开云体育

b) Why does the amplitude of the output in the transient analysis not
coincide with the magnitude in the Bode plot at 200 khz (452 mV vs. 7.5 mV
or 643 mV)?

You also need to realize that an .AC analysis is a small-signal linearized
analysis. The multiplier, which is an inherently nonlinear device, is
presumably linearized at the operating point, and treated as a linear gain
block.

Thus, if you were to input (say) 100 kHz to both input ports (as you have),
you would not find any 200 kHz on the output ... and LTspice would not plot
the amplitude of the 200 kHz (that this chip actually outputs) ... because
an .AC analysis does not generate sum-and-difference frequencies. If
anything, it will only tell you how much of the 100 kHz goes through
because of leakage/imbalance, and because of the fact that the other port's
bias voltage was not 0.0V.

One might even question if you can do an .AC analysis at all. Whether you
get anything meaningful, depends on what's inside the model for this part.
Depending on how they modeled it, it might work correctly in a .TRANsient
analysis, but not in an .AC analysis. I'm just sayin'.

Regards,
Andy

FYI ... after running an AC analysis, if you hover the mouse pointer over
any net, look in the lower left corner where LTspice will tell you the DC
operating point voltage on that net.

Andy

Maren (distheo@...) wrote:

a) Why is the .ac simulation influenced at all by the parameters of the

transient simulation?

In an .ac analysis, LTspice first needs to find the operating point. All
voltage and current sources are set to their values at t=0.

Since you specified a SINE source with a phase shift of 45 degrees, the t=0
value is 0.707* 3.0 = 2.12132V.

Regards,
Andy

Thank you for the options suggested.Could you give an idea how to
implement 1 sec delay using B-element.

The idea I will give you is to open Help in LTspice; Then go to LTspice >
Circuit Elements > B. Arbitrary Behavioral Voltage or Current Sources.
Scroll down and find the first table of functions.

Andy

Macy wrote:

I like the idea of 'including' the file with everything in it then I can

modify and control a bit better, BUT that separates the design into two
pieces, which may, or may not, be kept together. I know, I know sloppy
paperwork, but still something always happens and I'm not absolutely
certain that x1 schematic was used with x1 text file.

Well, you've got a choice. You can either (1) keep everything on the
schematic, or (2) move stuff off the schematic into a separate file. Pick
one approach or the other, and live with it. You can't do neither.

With it on the schematic, obviously, if you have a lot of text, it's going
to take up a lot of schematic space which shrinks the full view.

With it off the schematic, obviously, you have to deal with two or more
files. Create a new project folder for each schematic, and then you are
less likely to lose track of the second file.

The stuff on the schematic (or in a text file) doesn't need to be one long
line. Break it into shorter lines, with a "+" as the first character on
all lines after the first. If you stick with approach (1), that might make
it not quite so huge.

.ac LIST freq freq freq ...
+ more freqs freq freq ...
+ more freqs freq freq ...
etc....

When entering or editing the .ac or .noise lines on the schematic, be sure
to use the Ctrl-M trick to insert line breaks. You need those lines to be
kept together as one unit, not as independent SPICE directives.

You might also go into the LTspice Control Panel and change the font size.
This affects all text on the schematic (and all LTspice schematics you
edit), and it has a limited range so it might not make enough of a
difference.

Andy

On 7/15/2013 5:43 AM, feabyl wrote:

What is the equation for behavioral source with 1 sec delay?

_

Look up the behavioral B source function, absdelay( x, t [, tnax] ) in
the LTspice Help File.

Howard

Hi Macy,

To bounce between analyses I tried the right click on the comment,
convert to spice command, which works, but CANNOT UNDO THAT! I had to
ctrl-c the line and put it back as a comment, and then scissor cut
the spice command to change the spice command.

If the SPICE directive is something like .step or .param, you can
just right click. If the SPICE directive is something that the
simulation GUI normally deals with, then the GUI pops up, unless
*you press ctrl* and right-click :)

I also tried a trick I used to do on the old version of LTspice - put
an asterisk on the start of the spice command line to 'turn it off',
but that no longer works. Mike, perhaps in the next wish list put in
an easy way to toggle between spice and comment lines.

No need to, it already exists.

I like the idea of 'including' the file with everything in it then I
can modify and control a bit better, BUT that separates the design
into two pieces, which may, or may not, be kept together. I know, I
know sloppy paperwork, but still something always happens and I'm not
absolutely certain that x1 schematic was used with x1 text file.

C'mon man, surely you have created designs with hundreds of files.
What do you do when you layout your PCB, you've got a schematic,
a PCB file, a zillion symbols, etc.?

Just use two files. You've got a design that consists of graphics
and text, just put the text in a text file :)

Cheers,
Dave

now there are 'comments' on the schematic
.ac dec 500 10 100k
.noise V(out) Vsource dec 500 10 100k
.ac LIST this goes forevers.....
.noise V(out) Vsource LIST ditto.....
[Thanks for suggesting LIST. It also works in the noise analysis.]

The last two are so long that when I open the schematic I get almost NOTHING on the screen - a bit of blue smidgeon on the left and tiny little blue dots going across the page. At first, I thought LTspice broken. So I have to do the + circle about where I think the schematic is located, and voila! I get enough I can see it to position a bit better.

To bounce between analyses I tried the right click on the comment, convert to spice command, which works, but CANNOT UNDO THAT! I had to ctrl-c the line and put it back as a comment, and then scissor cut the spice command to change the spice command.

I also tried a trick I used to do on the old version of LTspice - put an asterisk on the start of the spice command line to 'turn it off', but that no longer works. Mike, perhaps in the next wish list put in an easy way to toggle between spice and comment lines.

I like the idea of 'including' the file with everything in it then I can modify and control a bit better, BUT that separates the design into two pieces, which may, or may not, be kept together. I know, I know sloppy paperwork, but still something always happens and I'm not absolutely certain that x1 schematic was used with x1 text file.


Thus, as you can see, there is a way to get around on this thing, but is there an easier way?



--- dwh@... wrote:

From: David Hawkins <dwh@...>
To: LTspice@...
Cc: Macy <macy@...>
Subject: Re: [LTspice] Re: Help! How do I do find maximum signal easily!
Date: Fri, 12 Jul 2013 16:07:44 -0700

[snip] and the .ac using specific values requires storing on the
schematic a list so long that it makes the schematic the size of a
postage stamp in auto size. perhaps a plus sign on the first of a few
lines will allow wordwrap - narrow width with long list.

Why not put all the relevant text into file, and then .include it.
It makes the schematic look nicer, and allows you to add
header comments to the file along with relevant comments
throughout the file.

Cheers,
Dave

Yes, all the files are in the location you mention. I will copy everything to a desktop folder and then see if I can copy that. Thanks!

RL,

Thank you for taking a look but I still have an issue. The bridge nodes that you renamed now disconnected the ZVS circuit of the chip because the nodes have been renamed to SWAB and SWCD the SWT and SWB nodes are no longer connected and are left floating.

Also when the when the input power supply drops to 18V the regulation of the 165V rail is not kept.

I would also appreciate it if you could tell me how you came to derive all of the compensation values.

Thanks for your help.

Leo

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

What is the equation for behavioral source with 1 sec delay?

feabyl,

Have you even thought of looking in the LTspice help file?

Rick

What is the equation for behavioral source with 1 sec delay?

Dear subscribers of the LTSpice-List,

I uploaded the concerned Schematic and the model of AD734 to

(files->temp->AD734 4 Quadrants Multiplier)

I am not sure, if my problem is actually related to my schematic or the model or if it is rather an LTSpice-operator problem (i.e. me).
Here it comes:

I run the transient analysis with 100 kHz sine waves on both inputs which converges thanks to the .options that I found in AD734_test.asc in the "files->lib->ad734" folder. The resulting waveform is a sine with 452 mV amplitude, 200 kHz, offset about 400 mV. Fine so far. I can play with phases between the inputs etc. It is not giving surprising results.
When I run an AC analysis the result depends on what I include in the sine wave parameters, especially on the phase.
Confer also the to jpg's in "files->temp->AD734 4 Quadrants Multiplier".
Example: Parameters of the input function 1 and 2 are sine waves (100 khz, 3 V). The Bode Plot shows a magnitude of 7.5 mV at 200 kHz.
When the first input is changed to the same sine wave but at a phase of 45°, the output changes to 643 mV at 200 kHz.

Now two questions arise for me:
a) Why is the .ac simulation influenced at all by the parameters of the transient simulation?
b) Why does the amplitude of the output in the transient analysis not coincide with the magnitude in the Bode plot at 200 khz (452 mV vs. 7.5 mV or 643 mV)?

I hope I could make my point clear. I would be very glad if someone could point me how to solve these issues.
Regards,
Maren

There is no inherent "time step" in LTspice. If you are thinking of a discrete-time system, then you need to add a "clock" (a pulse at some convenient frequency would work), and a sample/hold circuit. A second S/H can implement the t-1 function if the sample period is 1.

If this is a continuous time system, then a delay line or B element (either with delay of 1 second) will provide provide D(t-1). Another B element will sum the two with offset of a.

Jim Wagner
Oregon Research Electronics

On Jul 14, 2013, at 10:35 PM, feabyl wrote:

--- In LTspice@..., Andy <Andrew.Ingraham@...> wrote:

feabyl wrote:

How to implement an expression D(t)=D(t-1)+ a ?

Is that D(t-1) as in D(t - 1sec)?

If so, you can implement a 1 second time delay in either of two ways:

1. A (properly terminated) lossless transmission line (T-element) with a
delay of 1 second.

2. A behavioral source (B-element) with a delay of 1 second.

If the '-1' is supposed to represent the previous internal timestep in
LTspice, I don't think there is a way to do that. (But I'm not saying it
is impossible.)

Regards,
Andy

Thank you for the options suggested.Could you give an idea how to implement 1 sec delay using B-element.

[Non-text portions of this message have been removed]

--- In LTspice@..., Andy <Andrew.Ingraham@...> wrote:

feabyl wrote:

How to implement an expression D(t)=D(t-1)+ a ?

Is that D(t-1) as in D(t - 1sec)?

If so, you can implement a 1 second time delay in either of two ways:

1. A (properly terminated) lossless transmission line (T-element) with a
delay of 1 second.

2. A behavioral source (B-element) with a delay of 1 second.

If the '-1' is supposed to represent the previous internal timestep in
LTspice, I don't think there is a way to do that. (But I'm not saying it
is impossible.)

Regards,
Andy

Thank you for the options suggested.Could you give an idea how to implement 1 sec delay using B-element.

jason.vanryan <andrewc.russell@...> wrote:

Hello, have not posted here for quite a while!

Didn't you post here just this morning?

I have a number of schematic files that have a small lock icon just to the

left of them when I display the files in a folder. When I select all the
files and drag them into a USB memory stick folder, only the unlocked files
copy across. Any idea what I am doing wrong?

Please don't post the same question multiple times without bothering to
read what has already been posted in response to your question.

What is your computer operating system / version? In what folder are the
schematic files you are copying? Are any programs running when you attempt
to do the copy?

Andy

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

Hello,

I am trying to make a power supply using a 3722-1.

The input is 18 to 30Vdc and output is 165V@...

The issue that I am having is that at low input voltages like 24V or 18V the power supply is not able to reach full output level. At 30V the output level is reached but regulation is poor.

There's nothing wrong with the model, as such, but there seems to be a couple of issues with the circuit that you're simulating.

If you overcompensate it, you'll get a better idea about what is going on in the power train, as the control circuit will not be responsible for cycle by cycle variations.

There should be an overcompensated example posted in the temp files shortly.

In the working model, there is a shoot-through current occurring quite regularly. I don't know whether this is the result of intentional values placed in the drive delay circuits.

In real life, such spikes would invoke irregular limiting behavior in the 3722 that you'll want to avoid.

As to power throughput with reducing input voltage, you should take a look at the current waveforms and decide for yourself where the limitation lays.

RL

Hello, have not posted here for quite a while!

I have a number of schematic files that have a small lock icon just to the left of them when I display the files in a folder. When I select all the files and drag them into a USB memory stick folder, only the unlocked files copy across. Any idea what I am doing wrong?

Thanks

--- In LTspice@..., Andy <Andrew.Ingraham@...> wrote:

Herbert (<afu@...>) wrote:

Is it possible to give LTSPICE a value by a formula expression based on

a table ( interpolation???) ?

Yes you can. But the problem is that it tends to work well in .AC analysis
but not in .TRAN analysis.

Also, many inductive devices with iron-based cores are nonlinear, which
makes them difficult (impossible) to quantify in the frequency domain alone.

Andy

Andy,

Nonlinear inductor work fine in the frequency domain. The first thing LTspice does for an .AC analysis is to find the DC operating point. Then any nonlinear devices are linearized at their operating point. .AC analysis, by definition, is a small signal linear analysis and it does not deal with nonlinear devices other than noted above.

Rick

--- In LTspice@..., "highfidelityinc" <steve54@...> wrote:

Forgive me for asking such a basic question but is it possible to link several symbols (e.g. *.asy files) to the same package? I mean, say I have a quad opamp. I would like to position each of the 4 opamp individually on the schematic and maybe the power and ground to a separate symbol. Then when I export the Netlist to draw the PC layout, they are all assigned to the same package.

Currently I just make one big symbol with all four opamps and power and ground. But by doing that I cannot lay out my schematic as clearly without creating a rat nest of interconnecting wires.

Many thanks for your advice.
Steve

Hello Steve,

You could name the opamps U4A, U4B, U4C, U4D and do some
extra post-processing to modify the PCB-netlist.


Maybe this earlier discussion will help.

"pcb layout s/w for use with ltspice"

It starts with message #52018 and ends with the interesting
message/offer #52082 from Peter.

Best regards,
Helmut