• Welcome to our site! Electro Tech is an online community (with over 170,000 members) who enjoy talking about and building electronic circuits, projects and gadgets. To participate you need to register. Registration is free. Click here to register now.

equivalent in LTspice for PSpice/Probe command "search forward level (...)"

Thread starter #1
In the past, I used the Probe command "search forward level (...)" or in short form sfle(..) very frequently when checking simulation results from PSpice.
I am looking for something similar in LTspice. Until now, I only found out I could put cursors on the traces and then try manually to bring them to the intended point in the graph, which is quite cumbersome and not very precise. Can anyone here tell me how to accomplish this in LTspice the right way?

thanks in advance
Hugo
 

alec_t

Well-Known Member
Most Helpful Member
#2
Welcome to ETO!
Perhaps the .MEASURE command would meet your needs.
 
Thread starter #3
Thanks for the reply. I tried out your suggestion simulating a simple RC low passfilter (R=15k, C=2.2nF, VIN AC 1) .ac dec 20 100 1MEG and the following .measure statement: .MEAS AC BW when V(out)=1/sqrt(2) for checking the bandwidth of it (theoretically it should be 4822.9kHz)
To my surprise the result LTspice gave me was 3104.33Hz! If I use PSpice with the same .ac statement and use sfle(-3) on vdb(out), I get 4811.3kHz of with
sfle(0.707106781) on V(out) I get 4826.3k, which both seem acceptable results, given the 20 points per decade. Why does LTspice not give me a similar result?

thanks in advance
Hugo
 
Thread starter #4
Thanks for the reply. I tried out your suggestion simulating a simple RC low passfilter (R=15k, C=2.2nF, VIN AC 1) .ac dec 20 100 1MEG and the following .measure statement: .MEAS AC BW when V(out)=1/sqrt(2) for checking the bandwidth of it (theoretically it should be 4822.9kHz)

To my surprise the result LTspice gave me was 3104.33Hz! If I use PSpice with the same .ac statement and use sfle(-3) on vdb(out), I get 4811.3kHz, with
sfle(0.707106781) on V(out) I get 4826.3k, which both are acceptable results, given the 20 points per decade. Why does LTspice not give me a similar result?

I found out the reason for this strange result. The .measure statement should be .MEAS AC BW when mag(V(out))=1/sqrt(2)
The reason why I did not do it like that the first time is the misleading example information on " twiki.org/LTspiceHelp/LTspiceHelp/_MEASURE_Evaluate_User_Defined_Electrical_Quantities.htm", there it is stated:

.MEAS AC rel8 when V(out)=1/sqrt(2)
The result rel8 is the frequency that the magnitude of V(out) is equal to 0.7071067811865475.

Anyway, I can make it work now as it should but I think it is rather cumbersome and it is also a pity the vdb(x) syntax is not recognized

Hugo
 
Last edited:

alec_t

Well-Known Member
Most Helpful Member
#5
Glad you got it working.
 

MikeMl

Well-Known Member
Most Helpful Member
#6
Did you remember to suppress the data compression on the LTSpice output file? The default is that the output file is radically compressed to save disk space. You need to do the .Measure on an uncompressed output.
 
Thread starter #7
Did you remember to suppress the data compression on the LTSpice output file? The default is that the output file is radically compressed to save disk space. You need to do the .Measure on an uncompressed output.
I guess you mean by that adding ".options plotwinsize=0" to the schematic? I tried it out with and without and it makes no difference for the measure-result in this case. Is compressing the output file still the default action in LTspice these days (I think it shouldn't be the default)?

kind regards,
Hugo
 
Last edited:

Latest threads

EE World Online Articles

Loading

 
Top