Re: Passing a Mosfet Value as a parameter to a hierarchical subcircuit
.PARAM can only be used to pass numbers. From
the Help: To invoke parameter
substitution and expression evaluation, enclose the expression
in curly braces. The enclosed expression will be replaced with
the floating-point value.
Your .ASC is incomplete, anyway. There are
no supply voltages and no simulation directive. Your.ASY has no
attributes. Maybe that is OK, but maybe not.
On 2025-05-05 18:03, Per wrote:
Hi,
?
I want to make my own block for a bidirectional mosfet. I can
set up the .asc file with two mosfets in it and draw the .asy
file.
?
I want to do something like add MOS=IPB107N20N3 in the PARAMS
section on the Navigate/Edit Schematic Block but it moans at me
about not being able to resolve the parameter.
?
.asc and .asy file, hopefully, in the temp directory in a bit
as bimos.zip
?
Thanks for any help.
?
Per
--
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
|
Passing a Mosfet Value as a parameter to a hierarchical subcircuit
Hi,
?
I want to make my own block for a bidirectional mosfet. I can set up the .asc file with two mosfets in it and draw the .asy file.
?
I want to do something like add MOS=IPB107N20N3 in the PARAMS section on the Navigate/Edit Schematic Block but it moans at me about not being able to resolve the parameter.
?
.asc and .asy file, hopefully, in the temp directory in a bit as bimos.zip
?
Thanks for any help.
?
Per
|
Re: OPA square wave generator, single supply OPA is not working
I uploaded "LT1006 oscillator.zip" to the Temp folder.? It has three schematics:
?
- "Original (corrupt!).asc" is the original schematic that wai wai attached to a message.? It is corrupt, probably because it was attached to a message.
- "Fixed the corrupt values.asc" is the same except that I substituted the "mu" or "micro" character (?) for each instance of the corrupt character, hopefully restoring the original values.
- "Just the fixed oscillator.asc" is the same schematic but with the three other op-amps and all their unrelated circuitry removed, and with one change to the oscillator's biasing, which makes it oscillate with either dual or single supplies.
?
Why was the original file corrupt?? (Sorry, long story ahead.)? LTspice uses the Greek letter "mu" (?) to mean micro.? By default, if you have a capacitor, inductor, or resistor with a value in micro-anything - even if you physically type a "u" - LTspice converts it to a mu (?).? (You can disable that if you like, in the Settings / Control Panel.)? That letter is represented by the single byte hex B5 (0xB5).? Some may think of it as if it was part of the ASCII character set, but it is not.? PCs with MS-Windows knew 0xB5 meant "?".
?
All is well if those schematics stay within LTspice, and move to and from your computer's drive and most other drives.? But if you take the actual text code (of an LTspice .ASC schematic file) and open it or copy-and-paste it into a text editor, bad things might happen to it.? Some editors preserve it.? Others do not; they notice it is a non-ASCII character and attempt to convert it into something else, which might be either one or two bytes.? We saw that a lot before 2020 when this group was hosted on Yahoo!Groups, because Yahoo's editor would corrupt those bytes if anyone ever edited an LTspice schematic file that had been previously uploaded.
?
In this particular case, when wai wai copied-and-pasted the contents of their original schematic file into their message for the group, those characters found themselves converted from ? to Ϥ and they were now corrupt and not recognized by LTspice.? (That is one of the reasons why you should never ever paste a schematic file into your messages in this group!)? I think LTspice interpreted the "1Ϥ" capacitor as a 1 (Farad) capacitor.? And similarly for the others.? Like all good SPICE programs, unrecognized multipliers are ignored.
?
In the second file inside the .ZIP, I fixed those corrupt values.? I assumed that all six bad values were supposed to be microfarads.
?
Most of the circuitry on that schematic was entirely unrelated to wai wai's question about the oscillator.? So I deleted it.? The third schematic has just the oscillator, with one small change so that it oscillates with either dual or single supplies.
?
Andy
?
?
|
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.
?
|
John Woodgate
wai wai
Tony Casey