the Laplace and made my
own filters with op amps. Much much faster. I'm probably telling you
something you already know.... don't use Laplace if you can find another way
to do it!!!

Thanks for the tips on integration and differentiation. The idt() for
integration looks good but sdt() for integration is confusing as "s" normally
implies differentiation. I must say too that it would be much clearer to me
and students that are not "spice" experts to simply have the "math" blocks
available. Just MHO.

Pleased to report the wav file input works fine as a source.

George

 

[George Steber]

Mike,

Forgot to mention that I tried the Yahoo site and tried to register several
times but it wouldn't allow it. Perhaps it's just me <grin>. I guess I'll
just stay here in this group for now.

George

 

[Helmut Sennewald]

Mike,

Forgot to mention that I tried the Yahoo site and tried to register several
times but it wouldn't allow it. Perhaps it's just me <grin>. I guess I'll
just stay here in this group for now.

Hello George,
726 users have successfully become member of this group.
You are one of the first who has a problem.
I simply made a Yahoo e-mail account when I registered myself.
Maybe that helps.


Best Regards,
Helmut

 

[Helmut Sennewald]

Hi Mike and Helmut,

Thanks for the info. Last night I found the behavioral source (even before I
saw the email <grin>) and it works fine. I used the Laplace transform to do
integrations and some filtering Very slooooow. Took over an hour to
integrate just over a hundred msec. Finally dropped the Laplace and made my
own filters with op amps. Much much faster. I'm probably telling you
something you already know.... don't use Laplace if you can find another way
to do it!!!

Hello George,
what Laplace functions have you used?
There is a pitfall with high pass functions. The Laplace in (LT-)SPICE
requires that H(s) is 0 for s->infinity.

Thanks for the tips on integration and differentiation. The idt() for
integration looks good but sdt() for integration is confusing as "s" normally
implies differentiation. I must say too that it would be much clearer to me
and students that are not "spice" experts to simply have the "math" blocks
available. Just MHO.

It's just a few symbols. You could make a nice set of symbols for all users
and upload it to the LTSPICE group. They should look compatible to the
symbols used in general Control Loop Software.

Best Regards,
Helmut

 

[George Steber]

Hi Helmut,

Regarding the Laplace functions I used, they were basically low pass functions
like k/(s+a) and they worked well but very slowly. You can't make an integrator
this way ( like k/s) since spice has a problem with it. By letting "a" get small
you could approximate one to a good degree if desired. Because of speed problems
though I don't recommend using it. Thanks for your help.

George