Forums :: Resources :: Features :: Photo Gallery :: Vintage Radio Shows :: Archives :: Books
Support This Site: Contributors :: Advertise


It is currently Sep Wed 19, 2018 2:10 pm


All times are UTC [ DST ]





Post New Topic Post Reply  [ 14 posts ] 
Author Message
 Post subject: Cathode bias voltage measurement - LTSpice simulation
PostPosted: Jan Tue 23, 2018 8:26 pm 
New Member

Joined: Apr Tue 17, 2012 7:58 pm
Posts: 21
Hello all,

I need a quick sanity check; when looking at a tube datasheet that gives plate and screen voltages for cathode bias operation, the plate and screen voltages are measured with respect to the cathode of the valves, and not with respect to ground, correct?

Say for instance push pull 6L6s, pulled straight from the circa '36 datasheet:

400 volts on the plate
300 volts on the screen

A self bias resistor of 200 ohms to give a negative bias voltage of ~25 volts

6600 ohms plate to plate load
32 watts output at 2% THD

Under these conditions the plate voltage is measure from plate to cathode, and the screen voltage is measured from screen to cathode, so the actual plate and screen supply voltages, as measured with respect to ground, should be about 425 and 325 volts respectively, no?

I think I've created a reasonable looking simulation of such an output stage in LTSpice, attached to this post. The 6L6 model is included in the netlist, so no additional libraries should be necessary to run it.

I've tried to model the output transformer somewhat realistically; I'm getting about 28.5 watts of power output at 2.23% THD measured at the load resistor, with a 1 kHz signal. Does this seem reasonable with losses in the transformer, source impedance of the power supplies, etc?


Attachments:
File comment: LTSpice schematic and netlist for 6L6 30 watt output stage
6L6_30_Watter.zip [2.12 KiB]
Downloaded 26 times
Top
 Profile  
 
 Post subject: Re: Cathode bias voltage measurement - LTSpice simulation
PostPosted: Jan Wed 24, 2018 3:40 pm 
Member
User avatar

Joined: Jan Fri 06, 2012 8:47 pm
Posts: 6421
benman94 wrote:
the plate and screen voltages are measured with respect to the cathode of the valves, and not with respect to ground, correct?
Correct. The data sheet does not care how you bias the tube, just that the relative voltages between the cathode, grid, screen and plate are as stated.
Quote:
Under these conditions the plate voltage is measure from plate to cathode, and the screen voltage is measured from screen to cathode, so the actual plate and screen supply voltages, as measured with respect to ground, should be about 425 and 325 volts respectively, no?
Correct in your case as stated where the cathode is 25 V above ground.
Quote:
I think I've created a reasonable looking simulation of such an output stage in LTSpice, attached to this post. The 6L6 model is included in the netlist, so no additional libraries should be necessary to run it.
Actually with the files you provided they can't be run without "Ayumi_Tubes.lib" . If I tried to take out the include statement it just complained about a subcircuit.

I do not have that library file and did not see one around after a quick look.

Curtis Eickerman

_________________
http://curtiseickerman.weebly.com


Top
 Profile  
 
 Post subject: Re: Cathode bias voltage measurement - LTSpice simulation
PostPosted: Jan Wed 24, 2018 9:14 pm 
Member

Joined: Jan Tue 16, 2007 7:02 am
Posts: 2546
Location: Lexington, KY USA
I don't think you should bet your life on the "self bias" or "cathode bias" voltages in the tube manual being referenced to the tube cathode, even though they are termed "Plate Voltage" or "Screen Voltage", as seen in the 1938 6L6 data.

Real consistency among manufacturers and across time may be too much to ask for.

Note, that by RC-20 (1960), RCA was saying "Plate Supply Voltage" and "Screen Supply Voltage". That seems quite clear. But is the difference a change in method, or in terminology?

Fortunately, the difference is usually not terribly large.

Ted


Top
 Profile  
 
 Post subject: Re: Cathode bias voltage measurement - LTSpice simulation
PostPosted: Jan Wed 24, 2018 10:46 pm 
Member

Joined: Jul Wed 22, 2009 3:07 pm
Posts: 716
Eickerman wrote:
...
Actually with the files you provided they can't be run without "Ayumi_Tubes.lib" . If I tried to take out the include statement it just complained about a subcircuit.

I do not have that library file and did not see one around after a quick look.
...

Hi Curtis,

The .net file included in the zip folder by the OP has the Ayumi model in it, you can extract it (with a text editor) from there.
Also, the Duncan's Amp Pages have various models for the 6L6:
http://www.duncanamps.com/spicemodels.html

The Ayumi models were discussed in the LTspice Yahoo Group around '14 October, at least that is the date of my file. It has a different name, my file/folder is called "pctube_1.11_win". I can mail it to you if you require.
The most interesting was the method Ayumi used to fit the models. In the Yahoo Group discussions I had a link to his web-page (it also required translation). I do not know if those pages are still around, probably still can be found in the web archive...
One difference that required "wholesale" modification in his files was to change the exponent operator from "^" to "**" that LTspice understands.

The Ayumi models are probably in the file section of the Yahoo Group too.

Regards, Peter


Top
 Profile  
 
 Post subject: Re: Cathode bias voltage measurement - LTSpice simulation
PostPosted: Jan Wed 24, 2018 11:20 pm 
Member
User avatar

Joined: Jan Fri 06, 2012 8:47 pm
Posts: 6421
orbanp wrote:
The .net file included in the zip folder by the OP has the Ayumi model in it, you can extract it (with a text editor) from there.
Peter, I looked at the .net file and see the model inside of it.

However, there is an inc. statement in the .asc file that tries to open the .lib file. If I remove that statement and try to run the simulation it just complains about xu1 in the .net file. At that point I gave up. I am not a LTSpice guru.

I can see the circuit (rearranged slightly for better visibility)...
Attachment:
1.jpg
1.jpg [ 133.25 KiB | Viewed 888 times ]
Then I tried to run the simulation without changing anything and got this...
Attachment:
2.jpg
2.jpg [ 16.18 KiB | Viewed 888 times ]
So I noticed the 6L6 model is "inside" of the .net file so I figure the .lib should not be needed and I removed the .inc statement and got this...
Attachment:
3.jpg
3.jpg [ 16.29 KiB | Viewed 888 times ]
This is all probably painfully obvious to a power LTSpice user, but not to me. :shock:

Curtis Eickerman

_________________
http://curtiseickerman.weebly.com


Top
 Profile  
 
 Post subject: Re: Cathode bias voltage measurement - LTSpice simulation
PostPosted: Jan Wed 24, 2018 11:59 pm 
Member

Joined: Jul Wed 22, 2009 3:07 pm
Posts: 716
Hi Curtis,

Extract the 6L6 model with a text editor into a separate text file, name it to Ayumi_Tubes.lib (make sure the file extension is not .txt, but .lib, rename the extension to .lib if the system puts a .txt extension to it!).
The first extracted line starts with the "*", above the "* Generic pentode model: 6L6..." line.
(Lines starting with a "*" are comments.)
The last extracted line is the line starting with ".ENDS".

Put that .lib file into the same folder where the circuit is (the "30_Watt_6L6.asc" file).
That should do it!

Regards, Peter


Top
 Profile  
 
 Post subject: Re: Cathode bias voltage measurement - LTSpice simulation
PostPosted: Jan Thu 25, 2018 3:45 pm 
Member
User avatar

Joined: Jan Fri 06, 2012 8:47 pm
Posts: 6421
orbanp wrote:
Put that .lib file into the same folder where the circuit is (the "30_Watt_6L6.asc" file). That should do it!
Peter, thank you. That worked. Everything stopped complaining and the simulation runs.

So would a Ayumi_Tubes.lib be a single file that contains all of the Ayumi models within the same file? Not sure what the proper Syntax should be if that were done (guessing only one END statement at the very end?).

To see what happens I set the two inputs to 1 V p-p at 1 KHz and the output was also at 1 V p-p into the load. It also looked like the transient on the cathode settled out at about 150 mS so I cut short the 500 mS delay to 150 mS in presenting data and then shortened the simulation to end a 200 mS (didn't need 500 mS of 1 KHz sine waves).

Curtis Eickerman

_________________
http://curtiseickerman.weebly.com


Top
 Profile  
 
 Post subject: Re: Cathode bias voltage measurement - LTSpice simulation
PostPosted: Jan Thu 25, 2018 10:15 pm 
Member

Joined: Jul Wed 22, 2009 3:07 pm
Posts: 716
Hi Curtis,

Glad the simulation is working for you!
I also cleaned up the simulation a bit, except I did not want to reply just with the simulation results.

An interesting finding while "cleaning up" the simulation. When reducing the long fractional numbers, I truncated the coupling ratio of the output transformer to 0.99, the distortion was more than 8% with 15V input signal (about 8W output). When changing the coupling ratio to 1 (or back to that long fractional number that the OP used), the distortion went down below 1%!
Mike Engelhart, the author of LTspice, has a two page document on transformer modeling on the Linear web-site, but that did not make clear to me (after only one reading) why this sudden change in distortion.

The Duncan web-site has a few output transformer models, except no detailed explanations.

I have the Ayumi tube models downloaded as a zip file, with the individual .inc model files in them (.inc and .lib are totally equivalent in LTspice, no difference whatsoever how they are treated in LTspice).
I only extracted the model I required at that time, I was modeling the circuit of the HP-400 AC mV-meter.
It looks like someone extracted all the models, merged them into a single file, named it "Ayumi_Tubes.lib", and possibly converted the exponent syntax.

The simulation looks for the model in the included file, it is looking for the line ".SUBCKT _Name_..." where the _Name_ is the name of the component.
If you CTRL-right-click on the tube symbol in the simulation schematics, the attribute window of the tube symbol comes up, the name of the component is in the "Value" attribute entry. That has to match _Name_ in the .SUBCKT line in the file.
If the simulation does not find the included file you get the error message that the file could not be found, or if there is no included file, or the _Name_ can not be found in the included file, than you get the error message about the unknown subcircuit.

Regards, Peter


Top
 Profile  
 
 Post subject: Re: Cathode bias voltage measurement - LTSpice simulation
PostPosted: Jan Thu 25, 2018 10:27 pm 
Member
User avatar

Joined: Jan Fri 06, 2012 8:47 pm
Posts: 6421
orbanp wrote:
An interesting finding while "cleaning up" the simulation. When reducing the long fractional numbers, I truncated the coupling ratio of the output transformer to 0.99, the distortion was more than 8% with 15V input signal (about 8W output). When changing the coupling ratio to 1 (or back to that long fractional number that the OP used), the distortion went down below 1%!
That definitely would be a surprise to me as well. When modeling power supplies where I didn't really care about % distortion or actual coupling factor I have just used 1. That makes me wonder what happens if I drop back to .99 on those as well. I wonder if in some way the transformer is making up for distortion in the tube. If I recall correctly the 6V6 in push pull is only supposed to be good for about 3% or a little higher THD.

Curtis Eickerman

_________________
http://curtiseickerman.weebly.com


Top
 Profile  
 
 Post subject: Re: Cathode bias voltage measurement - LTSpice simulation
PostPosted: Jan Thu 25, 2018 10:46 pm 
Member
User avatar

Joined: Nov Sat 26, 2011 4:09 am
Posts: 9021
Location: Texas. USA
Eickerman wrote:
orbanp wrote:
An interesting finding while "cleaning up" the simulation. When reducing the long fractional numbers, I truncated the coupling ratio of the output transformer to 0.99, the distortion was more than 8% with 15V input signal (about 8W output). When changing the coupling ratio to 1 (or back to that long fractional number that the OP used), the distortion went down below 1%!
That definitely would be a surprise to me as well. When modeling power supplies where I didn't really care about % distortion or actual coupling factor I have just used 1. That makes me wonder what happens if I drop back to .99 on those as well. I wonder if in some way the transformer is making up for distortion in the tube. If I recall correctly the 6V6 in push pull is only supposed to be good for about 3% or a little higher THD.

Curtis Eickerman
I always take SPICE distortion numbers with a grain of salt because, IMO, they can be overly optimistic. For one, with a push-pull circuit, for example, all the components are 'identical' (unless you do a full Monte Carlo simulation) and the 2'nd harmonic (almost) perfectly cancels. That's not a real world result where values are never 'exact' (and that includes the tubes themselves). There are other 'coincidental' anomalies that can occur but you get the drift.


Top
 Profile  
 
 Post subject: Re: Cathode bias voltage measurement - LTSpice simulation
PostPosted: Jan Thu 25, 2018 11:11 pm 
Member
User avatar

Joined: Jan Fri 06, 2012 8:47 pm
Posts: 6421
orbanp wrote:
An interesting finding while "cleaning up" the simulation. When reducing the long fractional numbers, I truncated the coupling ratio of the output transformer to 0.99, the distortion was more than 8% with 15V input signal (about 8W output). When changing the coupling ratio to 1 (or back to that long fractional number that the OP used), the distortion went down below 1%!
I tried it.

I drove it with 16 V and had it producing about 12 Watts output at just barely under 1% (which the tube really can't do according to specs). Then I changed the coupling to .99 and darn near had triangle waves instead of sine waves at 1 KHz. The Distortion went up to 10%.

I wonder if that is real, or just an artifact of the model of either the tube or transformer? I am kind of guessing it is more an artifact of the modeling.

Curtis Eickerman

_________________
http://curtiseickerman.weebly.com


Top
 Profile  
 
 Post subject: Re: Cathode bias voltage measurement - LTSpice simulation
PostPosted: Jan Thu 25, 2018 11:16 pm 
Member
User avatar

Joined: Jan Fri 06, 2012 8:47 pm
Posts: 6421
Flipperhome wrote:
I always take SPICE distortion numbers with a grain of salt because, IMO, they can be overly optimistic.
I would generally agree with that.

Interestingly if I use a coupling factor on the transformer of .995 I get about 3.5% THD which is a reasonable approximation of what you actually might get with 6V6 in push pull at that power level.

Also, as noted, the worst case even harmonic is about 90 dB down from the fundamental which is probably unrealistic. In the simulation the tubes are "perfectly" matched which never happens.

Curtis Eickerman

_________________
http://curtiseickerman.weebly.com


Top
 Profile  
 
 Post subject: Re: Cathode bias voltage measurement - LTSpice simulation
PostPosted: Feb Sun 11, 2018 9:11 pm 
New Member

Joined: Apr Tue 17, 2012 7:58 pm
Posts: 21
Sorry for the long delay in responding. Other things in life came up...

I apologize for that mess I zipped up. Those were old "working versions" of the schematics I was playing with. I had cleaned up schematics with the tube models right in the netlist ready to go. I zipped up the wrong files by mistake.

Anyway, I too think the LTSpice simulations give rather optimistic results for distortion. Real tubes are never that well matched, a real OPT will never have primary windings that closely matched, resistors never perfectly match, etc. Still, it is a reasonable tool for ensuring that a circuit will work before you start punching holes in a chassis. You could also figure out rough operating points and rough estimates of distortion, gain, phase shift, etc via paper and pencil, but I can draw up an entire amp schematic in 10-15 minutes and play with it to my hearts content in LTSpice. It's just more efficient.

I was using a calculator provided by someone on the diyaudio forum to create a very rough but reasonable model of an output transformer, thus the strange values. If you keep the longer values for inductance and the coupling coefficient, you'll find that the transformer has particular -3 dB points at the high and low end as determined by the calculator. While his model can't account for core saturation or some of the parasitic effects, it does a decent job modelling an output transformer below clipping and within the power rating of the output transformer.

For a quick sanity check, I recently modeled this little push pull 6AS7G amplifier. I had already worked out the operating points of each of the stages and the power supply before hand on paper in order to check it against the LTSpice model. The model is very close to expected real behavior. RCA quoted 2% THD at 10 watts for a push pull 6AS7G at these voltages. I'm getting 2.57% THD at the output including the preceding Van Scoyoc input/phase splitter and the 6SN7 driver stage.

I had to cheat a little bit and model the power transformer as a 1:1 transformer with the primary side supplying 700 volts rms and thus each half of the secondary seeing 350 volts rms. I couldn't get a normal transformer with a 120 volts rms primary to work properly; this seems to work well enough.

In the zipped file you'll find the schematic. This time the necessary tube models should be visible right on the schematic as one big directive statement. The amplitude and frequency for transient analysis are entered as parameter statements.


Attachments:
File comment: LTSpice Schematic for 10 watt 6AS7G amplifier
6AS7_10_Watter_Cleaned_Up.zip [2.66 KiB]
Downloaded 18 times
Top
 Profile  
 
 Post subject: Re: Cathode bias voltage measurement - LTSpice simulation
PostPosted: Feb Tue 20, 2018 4:19 am 
Member

Joined: Jun Mon 24, 2013 3:00 pm
Posts: 1128
Location: Champaign IL 61822
Someone mentioned a tube data handbook listing "supply voltages".

The RCA books do list those sometimes, especially for resistance coupled
amps. They normally mean exactly that. For example, it might list a screen supply voltage
of 250 volts and a 33K resistor in series with the screen, with or without
a bypass cap.

Sometimes the supply voltages are listed as max with a certain resistor size.

In most cases its not reasonable to use a plate supply voltage of say 3000 volts
on a 6SN7 with a series resistor setting the max current at say 2 ma ... but people did that
for vertical output tubes of electrostatic deflection TVs.


Top
 Profile  
 
Post New Topic Post Reply  [ 14 posts ] 

All times are UTC [ DST ]


Who is online

Users browsing this forum: No registered users and 3 guests



Search for:
Jump to:  
























Privacy Policy :: Powered by phpBB