Re: Convergence problem with Sallen-Key filter circuit
Hello John,
Sorry, you are correct. The cut-off frequency is 38kHz. It's still a frequency where one can find much better suitable opamps.
Best regards, Helmut
---In LTspice@..., <jmw@...> wrote : That's odd. I get the -3 dB frequency as 38
kHz. The point about the resistor values is quite
subtle, as it doesn't apply to most common op-amps, and the data
sheet doesn't draw attention to it.
Best wishes
John Woodgate OOO-Own Opinions Only
J M Woodgate and Associates
Rayleigh, Essex UK
?Hello Jan,
Your circuit finds the operating point aftre a long
time in the pseudo transient analysis.
You can automatically skip the other methods. See
below.
.options noopiter gminsteps=0 srcsteps=0
This opamp is for resistors with a resistance below
1kOhm at it's input due to its maximum bias current of
10uA. It's the wrong opamp for your application of a
lowpass filter with 10kHz cut-off frequency.
Best regards, Helmut
|
Re: Convergence problem with Sallen-Key filter circuit
That's odd. I get the -3 dB frequency as 38
kHz.
The point about the resistor values is quite
subtle, as it doesn't apply to most common op-amps, and the data
sheet doesn't draw attention to it.
Best wishes
John Woodgate OOO-Own Opinions Only
J M Woodgate and Associates
Rayleigh, Essex UK
toggle quoted message
Show quoted text
?
Hello Jan,
Your circuit finds the operating point aftre a long
time in the pseudo transient analysis.
You can automatically skip the other methods. See
below.
.options noopiter gminsteps=0 srcsteps=0
This opamp is for resistors with a resistance below
1kOhm at it's input due to its maximum bias current of
10uA. It's the wrong opamp for your application of a
lowpass filter with 10kHz cut-off frequency.
Best regards,
Helmut
|
Re: Convergence problem with Sallen-Key filter circuit
Hello Jan,
Your circuit finds the operating point aftre a long time in the pseudo transient analysis.
You can automatically skip the other methods. See below.
.options noopiter gminsteps=0 srcsteps=0
This opamp is for resistors with a resistance below 1kOhm at it's input due to its maximum bias current of 10uA. It's the wrong opamp for your application of a lowpass filter with 10kHz cut-off frequency.
Best regards, Helmut
|
Re: Convergence problem with Sallen-Key filter circuit
Hello Jan,
Balance the opamp input resistances by inserting 10k in series with the inverting input of the first opamp and 15k in series with the inverting input of the second opamp.? This makes the LT6232 model happy (besides being good design practice).
|
Re: Convergence problem with Sallen-Key filter circuit
It's not about convergence really; LTspice
cannot find the DC operating point easily.? If you add the Spice
directive .option gminsteps=0, the simulation runs and gives
credible results for the AC sweep.
By the way, asking for 10 thousand points per
decade in your AC sweep is huge overkill, especially as you are
sweeping over many decades.
Best wishes
John Woodgate OOO-Own Opinions Only
J M Woodgate and Associates
Rayleigh, Essex UK
toggle quoted message
Show quoted text
?
Hello there
group members,
I'm trying to
simulate a Sallen Key filter with a cutoff frequency
of around 40kHz using a unipolar 5V source (See TEMP
section). The initial operating point solution does
not converge.?
I have added series resistances everywhere so?every
point in the circuit has a connection to GND as
described in?
Since I cannot find any problem in my circuit, I'm
out of ideas on where LTSpice might fail.?
Can someone hint me to where the problem might be?
?
Best regards,
Jan
|
Re: Convergence problem with Sallen-Key filter circuit
Jan wrote:
"I'm trying to simulate a Sallen Key filter with a cutoff frequency
of around 40kHz using a unipolar 5V source (See TEMP section). The
initial operating point solution does not converge.
I have added series resistances everywhere so every point in the
circuit has a connection to GND as described in
Since I cannot find any problem in my circuit, I'm out of ideas on
where LTSpice might fail.
Can someone hint me to where the problem might be?"
Your circuit converges fine and runs with .options gminsteps=0.
It make no sense to have 10000 points per decade in an .AC analysis,
unless you have a circuit with a Q of 1000s - I changed it to 24. It
just takes longer and you produce a huge .RAW file.
Regards,
Tony 
|
Re: Convergence problem with Sallen-Key filter circuit
Jan wrote, "The initial operating point solution does not converge.?"
Actually, it does.? But the Gmin Stepping algorithm has trouble, and either runs a very long time or never finishes.? We see this from time to time.? I don't know why LTspice seems to get stuck on one algorithm instead of moving on, but it happens occasionally.
LTspice has a handful of different algorithms that it tries when looking for the DC operating point.? It's supposed to know when one isn't working, and move on to try the next, and so on.? In your circuit's case, the Direct Newton-Raphson Iteration algorithm quickly fails, and then the Gmin Stepping algorithm tries but seems to keep trying forever.? So you need to tell LTspice to skip that algorithm:
? ? .options GminSteps=0
I see that you had that on your schematic, but it is commented out (ineffective).
Alternatively, you can press the Esc key when it's trying (forever) in that algorithm, and it moves on to the next one.? Watch the status messages in the lower left corner.? "Press Esc to quit" doesn't quit LTspice; it only quits the current algorithm.? Your circuit converges OK with either the Source Stepping or the Pseudo Transient algorithms.
See this Help page: LTspice > Dot Commands > .OP -- Find the DC Operating Point
Regards, Andy
Hello there group members,
I'm trying to simulate a Sallen Key filter with a cutoff frequency of around 40kHz using a unipolar 5V source (See TEMP section). The initial operating point solution does not converge.?
I have added series resistances everywhere so?every point in the circuit has a connection to GND as described in?
Since I cannot find any problem in my circuit, I'm out of ideas on where LTSpice might fail.?
Can someone hint me to where the problem might be?
?
Best regards,
Jan
|
Re: Drag/Drop circuit from one window into another
In order to copy a schematic or part of one to another schematic, you have to have both schematics open in the same instance of LTspice. Open them both before you try to copy.
I¡¯m talking about nothing else than having them open in the window of one and the same LTspice application. But I now see that I have to?
1. Select Duplicate (F6) 2. Frame the area to be selected. 3. Click on the target window 4. drag the circuit which then hangs at the cursor 5. drop it into the target window.
Thanks, got it.
(Forgot to select the raget window while the copy action was still active) Best wishes
John Woodgate OOO-Own Opinions Only
J M Woodgate and Associates
Rayleigh, Essex UK On 2018-12-02 14:34, ?kuku@...?[LTspice] wrote: ?I thought it would work to select/duplicate a portion of a schematic and drag it into a new window? But for the moment I can't find the protocol how to perform this.
With a copied circuit hanging on the cursor it's possible to open a new sheet on the fly and drop the circuit into that.
But how can I insert the circuit into an existing one which is currently open in the multiple window view?
-- Christoph
|
Convergence problem with Sallen-Key filter circuit
Hello there group members,
I'm trying to simulate a Sallen Key filter with a cutoff frequency of around 40kHz using a unipolar 5V source (See TEMP section). The initial operating point solution does not converge.?
I have added series resistances everywhere so?every point in the circuit has a connection to GND as described in?
Since I cannot find any problem in my circuit, I'm out of ideas on where LTSpice might fail.?
Can someone hint me to where the problem might be?
?
Best regards,
Jan
|
Re: Drag/Drop circuit from one window into another
In order to copy a schematic or part of one to
another schematic, you have to have both schematics open in the
same instance of LTspice. Open them both before you try to copy.
Best wishes
John Woodgate OOO-Own Opinions Only
J M Woodgate and Associates
Rayleigh, Essex UK
On 2018-12-02 14:34, kuku@...
[LTspice] wrote:
toggle quoted message
Show quoted text
?
I thought it would work to select/duplicate a portion
of a schematic and drag it into a new window? But for the
moment I can't find the protocol how to perform this.
With a copied circuit hanging on the cursor it's
possible to open a new sheet on the fly and drop the
circuit into that.
But how can I insert the circuit into an existing one
which is currently open in the multiple window view?
--
Christoph
|
Drag/Drop circuit from one window into another
I thought it would work to select/duplicate a portion of a schematic and drag it into a new window? But for the moment I can't find the protocol how to perform this.
With a copied circuit hanging on the cursor it's possible to open a new sheet on the fly and drop the circuit into that.
But how can I insert the circuit into an existing one which is currently open in the multiple window view?
-- Christoph
|
Re: Hilighting a voltage in schematics
Hello Christoph,
There is no cross probing available, but there is a workaround.?
Click the "search"-icon on the toolbar and enter the netname. Then the net will be highlighted.
Thanks, nice trick.?
¡ª Christoph
|
Re: Hilighting a voltage in schematics
I name all nodes that might be "interesting" so I know where everything is.
Donald.
--
*Plain Text* email -- it's an accessibility issue
() no proprietary attachments; no html mail
/\ <>
toggle quoted message
Show quoted text
On 2018-12-02 6:02 a.m., kuku@... [LTspice] wrote: To find a signal name in the schematics, is it possible to highlight this signale, e.g. from the plot view?
I have a lot of signal names but can't find them quicklx in the circuit drawing.
--
Christoph
|
Re: Hilighting a voltage in schematics
Hello Christoph,
There is no cross probing available, but there is a workaround.
Click the "search"-icon on the toolbar and enter the netname. Then the net will be highlighted.
Best regards, Helmut
|
Hilighting a voltage in schematics
To find a signal name in the schematics, is it possible to highlight this signale, e.g. from the plot view?
I have a lot of signal names but can't find them quicklx in the circuit drawing.
-- Christoph
|
Re: Auto loadbias and savebias for stepped simulations
Hello analogspiceman I recently asked Mike if would be possible to add a new feature to .savebias
and .loadbias invoked by the keyword ¡°eachstep¡± whereby in a stepped
simulation, each succeeding step would load the bias saved by the preceding
step. Among other uses, this could allow eliminating the startup transient
between steps when performing a time domain frequency response analysis. What was his response? I'm also curious because, by chance, I saw this topic come up on electronics.stackexchange a few days ago. -- Vlad ______________________ ltspicegoodies.ltwiki.org -- holding, among others: a universal analog/digital filter, block-level models for power electronics (and not only), math blocks with a more stream-lined approach, some digital ADC, DAC, (synchronous-)counter, JKflop, etc.
|
Auto loadbias and savebias for stepped simulations
I recently asked Mike if would
be possible to add a new feature to .savebias and .loadbias invoked by
the keyword ¡°eachstep¡± whereby in a
stepped simulation, each succeeding step would load the bias saved by
the preceding step.? Among other uses, this could allow eliminating the
startup transient between steps when performing a time domain frequency
response analysis.
Currently bias data may be saved from individual steps, but the syntax is cumbersome as each step must be specified:
.savebias bias1.txt time=1m step=0
.savebias bias2.txt time=1m step=1
.savebias bias3.txt time=1m step=2
Unfortunately, there is no way to load different bias data for steps, which is the reason for my request to Mike.
Yes, I realize that .savebias type commands do not save branch currents (inductor states), but that may be
neatly circumvented by creating a simple inductor subciruit that
converts a capacitor into its dual via controlled current sources. (I posted this a few days ago.)
.subckt L 1 2
.param L=1 Rser=1m Rpar=1/Gmin
C1 3 0 {L} Rser={1/Rpar} Rpar={1/Rser}
G1 1 2 3 0 1
G2 3 0 2 1 1
.ends L
?
Merry Christmas and a Happy New Year
|
Re: schematic erorr download from internet
|
Re: What does Heightened Def Con mean ?
wgrandner wrote, "What does Heightened Def Con mean ?"
It means LTspice is having some trouble, but hasn't given up yet.
In your case, it may mean there is something in your circuits that is making LTspice unhappy.
Here is a very old message, from the master himself (LTspice's author):
? ?? ? ? Def Con" comes from the term DEFCON or DEFense CONdition. ? ? In public service, this runs from 5 to 1. The lowest state ? ? of defensive readiness is condition 5, meaning normal ? ? peacetime. DEFCON 1 is the highest defensive condition ? ? readiness and means the country is at war. ? ? In LTspice, the scale is reversed, Def Con 0 means it's ? ? having no trouble solving the circuit and increases with ? ? circuit difficulty. Its main use for macro models circuits ? ? is to let you gauge a bit as to how robust the model is. ? ? I haven't looked at your circuit, bit it sounds like you ? ? might be exciting some some kind of a race condition in the ? ? model. Don't forget to try the alternate solver when you ? ? have convergence problems. ? ? --Mike Note the mention of the Alternate Solver.? It might (or might not) help eliminate those messages.? The Alternate Solver is usually more accurate, but slower; but in some cases it can be the other way around.? Don't forget that the Alternate Solver is a "sitcky" setting, so it remains selected until you un-select it.
Regards, Andy
|
What does Heightened Def Con mean ?
When I run simulations, I get a messages in the Spice error log stating
Heightened Def Con from 0.00011015 to 0.00011015
In most of my simulations I get over 100,000 messages, where the number is slowly changed. What does this mean?
|
John Woodgate
Tony Casey
Christoph