开云体育

Thank you Helmut... :D

--- In LTspice@..., "kbyrne10" <kbyrne10@...> wrote:

I down loaded a OP-AMP I need to study like your TL072 verses LT1057
Folder. Question What do I have to do in PSpad and or on schematic to use the Universal Symbol "opamp2.
It states: * LF353 OPERATIONAL AMPLIFIER "MACROMODEL" SUBCIRCUIT
.SUBCKT LF353 1 2 3 4 5
Is this just a .include LF353 .SUBCKT LTspice directive on schematic.
or do I have to open a window & change parameters again and if so what should it read for a OP-Amp instead of a Zener Diode. I just need the info to store in my collection of files for all types of parts introduced into LTspice so in the future I have help all figured out
if it is not a problem in a little bit of a guide not a drawn out affair. Best wishes Kevin

Hello Kevin,

You can use the symbol opamp2, because it has the same pin-order
+in -in V+ V- out.
You will need then only an additional .include LF353.mod in
the schematic.
The value have to be LF353/NS, because it's the name in the
.subckt line.

You can look-up an example.

Files > Lib > LF353_LF412_test.zip

Best regards,
Helmut


* connections: non-inverting input
* | inverting input
* | | positive power supply
* | | | negative power supply
* | | | | output
* | | | | |
* | | | | |
.SUBCKT LF353/NS 1 2 99 50 28

I down loaded a OP-AMP I need to study like your TL072 verses LT1057
Folder. Question What do I have to do in PSpad and or on schematic to use the Universal Symbol "opamp2.
It states: * LF353 OPERATIONAL AMPLIFIER "MACROMODEL" SUBCIRCUIT
.SUBCKT LF353 1 2 3 4 5
Is this just a .include LF353 .SUBCKT LTspice directive on schematic.
or do I have to open a window & change parameters again and if so what should it read for a OP-Amp instead of a Zener Diode. I just need the info to store in my collection of files for all types of parts introduced into LTspice so in the future I have help all figured out
if it is not a problem in a little bit of a guide not a drawn out affair. Best wishes Kevin

--- In LTspice@..., "imbvlad" <imbvlad@...> wrote:

Mike,

The -nowine switch is documented in the LTspice's help manual, see Modes of Operation > Command Line Switches:

"Prevent use of WINE(Linux) workarounds."

[...]

Good luck understanding,
Vlad :)

Thanks Vlad. That was a very good explanation. I'm running Ubuntu 10.04.02 LTS, but I never had any display problems or found a need to use the command line switches.

Most of the time I run LTspice in VirtualBox in WinXP SP3, and once in a while the cursor gets screwed up and blinks furiously. I simply press Esc and that stops it. I haven't found any other problems.

I believe LTspice is by far the most reliable code I have ever seen for XP or Ubuntu. I don't know how Mike can be such an expert in so many different fields - SPICE, Windows programming, electronics, and convincing the management at Linear to let him create the best SPICE program on the planet. It's just amazing.

Thanks,

Mike

--- In LTspice@..., "Tony Casey" <tony@...> wrote:

--- In LTspice@..., "Majid" <rafei.majid@> wrote:

Dear Helmut,
Do you know what is the correct syntax of network parameters for measuring purposes? (Z(11) or Z11 or ...?), Thanks.

Hello Majid,

The syntax is exactly the same as you would use in the waveform window, so I would develop the .meas statements in conjunction with plots of the data you're interested in, even if in the end you want to only use the command line (batch mode).

So, for example, if you're plotting Z11(V1) (assuming V1 is the source you're using), you would add the statements like:

.meas AC Z11-200M Z11(V1) at 200Meg; Z11 at 200MHz
.meas AC Z11-300M Z11(V1) at 300Meg; Z11 at 300MHz

...etc

You cannot save an array of measurements, unfortunately, so you will need a .meas statement for each frequency of each parameter you want to save. If there are a lot, it might be better to put all the .meas statements into an .included file to save cluttering up your schematic.

You can find all the information on syntax, surprisingly enough, in the Helpfile.

Regards,
Tony

Hello Tony,

Thanks for your explanation. I thought to complicated when I
advised to open the raw-file. Just looking in the "Add trace"
dialog as you have advised is a lot more convenient.

Best regards,
Helmut

Hi Tony,

You cannot save an array of measurements, unfortunately, so you will
need a .meas statement for each frequency of each parameter you want
to save. If there are a lot, it might be better to put all the .meas
statements into an .included file to save cluttering up your
schematic.

I'm not sure if that is totally true - depending on what you define
as 'an array of measurements' :)

You can use a .step statement and then extract the step details from
the .raw file. I wrote examples for .tran and .ac analysis here:



I mention this in case its a method you have not tried before.

Cheers,
Dave

--- In LTspice@..., "Majid" <rafei.majid@...> wrote:

Dear Helmut,
Do you know what is the correct syntax of network parameters for measuring purposes? (Z(11) or Z11 or ...?), Thanks.

Hello Majid,

The syntax is exactly the same as you would use in the waveform window, so I would develop the .meas statements in conjunction with plots of the data you're interested in, even if in the end you want to only use the command line (batch mode).

So, for example, if you're plotting Z11(V1) (assuming V1 is the source you're using), you would add the statements like:

.meas AC Z11-200M Z11(V1) at 200Meg; Z11 at 200MHz
.meas AC Z11-300M Z11(V1) at 300Meg; Z11 at 300MHz

...etc

You cannot save an array of measurements, unfortunately, so you will need a .meas statement for each frequency of each parameter you want to save. If there are a lot, it might be better to put all the .meas statements into an .included file to save cluttering up your schematic.

You can find all the information on syntax, surprisingly enough, in the Helpfile.

Regards,
Tony

--- In LTspice@..., "Majid" <rafei.majid@...> wrote:

Dear Helmut,
Do you know what is the correct syntax of network parameters for measuring purposes? (Z(11) or Z11 or ...?), Thanks.

Hello Majid,

Take a powerful text editor (PSPAD) and open the raw-file to get
an idea how LTspice has saved Z() or S() in the raw-file.
Try this with the example "s-param.asc" from the installation
folder LTC&#92;LTSPICEIV&#92;Examples&#92;Educational. You will see this
at the beginning of the raw-file.

72 Zout(v4) impedance
73 Yout(v4) conductance
74 Zin(v4) impedance
75 Yin(v4) conductance
76 S11(v2) S-parameter
77 S21(v2) S-parameter
78 S12(v2) S-parameter
79 S22(v2) S-parameter
80 Z11(v2) impedance

A measure command could look like below.

.measure V5o Find S11(V4) at 250meg

The result in the log-file is shown below.

v5o: s11(v4)=(-12.825dB,-68.8726°) at 2.5e+008


Best regards,
Helmut

--- In LTspice@..., "Basier philippe" <basier.philippe@...> wrote:

Hello all of you,
I download:
NE555 (Tansistor leveltimer.asc from Files&#92;Files sorted by message&#92;msg_31483 ( NE555 transistorlevel/leveltimmmer.asc }
Why is V( out) or V(OUput) are going in strange frequencies ?
Thanks
Best regards
Philippe B.

Hello Philippe,

I guess the circuit for the NE555 in his schematic has a mistake.

Best regards,
Helmut

Oooh I'm sorry. I made a misreading

--- In LTspice@..., "Shadow" <shadowvpr123@...> wrote:

I also need an op27 op amp.. sorry for the double post...
thank you..

Hello,

I have uploaded two examples. Both use the symbol "opamp2" from
[Opamp].

Files > Lib > OP27_test.zip

Files > Lib > OPA27_test.zip

Please be aware that the OP27 and OPA27 are different opamps.

Best regards,
Helmut

Dear Helmut,
Do you know what is the correct syntax of network parameters for measuring purposes? (Z(11) or Z11 or ...?), Thanks.

I tried Z11 and Z(11), but for both of them the result of measurement was FAIL'ed !

It seems very great, but I dont know the syntax for measuring the network parameters! (Z(11) or Z11 or ...)

--- In LTspice@..., "Majid" <rafei.majid@...> wrote:

Deer Helmut.
Yes, you are right, but I want not to work with waveform viewer,I work in command window, so, just working with commands. Thanks again.

Hello,

If you have .measure commands in your schematic or your netlist,
you will have their results in the log-file.

Best regards,
Helmut

Deer Helmut.
Yes, you are right, but I want not to work with waveform viewer,I work in command window, so, just working with commands. Thanks again.

--- In LTspice@..., Majid Rafei <rafei.majid@...> wrote:

Your are right, but i am looking toward extracting the results from a text
file which is directly obtained by executing scad3.exe from the command
window! I mean, I want to bypass the waveform window!

Hello,

Ltspice writes a file named design_name.txt when you export.
Please do exactly what I said in my last email.

Files -> Export

Best regards,
Helmut

Thanks in real, of you and also of the others for your and their guidance.

Thanks a lot, so, you say that the results of .Net analysis are adequately accompany the *.raw file? Am I right?
(I am wondered that when I change output format to ascii, there is no network analysis data!)

I have not performed a .net analysis, but whatever LTspice saves
to display in the waveform window goes into the .raw file, so
I assume that the .raw file contains the information you want.
I leave it up to you to investigate :)

Cheers,
Dave

Thanks a lot, so, you say that the results of .Net analysis are adequately accompany the *.raw file? Am I right?
(I am wondered that when I change output format to ascii, there is no network analysis data!)