• WARNING: Tube/Valve amplifiers use potentially LETHAL HIGH VOLTAGES.
    Building, troubleshooting and testing of these amplifiers should only be
    performed by someone who is thoroughly familiar with
    the safety precautions around high voltages.

DC coupled single ended cathode follower 6SJ7/6V6 amp project

Status
This old topic is closed. If you want to reopen this topic, contact a moderator using the "Report Post" button.
Sorry to hear about the misadventure with TubeCad. Once you have LTspice running, you won't need it. Besides, there are a kazillion models available on diyAudio's very own LTspice Tube Models thread. That's where I got almost all of mine.

I probably wouldn't build this particular amp because I don't have a need for a 5W SE speaker amp. But, I definitely want to build a headphone amp along these lines using 7-pin mini tubes. I'd use something like a 6AU6A for the first stage and a 12L6 or a 12C5, into an Edcor XSE10-8K-50 (8k ohm primary, 50 ohm secondary). I only need about 0.5W output at most.

I've attached the two tube models I used in that schematic.

There are two zip files, one with the *.inc files, the other with the *.asy files.

The *.inc files go in the /lib/sub/ directory. The *.asy files go into whichever /lib/sym/ folder you put your tube symbols in.

I have mine organized in subdirectories under /sym/, as in /lib/sym/tubes/triodes/ and /lib/sym/tubes/pentodes/.
--
 

Attachments

  • Rongon_Pentodes_INC-files.zip
    1.5 KB · Views: 66
  • RongonPentodes_ASY-files.zip
    926 bytes · Views: 60
Last edited:
I stuck that .asc file into my old version (LTSpice IV) of LT spice and applied my usual "mess with it till it works" techniques. This runs in my LTSpice IV on an 8 year old W7 box installation. Take the zip file here, unzip it into a single folder and load the .asc file into LT spice. The .inc files need to be in the same directory as the .asc files, or you need to mess with environment variables such that LT spice can find them. On my W7 box just clicking on the .asc file launches LT spice with that .asc file loaded, but I probably set that up long a go and forgot about it.
 

Attachments

  • 6SJ7.zip
    5.4 KB · Views: 63
Last edited:

PRR

Member
Joined 2003
Paid Member
...trying to get the tubecad program to run on my 64 bits computer, using virtual box...

TubeCAD won't compute an arbitrary circuit, just a single standard stage. You can pretty much trust the tube datasheet charts instead. (G.E. sheets are most likely to have R-C amp tables.)

FWIW: The V 1.0.0 version of Broskie's PPCalc from 2003 *does* run in my Win7 64-bit. I suspect I am running an *installed* copy salvaged from an older machine.
 
How to Load the Tube Models From the diyAudio Ayumi Tube Library into LTspiceIV
-------------------------------------------------------------------------------

I use the older LTspiceIV, not the newer LTspiceXVI version. I don't know how well this will translate to the newer version of LTspice, but I think it will be very similar. My understanding is that they use the same models.

First, you'll want to download the Ayumi_LTspice.zip file from the "Vacuum Tube SPICE Models" thread on diyAudio.com.
(https://www.diyaudio.com/forums/tubes-valves/243950-vacuum-tube-spice-models.html#post3662623)

[Give a HUGE thanks to Ayumi Nakabayashi, kevinkr, cogsncogs, jazbo8, jackinnj, koonw, Adrian Immler, Ale Moglia, and everyone else who contributed so much to make this incredible resource available to all of us!]

You'll notice that the files in the Ayumi_LTspice.zip file all end with the three-letter file extension ".inc". Unzip the *.inc files you want to use into your LTspice \lib\sub\ folder.

You'll see there are a lot of Linear Technologies *.sub files in there already. It doesn't really matter if those files are called "something.sub" or "something.inc". They could even be "something.txt", but that could get confusing. The Ayumi models are *.inc, so we'll work with that.

1) Open Ayumi_LTspice.zip and unzip the file 6V6.inc to the LTspice \lib\sub\ folder in your system. (That's usually in the path C:\Program Files (x86)\LTC\LTspiceIV\lib\sub - but your system might be different, and I don't know what it will be like for LTspiceXVI.)

2) In Ayumi_LTspice.zip, unzip the file 6V6.asy to the /lib/sym/ folder in your system. (In my system, it's C:\Program Files (x86)\LTC\LTspiceIV\lib\sym - and under that I have a subfolder for \Tubes\, and under that I have more subfolders for \Triodes\, \Pentodes\, \Tetrodes\ and \Diodes\. So in my setup, I placed 6V6.asy into C:\Program Files (x86)\LTC\LTspiceIV\lib\sym\Tubes\Pentodes\.)

That's it! Now, the next time you open LTspiceIV, create a New Schematic, click on the Component icon. The Select Component Symbol dialog will open. Go to the top level, drill down to the level where your tube models reside, and find 6V6. Select 6V6 and click OK. The 6V6 symbol will be inserted into your schematic.

___________________________________________

PS: When you're in an LTspice Schematic, you add Components from .asy files in the folders under \lib\sym\... LTspice knows that's where they live.
Each .asy symbol file has text in it that tells it what the name of the model file is that it should load. Within 6V6.asy, there's a line that reads

SYMATTR SpiceModel 6V6.inc

This line tells LTspice to use the contents of the file 6V6.inc when it processes the .asy symbol file 6V6.asy.
--

In my models, since I have a collection of tube models made by various contributors, I change the filenames so I can keep track. I put "_AN" after the tube number if that model was made using the Ayumi Nakabayashi method. So it follows that the files for my Ayumi 6V6 model are named 6V6_AN.inc and 6V6_AN.asy, and my Ayumi 6SJ7 models are named 6SJ7_AN.inc and 6SJ7_AN.asy. Makes sense?
--
 
Last edited:
Effect of plate to plate NFB on PS Hum & Noise

Here is a worked example of the PS hum & noise problem The audio signal input is set to zero. A 10V AC signal is injected on the PS line. 10V would be typical of the guitar amp sited earlier in this thread, output tube B+ straight from the rectifier.

Without NFB the signal at the speaker terminals is 63.34 mV. With the NFB connected the signal increases to 290.4 mV. Thats 13.23 db.:eek:

May not hear the 60 & 120 Hz unable to make the trip thru a cheesy guitar amp speaker but sidebands of those would be on all the program material.:Ouch:

Need considerable care designing a PS for an amp using internal NFB such as plate to plate, same as we do with triode amps.
 

Attachments

  • 6SJ7 6V6 Amplifier without NFB Load Connected PS Interference.png
    6SJ7 6V6 Amplifier without NFB Load Connected PS Interference.png
    26.1 KB · Views: 238
  • 6SJ7 6V6 Amplifier with NFB Load Connected PS Interference.png
    6SJ7 6V6 Amplifier with NFB Load Connected PS Interference.png
    18.4 KB · Views: 219
Aw, what the heck. I'm on a roll. Here's what I've learned the various "Attribute" lines in the .asy file mean. I don't know what they all mean, but here's what I got:

Code:
SYMATTR Value 6V6GT        ; what the object will be named in the schematic
SYMATTR Prefix X               ; the type of model(?) - "X"
SYMATTR SpiceModel 6V6_AN.inc     ; Name of the spice model file to be used             
SYMATTR Value2 6V6_AN      ; the name of the model within the model file
PIN 0 -48 NONE 0             ; the location of pin 1 in the model                       
PINATTR PinName A         ; the name to be assigned to the pin 1 in the model
PINATTR SpiceOrder 1        ; 1st pin processed in the model                            
PIN 48 0 NONE 0               ; the location of pin 2 in the model
PINATTR PinName G2         ; the name to be assigned to pin 2 in the model                               
PINATTR SpiceOrder 2        ; 2nd pin processed in the model 
PIN -48 16 NONE 0            ; the location of pin 3 in the model
PINATTR PinName G1          ; the name to be assigned to pin 3 in the model                          
PINATTR SpiceOrder 3         ; 3rd pin processed in the model                             
PIN -32 64 NONE 0            ; the location of pin 4 in the model
PINATTR PinName K            ;  the name to be assigned to pin 4 in the model                         
PINATTR SpiceOrder 4         ; 4th pin processed in the model

I've found that I'll often need to edit these lines in a particular .asy file to match a new .inc (or .sub) file's parameters. For example, some creators name the pins in a pentode P G2 G1 K, while others use A G2 G1 K, and others Anode Screen Grid Cathode (corresponding to pins 1 2 3 4). You'll also have to be careful of the order of the pins. Some models specify crazy stuff like 1 4 2 3. Then you have to change the PINATTR SpiceOrder lines to match.

I hope that helps somebody. It sure drove me nuts learning that.
--
 
Last edited:
This should be stickied in an other thread !

I really appreciate the time you have spent on the design and to write this tutorial. This is what makes our community grow ! I’ve been able to run the simulation, but now I have to learn how to get results from it ahah!

Since i’ve spent so much time to make tubecad work on my computer, I think I should do like you and write something down so the other members can benefit from it.
 
Here is a worked example of the PS hum & noise problem The audio signal input is set to zero. A 10V AC signal is injected on the PS line. 10V would be typical of the guitar amp sited earlier in this thread, output tube B+ straight from the rectifier.

Without NFB the signal at the speaker terminals is 63.34 mV. With the NFB connected the signal increases to 290.4 mV. Thats 13.23 db.:eek:

May not hear the 60 & 120 Hz unable to make the trip thru a cheesy guitar amp speaker but sidebands of those would be on all the program material.:Ouch:

Need considerable care designing a PS for an amp using internal NFB such as plate to plate, same as we do with triode amps.

Now THAT is interesting!

I thought adding NFB improved PSRR.

Does this increase in psu noise present at the output only happen with this shunt feedback, but not with the more usual global NFB from the OPT secondary to input stage cathode?
--
 

PRR

Member
Joined 2003
Paid Member
...I thought adding NFB improved PSRR.....

Sometimes.

You have to understand that a transformer-loaded Pentode has high PSRR. The load may be 6k and the pentode plate resistance may be 60k. So only 1/10th of the raw ripple appears on the load. (This is another reasons pentodes stole triodes' lunch: less buzz for limited cost.)

With the NFB taken from plate, the pentode "acts like" more a triode, perhaps few-k plate resistance. Now 50%-70% of raw power buzz appears on the load, 5X-7X more buzz, in line with what jhstewart9's sims say.

Taking NFB from the secondary avoids the problem of taking NFB relative to the buzzy DC supply. This is cleaner.

OTOH, for ultimate fidelity (not just commercial fidelity) you want the raw DC to be *clean*. Even if NFB masks the buzz in the linear zone, transient overload peaks gain a haze of ripple. Of course real clean DC is not cheap.
 
I measured my output transformers and adjusted the values accordingly into the simulation. The result is a half square half sine wave with unequal spikes everywhere. Do I get those results because the circuit doesn’t fit the OPTs or because I have to enter appropriate values in order for the simulation to work properly ? Here are the measurements :

Primary : 225 dcr / 5k ohm / 2.26Hy
Secondary : 0.01 dcr / 8 ohm

Inductance measured with cheap LCR meter, I am not shure if I can trust the results, especially when considering that the simulation has a 1khz input signal and the tester probably only does DC...
 
You should be able to get a decent simulation using a pre-existing model of an OPT that's similar to the one you'll be using.

A few years ago, someone contributed an Excel spreadsheet with a good number of useful OPT models, which I've been using for simulations. (Whoever you are -- Thank you!) It won't get you an *exact* sim of your circuit, but it will allow you to get close. Once you have a simulation that looks good to you, build it and do the necessary tweaking.

I've attached the Transformer Models Rev4.xls file in a zip. I hope it proves useful.
--

PS - There's a discussion of OPT models for LTspice on the Intact Audio site:
:: View topic - Drop down transformer models for LTSpice
--
 

Attachments

  • Transformer Models Rev4.zip
    64.7 KB · Views: 64
Last edited:
Summary of Triode Output Stage

This article should help. All summed up well in the last two paragraphs.:cool:
 

Attachments

  • The Cathode Follower Output Stage p30 AA Vol 2.pdf
    502.3 KB · Views: 117
  • The Cathode Follower Output Stage p31 AA Vol 2.pdf
    794.3 KB · Views: 107
  • The Cathode Follower Output Stage p32 AA Vol 2.pdf
    698.2 KB · Views: 140
Status
This old topic is closed. If you want to reopen this topic, contact a moderator using the "Report Post" button.