This part is a double dice. For now, I contoured the problem by using two JFET A units instead of one JFET with units A and B in the simulation. But I have no gain in the simulation. I also disabled all the zener diodes and replaced them with DC voltage sources in the simulation to get ride of their errors in the log.
I do suspect now that these JFET models aren't right. I have start the chapter of the book on the model creation and modifications. I will test the models following the procedures in the book first.
When you ask for the simulation files, witch one are you referring to exactly? In KiCad, the schematic file is the simulation file. One thing that is very useful is when I make a resistor adjustable in the simulation, once the right value is found, I can click the save button on the slider resistor of the simulator and the value is automatically modified into the schematic! In KiCad, all the software modules are synced. If you modify a reference value into the PCB, the schematic is updated. If you modify a library footprint in the schematic, the PCB is updated. If you modify a part in the schematic, the simulation is also update in the simulator. All that make me find the LTSpice compatibility of the KiCad simulator more attractive, but it is not as sophisticated as the real LTSpice under Windows :-/
And I hate Windows!
Here are the library files. In my simulation, I merged the whole file containing the needed models into the original LTSpice lib files. I took care to keep a backup of the original first. But this created doubles so I reverted that in the files attached.
In the files attached, only the missing models needed has been merged into the original files like this:
In my KiCad schematic, I want to use TTC004B,Q for Q503 and TTA004B,Q for Q603. These choices come from my previous project into which I was using 2SD669A and 2SB649A respectively. They were bought on eBay and they were finally a lot of trouble with oscillation. Now, seeing that I didn't find the TTC004B,Q nor the TTA004B,Q LTSpice models, I added those 2SB669A and 2SB649A models into the LTSpice library for the simulation, like this:
Thank you for the new asc file. I will tried it right now...
In the files attached, only the missing models needed has been merged into the original files like this:
standard.mos:.model 2SJ49C VDMOS(pchan Vto=-0.08 Kp=0.6 Lambda=0.1 Rs=0.55 Rd=0.1 Rds=1e7 Cgdmax=215p Cgdmin=10p a=0.25 Cgs=900p Cjo=1200p m=0.7 VJ=2.5 IS=4.0E-06 N=2.4)
standard.mos:.model 2SK134C VDMOS(nchan Vto=0.02 Kp=0.85 Lambda=0.02 Rs=0.62 Rd=0.1 Rds=1e7 Cgdmax=100p Cgdmin=5p a=0.25 Cgs=600p Cjo=1080p m=0.7 VJ=2.5 IS=4.0E-06 N=2.4)
In my KiCad schematic, I want to use TTC004B,Q for Q503 and TTA004B,Q for Q603. These choices come from my previous project into which I was using 2SD669A and 2SB649A respectively. They were bought on eBay and they were finally a lot of trouble with oscillation. Now, seeing that I didn't find the TTC004B,Q nor the TTA004B,Q LTSpice models, I added those 2SB669A and 2SB649A models into the LTSpice library for the simulation, like this:
standard.bjt:.MODEL 2SD669A NPN ( BR=0.0116 CJE=1.5E-10 CJS=0 EG=1.11 FC=0.5 IKF=0.403 IKR=1 IRB=1E-06 IS=6.73f ISC=1E-13 ISE=1.14E-14 ITF=9.99 MJC=0.407 MJE=0.33 NC=2 NE=1.04 NF=0.8 NR=1.03 RB=4 RBM=0.761 RE=0.00255 TR=0 VAF=25.1 VAR=50 VJC=0.3 VJE=0.75 VTF=1E +06 XTB=3.82 XTI=2.5 BF=3.350000E+02 CJC=6.110000E-11 RC=5.550000E-01 TF=9.010000E-10 XTF=4.450000E+01)
standard.bjt:.model 2SB649A pnp ( IS=293.5f BF=216 NF=1.0 VAF=40 IKF=1.5 ISE=101.1p NE=2.6797 BR=7 NR=1.0 VAR=20 IKR=0.05 ISC=1.345p NC=1.5558 RB=0.46 RBM=0.46 RE=5m RC=1.07 CJE=295.4p VJE=0.6977 MJE=0.5197 TF=0.8569n XTF=53.4 VTF=2.83 ITF=1.22 CJC=113.1p VJC=0.5466 MJC=0.5742 XCJC=0.5 TR=14.65n XTB=1.87 EG=1.11 XTI=3.0 FC=0.5)
Thank you for the new asc file. I will tried it right now...
The most convenient is to put all your models into a text file (like in my case minek.lib), and then
a) place the file in the same directory with your asc file and use ".lib minek.lib" directive in your asc file
or
b) place the file on some webserver, and use ".lib http://www.servername.com/lib/minek.lib" directive in your asc file.
I do b) so whoever wants to run my sims, can do it without copying any additional files
Better do not copy your own models into standard lt spice directory structure (unless you have to, e.g. for op-amps)
You can find models for TTC/TTA transistors in my minek.lib file.
a) place the file in the same directory with your asc file and use ".lib minek.lib" directive in your asc file
or
b) place the file on some webserver, and use ".lib http://www.servername.com/lib/minek.lib" directive in your asc file.
I do b) so whoever wants to run my sims, can do it without copying any additional files
Better do not copy your own models into standard lt spice directory structure (unless you have to, e.g. for op-amps)
You can find models for TTC/TTA transistors in my minek.lib file.
Good!
I am now able to get the expected results. RV1 is set at 170 Ohms with R3 at 120 Ohms for a current of 4mA into R3. RV2 is set at 379 Ohms for a current of 18mA across R505 (TP3).
I can raise the input to 1.8 Vpp and get an output of 50 Vpp without distortion. At 1.9 Vpp I start to see distortion.
I am now able to get the expected results. RV1 is set at 170 Ohms with R3 at 120 Ohms for a current of 4mA into R3. RV2 is set at 379 Ohms for a current of 18mA across R505 (TP3).
I can raise the input to 1.8 Vpp and get an output of 50 Vpp without distortion. At 1.9 Vpp I start to see distortion.
@minek123 I tried to create a lib file and I putted the file path\name in the .lib directive of the drawing but even after having restart LTSpice it doesn't see the parts when I Right-click the part schematic to replace the model. I tried a full path and a local path in the .lib directive without result. I even tried to add the Path into the preference tab.
In my previous PCB I used Exicon ECX10N20 and ECX10P20 MOSFETs. I want of course reuse them. For the simluation to be as close as the original book schematic, I kept the MOSFETs of the book but my goal is to use the Exicon MOSFET. I noticed that in your file you have similar MOSFET, named 10N20/10P20 and 10N20-75/10P20-75. The book suggest to always check models with the datasheet. Are these MOSFET have been check or created by you? Should I trust them blindly?
Thanks for all your time and help
In my previous PCB I used Exicon ECX10N20 and ECX10P20 MOSFETs. I want of course reuse them. For the simluation to be as close as the original book schematic, I kept the MOSFETs of the book but my goal is to use the Exicon MOSFET. I noticed that in your file you have similar MOSFET, named 10N20/10P20 and 10N20-75/10P20-75. The book suggest to always check models with the datasheet. Are these MOSFET have been check or created by you? Should I trust them blindly?
Thanks for all your time and help
So I am trying to reach the exact same current as those on the book schematic of Figure 9.20 and 14.17.
I got 4.0037mA across R3:
I got 9.3213mA across R303:
I got 18.346mA across R505:
But I only got 44.056mA in the source of the MOSFETs.
In the video of Bob Cordell, I remember he says that he like to push the MOSFETs to the most he can. The schematic show 200mA. I have plenty of Heat-Sink with the Dissipante_3U casing. How to I raise the current to 200mA? The only way I found was to raise R505 and R605 to something like 47K. But the wave is totally dis-formed. The original value of the book are 33 Ohms.
I got 4.0037mA across R3:
I got 9.3213mA across R303:
I got 18.346mA across R505:
But I only got 44.056mA in the source of the MOSFETs.
In the video of Bob Cordell, I remember he says that he like to push the MOSFETs to the most he can. The schematic show 200mA. I have plenty of Heat-Sink with the Dissipante_3U casing. How to I raise the current to 200mA? The only way I found was to raise R505 and R605 to something like 47K. But the wave is totally dis-formed. The original value of the book are 33 Ohms.
1) Exicon models are from Exicon. I did not define any models in minek.lib by myself.
2) If you are paralleling output device you will need to add source resistors (E.g. 0.22 Ohm)
AND you will need to match the pairs (for Vgs). This can be tricky, and you'll need more devices to select from.
If they are not matched, the amp will oscillate.
It's easier to buy double-die exicons (20N/20P), they will be factory matched, and you save space.
3) >I even tried to add the Path into the preference tab.
LT Spice will not 'see' your custom models from lib file, so you can't just select it from the list like before.
Or at least I'm not aware how to do this easily (without adding files to the LT Spice library directory).
Quick LT Spice hint on how to use models from user's lib file:
a) CTRL + Right Click on the element
b) a popup will show up, see picture attached
c) Change (manually type) the 'Value' field to some 'name' from your lib
d) Click OK
Now here is a tricky part:
In the attached example image you see 'Prefix' set to 'MN' (N channel Mosfet), that's correct, BUT
if your model in the lib file is defined using .SUBCKT keyword (e.g. for FQA36P15 mosfet in my minek.lib),
as opposed to .MODEL keyword, then you need to set prefix to 'X'.
2) If you are paralleling output device you will need to add source resistors (E.g. 0.22 Ohm)
AND you will need to match the pairs (for Vgs). This can be tricky, and you'll need more devices to select from.
If they are not matched, the amp will oscillate.
It's easier to buy double-die exicons (20N/20P), they will be factory matched, and you save space.
3) >I even tried to add the Path into the preference tab.
LT Spice will not 'see' your custom models from lib file, so you can't just select it from the list like before.
Or at least I'm not aware how to do this easily (without adding files to the LT Spice library directory).
Quick LT Spice hint on how to use models from user's lib file:
a) CTRL + Right Click on the element
b) a popup will show up, see picture attached
c) Change (manually type) the 'Value' field to some 'name' from your lib
d) Click OK
Now here is a tricky part:
In the attached example image you see 'Prefix' set to 'MN' (N channel Mosfet), that's correct, BUT
if your model in the lib file is defined using .SUBCKT keyword (e.g. for FQA36P15 mosfet in my minek.lib),
as opposed to .MODEL keyword, then you need to set prefix to 'X'.
In fact, (I am learning every day since the beginning of this project) my first goal was to make the place for the paralleling output MOSFETs. But if it is a problem to mach them, I would probably forget the option and use only one set of N and P device. That will also make it easier for the PCB. But when you say to mach them, is it something I must also be careful also if I don't the paralleling?