Re: OPA square wave generator, single supply OPA is not working
On Sun, May 4, 2025 at 04:11 AM, wai wai wrote:
LT1006 was a single supply OPA. Trying and gathered no output when single supply was used. welcome any hints or experience would be share, thanks.
Suggestion:
?
Connect the bottom end of R7, to a voltage which is between VEE and VCC.? That allows the voltage across the capacitor to ramp above and below that voltage.
?
By connecting the bottom end of R7 to VEE itself (to a grounded negative supply), the voltage across the capacitor is unable to swing to both sides of it, which is necessary for it to oscillate.
?
Andy
?
|
Re: Crystal oscillator oscillation startup
On Sun, May 4, 2025 at 10:46 AM, Cheng Fei Phung wrote:
May I ask how to resolve the issue for floating node N004 ?
You might not need to, since LTspice resolves that problem for you, by connecting a 1T resistor (GFLOAT) from that net to ground.? Note that the message is a Warning, not an Error, and it fixes it and proceeds with the simulation.
?
If 1 Tohms is not big enough, you can change the value of GFLOAT (.options GFLOAT=1e-15).? This resistor adds damping and reduces the Q of your crystal's equivalent circuit.? It might be insignificant in this case, but that might not always be true.? Also there are cases where adding a single resistor disturbs the balance of a balanced circuit - so it might (sometimes) be better to fix this problem yourself (instead of letting LTspice), by adding appropriate resistor(s), so that every circuit node has at least one DC path to ground.
?
If you want to fix the problem yourself, add a very big resistor from the node to ground, or to another voltage if there is one that is better than ground.
?
In your circuit, nodes Q1, N004, and N005 all lack a DC path to ground.? They have a DC path to each other.? They are isolated from ground by C1, C6, C7, and C8 on one end, and by C3 on the other end.
?
LTspice picks one of those three nets (not quite arbitrarily) and adds GFLOAT between that net and ground, which fixes the problem for all of them because they share a DC path to each other.
?
Note: The series RLC circuit or Figure 2(b) is an equivalent model of Figure 2(a) inside the IEEE paper.
Perhaps.? But neither is equivalent to the crystal model in Figure 1 in the paper.
?
I rarely ever see cases where a crystal needs to be modeled in SPICE as more than two resonant circuits (series and parallel), and one is usually sufficient.? I wonder if the model in Figure 1 was supposed to represent the first three harmonics?? If that is the case, one might be able to omit the other harmonics.? Crystal oscillators can be tricky and under the right circumstances they can oscillate on an unintended harmonic.? Good oscillator circuits are designed to suppress the other harmonics.
?
Andy
?
?
|
Re: OPA square wave generator, single supply OPA is not working
Oops - correcting a typo.? I wrote:
It does not oscillate because the voltage on the "voltage" net (across the capacitor) ...
but that should have said:
It does not oscillate because the voltage on the "vcharge" net (across the capacitor) ...
?
Andy
?
|
Re: OPA square wave generator, single supply OPA is not working
wai wai,
?
The schematic you attached to your message today has several mistakes.? I am just letting you know.? It was a very sloppy schematic and you should not have used it as an example.
?
Apparently the question was about the LT1006.? But your schematic also has three other op-amps, which are apparently unrelated to the question, and you forgot to connect any power to those op-amps.? Without power, they can not operate.? Leaving inoperable circuits on the same schematic can cause problems with the simulation.? It might even have caused the oscillator to not oscillate (although that was not the reason in this case).
?
You used multiple net names on the same nets.? That is unwise and should be avoided.? Nets (wires) can have only one net name.
?
The comment on your schematic asked:
LT1006 is single supply OPA
but single 5V has no square wave oputput
dual power supply vcc & vee must be, why ?
The answer to that question is because your circuit is wrong.? It does not oscillate because the voltage on the "voltage" "vcharge" net (across the capacitor) never drops below the voltage at the R7/R6 junction, when the op-amp drives Low.? That voltage must become lower in order for the op-amp's output to go High, which it can never do.? The circuit has a stable operating point when the amp's output is Low.
?
You must re-arrange the bias conditions of your circuit to make it oscillate with a single supply.? The LT1006 op-amp is operating correctly.
?
Andy
?
?
|
Re: OPA square wave generator, single supply OPA is not working
wai wai,
?
I have edited your message to remove the nonsense schematic that you attached to your message.? DON'T EVER DO THAT!
?
Go back and read (actually read!) the instructions about using this group.? Notice where it says:
Important:? Do not attach?or include or embed or drag-and-drop any files or pictures in your messages.? Instead,?upload?files to this group's "Temp" folder -
Now, if you want help, upload your schematic file to the group's Temp folder.? Then tell us that you uploaded a file there.
?
You almost did the right thing earlier today, by uploading a schematic (humidity_sensor.asc), but then you deleted it!? Why?
?
I also deleted your schematic text because it has an unrecognizable character which even LTspice can't use.? That might have been caused by attaching your schematic code to a message.? Instead, UPLOAD the file, which preserves the characters.
?
Andy
?
?
?
|
Re: Crystal oscillator oscillation startup
@Andy
?
?
May I ask how to resolve the issue for floating node N004 ?
?
Note: V004 is between Q1 and the R1 of the series RLC circuit.
Note: The series RLC circuit or Figure 2(b) is an equivalent model of Figure 2(a) inside the IEEE paper.
?
Please advise, thanks !!
?
|
Re: OPA square wave generator, single supply OPA is not working
Please don't post such long netlists. Few of us will try to help using a netlist. Upload your .ASC file AND all the other files required to run the simulation, but not .RAW? and .LOG files or pictures,? in a ZIP archive to Files => Temp.
Go to the web page: /g/LTspice/topics. Click on Files in the list on the left. Then click on Temp. Then click on New Upload in the blue box at top left. Click on Upload File in the drop-down menu. Then send a message to tell us that you did that.
On 2025-05-04 09:02, wai wai via groups.io wrote:
LT1006 was a single supply OPA. Trying and gathered no output when single supply was used. welcome any hints or experience would be share, thanks.
the code used,
?
?
[Mod note: Edited for brevity]
--
Best wishes John Woodgate RAYLEIGH Essex OOO-Own Opinions Only If something is true: * as far as we know - it's science *for certain - it's mathematics *unquestionably - it's religion
|
OPA square wave generator, single supply OPA is not working
LT1006 was a single supply OPA. Trying and gathered no output when single supply was used. welcome any hints or experience would be share, thanks.
the code used,
?
?
[Mod note:? schematic code deleted]
?
|
Re: Crystal oscillator oscillation startup
On Sat, May 3, 2025 at 12:38 PM, Cheng Fei Phung wrote:
> Just be aware that all of your MOSFETs default to AS=0, AD=0, PS=0, and PD=0
Noted, is it safe to use 0 for these in your expert opinion ?
"Safe"?? I don't know, it depends on one's definition of "safe".
?
Accurate?? Probably not.? Any time you omit something that you know about, or change a value from what it ought to be, it degrades accuracy.? If I remember right, SPICE MOSFET models include the capacitances of the bottom and sidewalls of the source and drain diffusions.? Leaving them set to 0 removes (ignores) that capacitance.? It might also ignore DC effects from their junction diodes.? Those omissions might be significant or insignificant.
?
You might have noticed several warnings about PS and PD in your SPICE Error Logs.
?
It is a simple (but tedious) schematic change to switch to the .SUBCKT models which automatically calculate AS, AD, PS, and PD.? Change the Prefix attribute to "X" to use the .SUBCKT version.
? ? Prefix = "X":? call the .SUBCKT model.
? ? Prefix = "MN" or "MP":? call the .MODEL model.
Use Ctrl-right-click to get to LTspice's General Attribute Editor where you can change the Prefix attribute's value.? That must be done to each of your transistors.
?
Apparently these models were designed for a fab process with an effective length of 1.1 microns for each Source and Drain diffusion.? Hopefully that is correct.
?
Andy
?
?
|
Re: LTspice24 windows version run on macOS
#Mac
On Sat, May 3, 2025 at 01:30 AM, professor_chaos99 wrote:
installed in /opt/homebrew/bin/ instead of /usr/local/bin/
That's because homebrew uses a different installation location on Apple Silicon Macs that it does on Intel Macs. You are using an Apple Silica Mac and I posted instructions based on my old Intel iMac.
?
|
Re: Crystal oscillator oscillation startup
@Andy
?
Your advices are valuable and very useful !!! ? Thanks !!!
?
> .MODEL statements are meant to use the pin-order D-G-S-B
Got it, noted. I will swap the order and get back to you tomorrow with a corrected circuit.
> at M19, M17, M9, M37, M39, M5, M22, M33, and M35, their Bulk pins connect to internal circuit nodes between the supply voltages
I will double check these and get back to you tomorrow with a corrected circuit.
?
> Just be aware that all of your MOSFETs default to AS=0, AD=0, PS=0, and PD=0
Noted, is it safe to use 0 for these in your expert opinion ?
|
Re: Crystal oscillator oscillation startup
On Sat, May 3, 2025 at 05:45 AM, Cheng Fei Phung wrote:
That is a huge change!
?
The fact that you moved the ground is insignificant.? It just shifts the voltages.? But you are no longer powering the "VN" net with a voltage source that had the polarity wrong, and that is a significant change.
?
Not having studied the IEEE article, I wasn't sure but I suspected that the purpose of the "Output voltage regulator" section (and your M32) was to derive a regulated DC voltage on node VN.? And it looks like that is finally working now, in this schematic.? The earlier schematics you uploaded had that wrong, both by driving VN with a separate voltage source and by giving it the wrong polarity.
?
However, I would not expect much difference in circuit performance at this stage.? The oscillator is the part of the circuit way over on the left, and everything else in the schematic is superfluous, except for the DC biasing voltages on nodes "g_a" and "g_b".? The output amplifier is just an output buffer and you could have omitted it because it is not part of the oscillator.? It adds a little load on the "Q1" net but I think that could be mostly ignored.
?
What do you hope to achieve by sweeping the supply voltage, V_1?? Does it give you any significant information about the operation of the circuit?? In the end it does, after everything is working.? It tells you about things like supply voltage "pull".? But until the circuit oscillates, I think sweeping V_1 does not give you any useful information.
?
I think I might be more interested in sweeping the DC voltage at the input of the oscillator's amplifier (node "M1_gate") and examining what is the transfer function and signal gain of M1.? That gain is what makes the oscillator oscillate - or perhaps why it does not oscillate.? Perhaps you should be looking there.
?
I am now interpreting the underlying theory, I will get back to you next week with details.
That's good - but why have you not considered much of the advice you were given?? It seems to me that you are not very interested in trying to get your circuit right.? Do I read that incorrectly?
?
Andy
?
?
|
Re: Crystal oscillator oscillation startup
@Tony See ck_osc_positive_supply.asc , I had actually checked the operating points conditions for each transistors according to circuit requirements. I am now interpreting the underlying theory, I will get back to you next week with details.
|
Re: Crystal oscillator oscillation startup
On 03/05/2025 03:02, Cheng Fei Phung
via groups.io wrote:
@Andy
?
still do not show any oscillatory phenomenon after adding RLC
between Q1 and Q2.
?
Did you check the DC conditions on your circuit? Is it biassed
correctly? What gain do you get from each inverter?
Make one step at a time.
To help you (and anyone else following) along the way, I have made
some testjigs to validate the characteristics of both P and N
devices, including both the normal and inverted N configurations
(they are identical, so the devices are symmetrical).
See 180nm_Testjigs.zip
--
Regards,
Tony
|
Re: LTspice24 windows version run on macOS
#Mac
Dennis, thank you much for this detailed install guide!
?
My Wine application wound up being installed in /opt/homebrew/bin/ instead of /usr/local/bin/, but that might be because of how I installed brew.
|
Re: Using Op Amp as comparator
SUCCESS. Big thanks again.? Changing the MAX9095 power supply to 6 VDC did the trick.? Note the extra parts for hysteresis, per the datasheet.
?
Thanks for the suggestions.? I've heard the suggestion about how to deal with decimals before, but I guess I have a kind of dyslexia where I make fewer mistakes when I can actually see the number of zeros.? I'll try to remember that's not optimum for those who are helping me.
?
Here's the asc file: /g/LTspice/files/z_groups.io/Files-sorted-by-message-number/msg_ZZZZZZ/Macrohenry/comparator_test.asc
|
Re: Crystal oscillator oscillation startup
You (Cheng Fei Phung) seem to be grasping at straws with pretty minimal understanding. In your situation, I would disconnect the "crystal" and feed a small transient 1.1MHz signal (say a hundred mV ppk or less) through a small capacitor (few 10s of pF). Verify that the amplifier has the expected operating point and has some actual gain at that frequency. Use a reasonable maximum time step (less than 50ns) and let the simulation run more than a few cycles (10 uS or longer). ?
?
Once you have an operating amplifier, THEN hook the simulated crystal.
?
You might actually learn something if you observe the results fully and carefully! AND you convey those observations back to the list, in good detail. Hint: that report might include a full spice circuit with all the supporting models that either fails to operate or operates with some degree of success.
?
Jim
Oregon Research Electronics
?
?
On 05/02/2025 6:02 PM PDT Cheng Fei Phung via groups.io <feiphung@...> wrote:
?
?
@Andy
?
still do not show any oscillatory phenomenon after adding RLC between Q1 and Q2.
?
|
Re: Crystal oscillator oscillation startup
On Fri, May 2, 2025 at 09:02 PM, Cheng Fei Phung wrote:
still do not show any oscillatory phenomenon after adding RLC between Q1 and Q2.
?
I see you added a simple RLC series resonant circuit to represent a crystal.? Do you know that it is an appropriate model?? Does this oscillator circuit depend on series resonance, or parallel?? (I don't know; I am just asking.)? Are the electrical characteristics OK to model the motional parameters of the crystal?
?
Glancing at the IEEE article, it looks like they used a much more complex electrical model for the crystal, with not one or two but three series resonant RLC circuits in parallel with each other, plus three additional capacitors.? Your equivalent circuit is much simpler.? Is the simpler model adequate?
?
The .tran statement on your schematic is ".tran 0 10 0 100u startup", so it calls for a Maximum Timestep of 100 us.? With a timestep of 100 us, it can simulate signals with frequencies up to about 5 kHz.? But your crystal model's series resonance is around 1.1 MHz.? To simulate a circuit oscillating at 1.1 MHz requires a timiestep that is smaller than 500 ns.? There is a chance that you made the Maximum Timestep so large that LTspice is incapable of seeing any sort of oscillation around 1 MHz.
?
This is where simulations can become very difficult.? With a timestep smaller than 500 ns, it can take a very long time to simulate 10 seconds or 1000 seconds.
?
Your N channel transistors are still upside-down, and the Bulk pins of many of the transistors are likely connected wrongly.? Also you have zero values for PS, PD, AS, and AD, which is technically incorrect, but I don't know how much difference it makes.? As you probably know already, I1 should not be there, but LTspice removes it.
?
I suspect that your DC voltages are not right.? The negative supply voltage for the first three stages (node V1) is at -1.5 V which might be right.? But the regulated voltage for the output amplifier (node VN) is +1.5 V.? Is that right?? I think it powers the output amplifier with the wrong polarity.? Are you powering that section correctly?
?
There is no DC path from node Q1 to ground, which extends to nodes N004 and N005.? LTspice tells you that the nodes float, and it "corrects" for it by adding GFLOAT to one of the nodes.? I think this won't affect the performance of this circuit, but I'm not sure.? GFLOAT will lower the Q of the resonant circuit a little.
?
Note I have not read the IEEE article.
?
Andy
?
|
Re: Crystal oscillator oscillation startup
@Andy
?
still do not show any oscillatory phenomenon after adding RLC between Q1 and Q2.
?
|
Re: Using Op Amp as comparator
I met one of those, so I used the 'bullet'
character ? as the decimal point in my report.
On 2025-05-02 23:48, Andy I via
groups.io wrote:
On the other hand,
there are others who insist on omitting a leading "0" when there
is one, thus encouraging people to write ".002", to the dismay of
others who have greater sense.)
--
Best wishes John Woodgate RAYLEIGH Essex OOO-Own Opinions Only
If something is true: * as far as we know - it's science *for
certain - it's mathematics *unquestionably - it's religion
|
John Woodgate
wai wai
Tony Casey