Re: Estimating Base spreading resistance for a bipolar transistor via LTspice
I meant to say the fall in transconductance as frequency increases.
|
Re: Estimating Base spreading resistance for a bipolar transistor via LTspice
For a BJT model, the parameters Rb, Rbm and Irb determine the base spreading resistance. The resistance is Rb at low currents and falls to the value of Rbm as current increases past the value of Irb.
?
The base spreading resistance is not present in LTspice unless it has been specified in the model. Many models use Rb=10 as a default value. There are many thousands of garbage models in existence which bear only a passing resemblance to the BJTs they are named after (likely the result of a failed attempt to batch process a dataset into SPICE models).
?
Rb can be estimated by measuring the base voltage noise of a transistor at the collector current you plan to use it at. This does not always give the same value of Rb as the high frequency estimation method where you determine Rb based on the rise in transconductance as frequency approaches Ft (this is possible with s-parameters).
?
There are still other methods of extracting Rb that are given in multiple long PDFs about the SGP model, although I can't find any of them at the moment.
?
Here is a page with a calculator for using the noise method:
http://www.dicks-website.eu/low_noise_amp_part4/part4.html
|
Re: 12AU7 tube heater model
I think it's a question that's no often asked:
people just accept it as a magic number. I did a web search,
which led to a URL about half a km long, so I can't post it.
Instead, do a web search for 'Coefficient
of Determination, R-squared'. It's a measure of the accuracy of
the trend line, based on RMS deviations from the curve. A
perfect match is a value of 1.
On 2025-02-22 17:38, Carlo wrote:
On Sat, Feb 22, 2025 at 08:14 AM, John Woodgate wrote:
A bit of Excel work gives a resistance trend line
(for voltages between 3.0 and 6.5)? R = 0.22*V^2 + 3.61*V +
6.50. The R^2 (accuracy measure) = 0.9993, good enough for
government work.
Sorry, what does R^2 accuracy measure of 0.9993 actually mean ?
?
Thanks.
--
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
|
Re: 12AU7 tube heater model
On 22/02/2025 16:30, Andy I via
groups.io wrote:
I believe that this
has been somewhat restricted now, in LTspice version 24.1.?
Previous versions generated a SPICE Netlist file when they ran,
which was saved on your drive but deleted when LTspice is closed.?
Version 24.1 no longer generates a runnable SPICE Netlist file.? I
believe it can still run (process) a Netlist file if you have one,
but saving one might no longer be an option.? I could be wrong.
I haven't yet tried other than 24.1.0, but View > SPICE Netlist
> Right-click > Edit as Independent Netlist > Save, is
still available from the Schematic menu.
I hope that feature remains, otherwise how about if you wanted to
use batch mode (with -b) to run a netlist? (Assuming batch mode,
itself, is still available.)
--
Regards,
Tony
|
Re: 12AU7 tube heater model
On Sat, Feb 22, 2025 at 08:14 AM, John Woodgate wrote:
A bit of Excel work gives a resistance trend line (for voltages between 3.0 and 6.5)? R = 0.22*V^2 + 3.61*V + 6.50. The R^2 (accuracy measure) = 0.9993, good enough for government work.
Sorry, what does R^2 accuracy measure of 0.9993 actually mean ?
?
Thanks.
|
Estimating Base spreading resistance for a bipolar transistor via LTspice
Hello friends,
?
Is there a way of estimating the base spreading resistance of a bipolar transistor by using LTspice? Perhaps via getting the transistor's S-parameters?
Many thanks in advance!
|
Re: 12AU7 tube heater model
FYI - My advice about adding GMIN across current sources, is that you should specifically add them to your current sources, by adding a resistor in parallel with them.
?
The checkbox in the Control Panel's Hacks! tab is not permanent (it goes away when you close and then re-start LTspice), and it does not solve any topology problems and won't eliminate that error you had.? If you think you need a conductance added across your current sources, do it by adding resistors to the schematic!? That is my advice.
?
Andy
?
?
|
Re: Build spice model of transimpedance amplifier
Keep in mind, this question was asked nearly a year ago.? This conversation ran out months ago and I don't know if the OP is still looking for answers.
?
If I remember correctly, that person was looking to find an actual transimpedance amp they could purchase, for a specific high-speed application.
?
Andy
?
?
|
Re: 12AU7 tube heater model
On Sat, Feb 22, 2025 at 11:55 AM, Carlo wrote:
Do you think .options gmin=<value> is actually the same as "Add GMIN across current sources" checkbox?
No, they are not the same.
?
".options gmin=<value>" sets GMIN to a number.? GMIN is used in a number of places in SPICE/LTspice, including in parallel with EVERY semiconductor junction.? GMIN is used in other places too.? If you search LTspice's Help for "GMIN", you can see some of the other places.
?
Checking the checkbox to "Add GMIN across current sources" adds yet another place where a conductance with value GMIN may be added.? But for that to work, first GMIN needs to have a value.? Giving GMIN a value does not cause it to magically appear in extra places where it does not normally appear.? Note that GMIN must always have a value.? SPICE won't run without it.
In other words, does .options gmin=<value> add a <value> Siemens conductance in parallel to each (controlled or independent) current sources as well ?
No, not unless you check that checkbox!
?
Again, I note that GMIN always has a value.? Its normal value is 1e-12, as shown on the Help page for .OPTIONS.? It can also be set in the Control Panel, and that is the same GMIN.? It might not be possible to set GMIN to 0.0000000000000.? Trying to do that might instead set it to its default value of 1e-12.? SPICE/LTspice might not run at all if GMIN were actually set to 0, or if it did, it might run poorly.? All this has nothing to do with current sources.? GMIN is a necessary convergence aide to help SPICE converge when there are semiconductor PN junctions, as well as a handful of other things.
?
(Interesting note:? LTspice also uses the value of GMIN to set a minimum resistance value, in certain cases where a resistance must not reach zero.? That is kind of contrary to engineering logic, because GMIN is supposed to be a small conductance, not a small resistance.? But it silently does that anyway.? I guess it does this as a way of avoiding yet one more OPTION variable.? Yes it's cheating, but it works.)
?
Andy
?
?
|
Re: Build spice model of transimpedance amplifier
I have never been mistaken for an analog designer but if your application demands bandwidth, would considering a current feedback amplifier as the basis of your transimpedance amp be a consideration?? I'm not sure if you're able to use a device with an external resistor or not.? I don't know your application and even if I did I probably wouldn't appreciate the intricacies of its design.? So, best wishes,
Coop, aa1ww
?
|
Re: 12AU7 tube heater model
Thank you Andy.
Do you think .options gmin=<value> is actually the same as "Add GMIN across current sources" checkbox? In other words, does .options gmin=<value> add a <value> Siemens conductance in parallel to each (controlled or independent) current sources as well ?
|
Re: using LTSPICE symbols for representation of spice netlist of OPAMP
john23,
?
Apparently, LTspice incorrectly processes the AD797 model file.? I don't understand why it did that, but here is how to fix it.
?
Change from this:
.SUBCKT MyAD797 In+ In- V+ V- Out
X? In+ In- V+ V- Out Decomp? AD797
.LIB AD797.cir
.ENDS MyAD797
to this:
.SUBCKT MyAD797 In+ In- V+ V- Out
X ?In+ In- V+ V- Out Decomp ?AD797
.ENDS MyAD797
.LIB AD797.cir
?
By the way, you uploaded the wrong schematic.? The schematic you simulated is not the one you uploaded.
?
Andy
?
?
?
|
For tubes/valves, I always look into Radio
Designer's Handbook, because the editor was a particular expert
on them. Well-hidden in Figure 35.14, in the chapter on
communications receivers, is a current/voltage curve for a 6.3 V
0.3A heater, which is one way of powering the 12AU7 heater, both
sections in parallel. A bit of Excel work gives a resistance
trend line (for voltages between 3.0 and 6.5)? R = 0.22*V^2 +
3.61*V + 6.50. The R^2 (accuracy measure) = 0.9993, good enough
for government work. With the sections? series, the resistance
is obviously 4 times as large.
I think using this in the model will eliminate
the potentially troublesome singularity. I have to say that I
also found elsewhere resistivity/temperature data for pure
tungsten, which shows very close to a linear law, but the RDH
data above 6.5 V shows a steepish increase. Whether that is
because the heater wire is not pure tungsten, I do not, of
course, know.
--
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
|
Re: Looking for advice on TRAN timing
#FFT
Ryu,
?
See the file STEP_Sine_FFT.zip that I uploaded to the Temp folder.? It shows what happens to your waveform when you .STEP the .TRAN simulation's stop time.? When the waveforms are separated into different plot panes, you can see that part of some waveforms are missing.? That causes the FFT to process a modulated signal, unless you restrict the time interval that is passed to the FFT.? Without that step, the FFT processes the waveform over the full extent of the simulated data, which includes time where some of the .STEPs were not simulated.
?
Andy
?
|
Re: 12AU7 tube heater model
On Sat, Feb 22, 2025 at 08:46 AM, Carlo wrote:
From , you can explicitly add specific option directives on .asc schematics, then to the auto-generated netlist:
You do not need to look in the LTwiki's "undocumented" options for that.? It is standard in LTspice, in fact in all SPICE programs.? LTspice's Help is somewhat terse about it and does not show you how to add the .options command, assuming that you know how to add SPICE Directives already.? But the list of (most of the) .options choices is on the Help page for LTspice?? > Dot Commands > .OPTIONS -- Set Simulator Options.
?
.options gmin
.options gshunt
.options gfarad
.options gfloat
The correct format should be something like this:
.options gmin = 1e-14
.options gshunt = 0
.options gfarad = 1e-13
.options gfloat = 0.001
or this:
.options gmin = 1e-12 gshunt=1e-13 gfarad=1e-14
where each option is given a numerical value.
?
BTW, just few days ago, I realized that LTspice can run a netlist directly (just open the netlist and run it).
I believe that this has been somewhat restricted now, in LTspice version 24.1.? Previous versions generated a SPICE Netlist file when they ran, which was saved on your drive but deleted when LTspice is closed.? Version 24.1 no longer generates a runnable SPICE Netlist file.? I believe it can still run (process) a Netlist file if you have one, but saving one might no longer be an option.? I could be wrong.
?
Andy
?
|
Re: Build spice model of transimpedance amplifier
You could start with a current controlled voltage source. It is the H device in the list of circuit elements.
|
Re: 12AU7 tube heater model
On Fri, Feb 21, 2025 at 11:41 AM, Andy I wrote:
?
SPICE (and by extension LTspice) adds GMIN and others such as GSHUNT, GFARAD, and GFLOAT wherever they are needed, and that is done internally and they do not appear in the netlist.? That's just how it is done.? They are not explicit components
From , you can explicitly add specific option directives on .asc schematics, then to the auto-generated netlist:
?
.options gmin
.options gshunt
.options gfarad
.options gfloat
?
BTW, just few days ago, I realized that LTspice can run a netlist directly (just open the netlist and run it).
?
Carlo.
|
Re: using LTSPICE symbols for representation of spice netlist of OPAMP
Hello Andy , I am trying to implement the method you reccomended.
I have added the OPAMP2 symbol and made the include command for the ad797.cir file.
then I tried to added the spice directive script? for a wrapper but I got and error.
It says U1:22 uknown circuit node.
Where did I go wrong?
Ltspice files and error massage are attached in the ZIP.?
.SUBCKT MyAD797 In+ In- V+ V- Out
X? In+ In- V+ V- Out Decomp? AD797
.LIB AD797.cir
.ENDS MyAD797
?
?
/g/LTspice/files/Temp/22_02_25.zip
|
Re: Looking for advice on TRAN timing
#FFT
@Tony
Thank you for your answer, Tony. Is the new version available in the Files section?
I also had a look at the PDF file you mentioned.
I presume Tswp stands for sweep time, Tdel for the time you delete from the beginning,?
and Mcycles for the amount of cycles that you actually use for measuring, is that right?
?
Ryu
|
Re: Looking for advice on TRAN timing
#FFT
On Sat, Feb 22, 2025 at 12:02 AM, Ryu wrote:
One more thing that troubles me is: when I step Tstop from let's say 12m to 18m in (1m or whatever) steps and thereafter do an FFT on v(out), only the very last step is displayed as an FFT as I expect it to be . . . :-(
I am a little confused whether it works as you expected, or not as you thought and this troubles you.
?
I suspect there could be a problem doing an FFT when .STEPping Tstop, if the requested time interval is not the same in all of them.? I think the FFT is performed all at once, and that would not work unless the time interval is correct.? I think you can compensate for that by specifying a time range for the FFT that is smaller than that of the shortest .STEP, and is appropriate for the waveform's frequency.? Thus it would apply the FFT over only a portion of the saved waveforms, which is hopefully the same time interval regardless of the .STEP.
?
It looks like some of your FFT spectra in your uploaded screenshots are corrupted.? Maybe that happened because of the time interval problem described above.? The "Run: 1/2" plot in your "FFT-step Tstop 10m + 12m.png" looks particularly bad.? "Run: 1/2" in "FFT-step Tstop 12m + 18m.png" looks bad too.
?
Note it might help to turn on View > Mark Data Points, to see where the "real" spectral data is.
?
Andy
?
|
John Woodgate
Tony Casey
Carlo
aa1ww