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


It is currently Sep Mon 16, 2019 9:08 am


All times are UTC [ DST ]





Post New Topic Post Reply  [ 19 posts ] 
Author Message
 Post subject: Tube Amplifier Modeling Software
PostPosted: May Wed 15, 2019 7:20 pm 
Member
User avatar

Joined: Mar Sun 11, 2007 6:55 am
Posts: 10919
Location: Mission Viejo, southern California
Which tube amplifier modeling software do you recommend? Why? It would be fun to model the 6L6GB/C amplifier I built, and future projects.

_________________
many of my radios http://s269.photobucket.com/user/FSteph ... t=3&page=1


Top
 Profile  
 
 Post subject: Re: Tube Amplifier Modeling Software
PostPosted: May Wed 15, 2019 11:48 pm 
Member
User avatar

Joined: Jan Thu 01, 1970 1:00 am
Posts: 5534
Location: Montvale NJ, 07645
Ltspice. You can download tube amps for guidance.


Top
 Profile  
 
 Post subject: Re: Tube Amplifier Modeling Software
PostPosted: May Wed 15, 2019 11:59 pm 
Member
User avatar

Joined: Jul Mon 26, 2010 8:30 pm
Posts: 26378
Location: Annapolis, MD
LTSpice: +1

But: circuit simulation SW does not typically allow for non-linear component characteristics. Also, I doubt if it will deal with things like phase linearity.

To me, analysis is for getting you in the ballpark, and for dealing with pesky thinks like component ratings. Performance is determined on the test bench based on "appropriate and relevant" criteria---eg "Do it Sound Gud?"

_________________
-Mark
"Measure voltage, but THINK current." --anon.


Top
 Profile  
 
 Post subject: Re: Tube Amplifier Modeling Software
PostPosted: May Thu 16, 2019 2:59 am 
Member
User avatar

Joined: Nov Sat 26, 2011 4:09 am
Posts: 9572
Location: Texas. USA
pixellany wrote:
LTSpice: +1

But: circuit simulation SW does not typically allow for non-linear component characteristics. ...
Maybe you meant something else but all active devices are "non-linear" and that's what SPICE simulates.


Top
 Profile  
 
 Post subject: Re: Tube Amplifier Modeling Software
PostPosted: May Thu 16, 2019 3:54 am 
Member
User avatar

Joined: Jan Thu 01, 1970 1:00 am
Posts: 5008
Location: Perrysburg, OH, U.S.A.
^ +1
Indeed, there are even models for actual iron core transformers that can indicate saturation and non-liner inductance with current.
John

EDIT: Just for grins I used a SPICE model of a 6L6 and ran a simulation of the plate characteristics.
Attachment:
Nakabayashi 6L6 Model Plate Curves.jpg
Nakabayashi 6L6 Model Plate Curves.jpg [ 63.96 KiB | Viewed 671 times ]

Each curve represents grid voltages from -30v at the bottom to 0v in increments of 5v. The screen voltage was 250v as called out in the data sheet.
John

_________________
“Never attribute to malice that which can be adequately explained by stupidity.”
― R. A. Heinlein


Last edited by OldWireBender on May Thu 16, 2019 4:32 am, edited 1 time in total.

Top
 Profile  
 
 Post subject: Re: Tube Amplifier Modeling Software
PostPosted: May Thu 16, 2019 4:30 am 
Member
User avatar

Joined: Mar Sun 11, 2007 6:55 am
Posts: 10919
Location: Mission Viejo, southern California
Thank you-all!

_________________
many of my radios http://s269.photobucket.com/user/FSteph ... t=3&page=1


Top
 Profile  
 
 Post subject: Re: Tube Amplifier Modeling Software
PostPosted: May Thu 16, 2019 1:23 pm 
Member
User avatar

Joined: Jul Mon 26, 2010 8:30 pm
Posts: 26378
Location: Annapolis, MD
Flipperhome wrote:
pixellany wrote:
LTSpice: +1

But: circuit simulation SW does not typically allow for non-linear component characteristics. ...
Maybe you meant something else but all active devices are "non-linear" and that's what SPICE simulates.

Looks like I need to do my homework on Spice, but "all active devices are non-linear"?? We certainly know that real-world devices have less that ideal characteristics, but why would non-linearity be a fundamental truth?

So--in Spice--the crude model of a tube is a current source linked to an AC voltage. (Vac * Gm = Iac) There's a command to make Gm dependent on DC current?

_________________
-Mark
"Measure voltage, but THINK current." --anon.


Top
 Profile  
 
 Post subject: Re: Tube Amplifier Modeling Software
PostPosted: May Thu 16, 2019 1:45 pm 
Member
User avatar

Joined: Jul Mon 26, 2010 8:30 pm
Posts: 26378
Location: Annapolis, MD
From the Berkeley SPICE webpage:
Quote:
SPICE is a general-purpose circuit simulation program for nonlinear dc, nonlinear transient, and linear ac analyses.

emphasis in bold is mine...

Can someone translate??

_________________
-Mark
"Measure voltage, but THINK current." --anon.


Top
 Profile  
 
 Post subject: Re: Tube Amplifier Modeling Software
PostPosted: May Thu 16, 2019 2:15 pm 
Member

Joined: Oct Thu 04, 2018 2:11 pm
Posts: 127
Location: Suburban Chicago
The AC analysis part of any SPICE implementation, any of them that I have worked with anyway, will "linearize" the circuit models by solving for the DC operating points and calculating the effective gains at those points. It can then generate the frequency response of the circuit and those calculations will be accurate for signal levels that do not generate significant distortion. If you want to know what the circuit does under high signal level conditions you need to run a transient analysis instead. However well designed audio amps, for example, will behave as the linear model predicts at quite high signal levels.

More advanced simulators for professional use can use other techniques to produce accurate simulations at high signal levels nearly as quickly as a linear AC analysis can produce inaccurate results. Simulation times with transient analysis can be very long which is why it is not used exclusively. Harmonic balance is one of the techniques that are commonly used to get rapid, accurate numbers for certain kinds of analyses but there are others whose names escape me and may differ from vendor to vendor.

If you are careful to respect its limitations SPICE is an excellent tool in spite of all the nasty things Bob Pease, rest his soul, said about it. And you simply cannot beat the price of LTSpice! If you want vacuum tube models there is an excellent thread about them on DIY Audio:

https://www.diyaudio.com/forums/tubes-valves/243950-vacuum-tube-spice-models.html


Top
 Profile  
 
 Post subject: Re: Tube Amplifier Modeling Software
PostPosted: May Thu 16, 2019 2:53 pm 
Member
User avatar

Joined: Jul Mon 26, 2010 8:30 pm
Posts: 26378
Location: Annapolis, MD
Veering further off-topic.....

Different Implementations? Is there a basic core that is common to all---but some have features that are not available on others?
AKA, LTSpice is free, but adding certain features involves money?

_________________
-Mark
"Measure voltage, but THINK current." --anon.


Top
 Profile  
 
 Post subject: Re: Tube Amplifier Modeling Software
PostPosted: May Thu 16, 2019 6:55 pm 
Member
User avatar

Joined: Nov Sat 26, 2011 4:09 am
Posts: 9572
Location: Texas. USA
pixellany wrote:
Flipperhome wrote:
pixellany wrote:
LTSpice: +1

But: circuit simulation SW does not typically allow for non-linear component characteristics. ...
Maybe you meant something else but all active devices are "non-linear" and that's what SPICE simulates.

Looks like I need to do my homework on Spice, but "all active devices are non-linear"?? We certainly know that real-world devices have less that ideal characteristics, but why would non-linearity be a fundamental truth?

So--in Spice--the crude model of a tube is a current source linked to an AC voltage. (Vac * Gm = Iac) There's a command to make Gm dependent on DC current?
I don't know about "fundamental truth" but all (known) active devices are non-linear. Find a linear one and you'll probably win a Nobel prize.

The first thing you need to realize about SPICE is it isn't just 'one equation'. It's a collection of circuit analysis tools that automate what, previously, was done by hand.

The apparent point of confusion is the "Linear AC Analysis" tool but the "linear" there means the criteria under which the assumptions are valid and not a statement about the devices. Namely that the device(s) are biased into their 'active region' and the AC signal applied is small enough so that their non-linear characteristics can, to some degree, be approximated by a linear function. (Note, if your devices aren't biased properly then you need to first fix the circuit before the "Linear AC Analysis" has valid meaning.) This 'simplification' was done long before SPICE came about.

But to even get to the 'Linear AC Analysis" you have to first do a DC Analysis, and that includes the full non-linear parameters. In my case, amplifier design, I also do a "Transient Analysis," which again includes the full non-linear parameters and is what gives you the waveform graphs (you can 'probe' the circuit like you had a scope on it). In addition, I do a Fourier transform for distortion, which is based on the transient analysis. So, of the three tools I use (there are at least 6 more) only the "Linear AC Analysis" is based on the assumption of 'linear' operation (because you're trying to see what the amplifier does when it's operating properly and well within it's bounds, often referred to as "small signal analysis" {in the frequency domain}).

Your "crude" model is indeed crude and I don't know of any SPICE tube model that uses it. Doesn't mean there isn't one, I've just never seen it. For example, here's my model of a 6SN7.

Vacuum Tube Triode (Audio freq.) pkg:VT-8 (A:2,1,3)(B:5,4,6)
.SUBCKT X6SN7GTB A G K
* ANODE MODEL
BLIM LI 0 V=(URAMP(V(A)-V(K))^ 1 )* 0.0037
BGG GG 0 V=V(G)-V(K)- 0
BRP1 RP1 0 V=URAMP(-V(GG)* 0.02 )
BRP2 RP2 0 V=V(RP1)-URAMP(V(RP1)-0.999)
BRPF RP 0 V=(1-V(RP2)^ 2 )+URAMP(V(GG))* 0.002
BGR GR 0 V=URAMP(V(GG))-URAMP(-(V(GG)*(1+V(GG)* 0.006167 )))
BEM EM 0 V=URAMP(V(A)-V(K)+V(GR)* 19.2642 )
BEP EP 0 V=(V(EM)^ 1.4 )*V(RP)* 0.0000189
BEL1 EL1 0 V=URAMP(V(EP))
BEL EL 0 V=V(EL1)-URAMP(V(EL1)-V(LI))
BLD LD 0 V=URAMP(V(EP)-V(LI))
BAK A K I=V(EL)
* GRID MODEL
BGF GF 0 V=(URAMP(V(G)-V(K)- 0 )^1.5)* 0.000213
BG G K I=V(GF)+V(LD)
* CAPS
CAK A K 0.0000000000007
CGK G K 0.0000000000024
CGA G A 0.0000000000039
.ENDS X6SN7GTB

Does that look like your Vac * Gm = Iac ?

SPICE is a fantastic set of tools but you do need to know when and why their valid and when their (perhaps) not. Case in point, the 'base' simulation can give unusually low 2'nd harmonic distortion numbers for tube push pull outputs (it can happen in other circumstances too) because all components are 'perfect'. I.e. a 100k resistor is exactly 100k and all of them are the same. And all the 6L6s are the same, as is every other tube of the same type, so the circuit can be 'perfectly' balanced. That's never the case in real life since everything has tolerances. However, you can simulate that too with a Monte Carlo run, which randomly varies components within tolerances you specify. It takes forever to run though, at least on my pitiful machine, because you're doing multiple simulations to get a good distribution of random values.


Top
 Profile  
 
 Post subject: Re: Tube Amplifier Modeling Software
PostPosted: May Thu 16, 2019 7:27 pm 
Member
User avatar

Joined: Jul Mon 26, 2010 8:30 pm
Posts: 26378
Location: Annapolis, MD
Having displayed my ignorance, maybe i can recover just a little bit...:)

How about an Op-Amp? With the right set of assumptions--and some precision resistors--we can build a widget that has E(out) = k * E(in) over a wide range of conditions. In my pea brain, that is a linear device.....So, if the statement is that active devices tend to be non-linear in certain conditions, then there will be peace in the valley.

To further refine this, we'll probably need to quantify the linearity. In my Op-Amp example there is a deterministic relationship to the loop gain. With high-end audio, we typically talk about Total Harmonic Distortion, but that parameter is also related to linearity.

But perhaps the only point is that real-world analog DEVICES tend to be non-linear. That is certainly true, but can it be shown from first principles that it MUST be true?

As for SPICE, I'm not qualified. I use it, but only for really simple things.

_________________
-Mark
"Measure voltage, but THINK current." --anon.


Top
 Profile  
 
 Post subject: Re: Tube Amplifier Modeling Software
PostPosted: May Thu 16, 2019 7:28 pm 
Member
User avatar

Joined: Jan Thu 01, 1970 1:00 am
Posts: 5008
Location: Perrysburg, OH, U.S.A.
^ +1
Here's 6L6 the model I used to produce the plate characteristics:

* Generic pentode model: 6L6
* Copyright 2003--2008 by Ayumi Nakabayashi, All rights reserved.
* Version 3.10, Generated on Sat Mar 8 22:40:38 2008
* Plate
* | Screen Grid
* | | Control Grid
* | | | Cathode
* | | | |
.SUBCKT 6L6 A G2 G1 K
BGG GG 0 V=V(G1,K)+0.91804059
BM1 M1 0 V=(0.10751078*(URAMP(V(G2,K))+1e-10))**-1.743575
BM2 M2 0 V=(0.4624527*(URAMP(V(GG)+URAMP(V(G2,K))/4.9999386)))**3.243575
BP P 0 V=0.0016883841*(URAMP(V(GG)+URAMP(V(G2,K))/10.811784))**1.5
BIK IK 0 V=U(V(GG))*V(P)+(1-U(V(GG)))*0.0021948901*V(M1)*V(M2)
BIG IG 0 V=0.0022135943*URAMP(V(G1,K))**1.5*(URAMP(V(G1,K))/(URAMP(V(A,K))+URAMP(V(G1,K)))*1.2+0.4)
BIK2 IK2 0 V=V(IK,IG)*(1-0.4*(EXP(-URAMP(V(A,K))/URAMP(V(G2,K))*15)-EXP(-15)))
BIG2T IG2T 0 V=V(IK2)*(0.942171668*(1-URAMP(V(A,K))/(URAMP(V(A,K))+10))**1.5+0.057828332)
BIK3 IK3 0 V=V(IK2)*(URAMP(V(A,K))+2180)/(URAMP(V(G2,K))+2180)
BIK4 IK4 0 V=V(IK3)-URAMP(V(IK3)-(0.00056920996*(URAMP(V(A,K))+URAMP(URAMP(V(G2,K))-URAMP(V(A,K))))**1.5))
BIP IP 0 V=URAMP(V(IK4,IG2T)-URAMP(V(IK4,IG2T)-(0.00056920996*URAMP(V(A,K))**1.5)))
BIAK A K I=V(IP)+1e-10*V(A,K)
BIG2 G2 K I=URAMP(V(IK4,IP))
BIGK G1 K I=V(IG)
* CAPS
CGA G1 A 0.6p
CGK G1 K 5.7p
C12 G1 G2 3.8p
CAK A K 5.9p
.ENDS

There's even a model for the triode connected 6L6:
* Generic triode model: 6L6T
* Copyright 2003--2008 by Ayumi Nakabayashi, All rights reserved.
* Version 3.10, Generated on Sat Mar 8 22:40:38 2008
* Plate
* | Grid
* | | Cathode
* | | |
.SUBCKT 6L6T A G K
BGG GG 0 V=V(G,K)+0.91804059
BM1 M1 0 V=(0.10751078*(URAMP(V(A,K))+1e-10))^-1.743575
BM2 M2 0 V=(0.4624527*(URAMP(V(GG)+URAMP(V(A,K))/4.9999386)+1e-10))^3.243575
BP P 0 V=0.0016883841*(URAMP(V(GG)+URAMP(V(A,K))/10.811784)+1e-10)^1.5
BIK IK 0 V=U(V(GG))*V(P)+(1-U(V(GG)))*0.0021948901*V(M1)*V(M2)
BIG IG 0 V=0.0022135943*URAMP(V(G,K))^1.5*(URAMP(V(G,K))/(URAMP(V(A,K))+URAMP(V(G,K)))*1.2+0.4)
BIAK A K I=URAMP(V(IK,IG)-URAMP(V(IK,IG)-(0.00056920996*URAMP(V(A,K))^1.5)))+1e-10*V(A,K)
BIGK G K I=V(IG)
* CAPS
CGA G A 4.4p
CGK G K 5.7p
CAK A K 5.9p
.ENDS

John

_________________
“Never attribute to malice that which can be adequately explained by stupidity.”
― R. A. Heinlein


Top
 Profile  
 
 Post subject: Re: Tube Amplifier Modeling Software
PostPosted: May Thu 16, 2019 10:39 pm 
Member

Joined: Oct Thu 04, 2018 2:11 pm
Posts: 127
Location: Suburban Chicago
pixellany wrote:
Veering further off-topic.....

Different Implementations? Is there a basic core that is common to all---but some have features that are not available on others?
AKA, LTSpice is free, but adding certain features involves money?


The SPICE core was written in Fortran (I think) a long time ago at some university. Stanford perhaps? Since then it has been rewritten in more modern languages and every company that sells or gives it away adds a lot of bells and whistles to it. Almost everything you interact with on your screen when you run LTSpice was added to the core. Back in the day there were no schematic drawing tools, you did that with a pencil and paper (and probably an eraser!!). You labeled the circuit nodes carefully so that you could then type the netlist in by hand. If you needed device models you had to make them from looking at data sheets and then type them in too. The data came out in tabular form, you either developed the skill of interpreting the columns of numbers or plotted them by hand with a pencil and graph paper. The really, really advanced versions used ASCII art to print your schematic and graph your results. Tedious? Sure. But so much better than doing all that by hand. Most of us did not have weeks and weeks of time in which to solve all the differential equations with a slide rule!!

LTSpice has a nice array of features. I think it is a real gift to us that Linear Technology created and that Analog Devices assures me will be continued. If you want more or nicer features I am told there are still commercial versions available and you would have to look them up and evaluate their feature sets to see if they are worth anything to you or not. I virtually stopped looking when someone told me the price of LTSpice and once I had installed and used it for a while any thought of looking for something better vanished!

Commercial grade circuit simulators tend to use proprietary simulation engines. The one I use the most at work, ADS, is a very powerful tool for RF design but I could never justify the expense of the license for hobby use.


Top
 Profile  
 
 Post subject: Re: Tube Amplifier Modeling Software
PostPosted: May Fri 17, 2019 5:01 am 
Member
User avatar

Joined: Nov Sat 26, 2011 4:09 am
Posts: 9572
Location: Texas. USA
pixellany wrote:
Having displayed my ignorance, maybe i can recover just a little bit...:)

How about an Op-Amp? With the right set of assumptions--and some precision resistors--we can build a widget that has E(out) = k * E(in) over a wide range of conditions. In my pea brain, that is a linear device.....So, if the statement is that active devices tend to be non-linear in certain conditions, then there will be peace in the valley.

To further refine this, we'll probably need to quantify the linearity. In my Op-Amp example there is a deterministic relationship to the loop gain. With high-end audio, we typically talk about Total Harmonic Distortion, but that parameter is also related to linearity.

But perhaps the only point is that real-world analog DEVICES tend to be non-linear. That is certainly true, but can it be shown from first principles that it MUST be true?

As for SPICE, I'm not qualified. I use it, but only for really simple things.
Yes, Total Harmonic Distortion is "related to linearity" in that it measures how much it deviates from linear. In other words, it's a measure of it's non-linearity. Why would you need to measure what it doesn't have (non-linearity)? If it were truly "linear" then measuring Total Harmonic Distortion would be a waste of time.

Btw, the reason an opamp is so 'close' to linear is through the magic of negative feedback.

Part of this is a matter of 'reality' vs 'reasonable' assumptions (for the purpose to hand). Any curve can be approximated, to any arbitrary degree of accuracy, by a series of linear segments and can 'be considered linear' within each segment. Is it really linear? No. But for a specific purpose it can be 'close enough' so that we may ignore (for convenience) the non-linearity.

It's the same with the opamp. You want to 'consider it linear' because the deviation is so dern small (for your purposes), but in reality it's still non-linear. Now, for your purposes that might be a reasonable simplification (assumption) but for other applications it might not. It all depends on 'how linear' you need it to be (which is just one reason why there are so many different opamps out there).


Top
 Profile  
 
 Post subject: Re: Tube Amplifier Modeling Software
PostPosted: May Thu 23, 2019 7:53 pm 
Member

Joined: Apr Tue 17, 2012 7:58 pm
Posts: 113
Location: Metamora MI, 48455
My experiences with LTSpice and tube circuit modelling have been fairly good. The accuracy of the simulation ultimately depends on the accuracy of your tube models, and where relevant, transformers. Unfortunately, most of the tube models out there are junk. Still, a quick mock-up in LTSpice can save a lot of trouble when bench testing later.

For audio design I follow a pretty basic formula that works for me:
    Draw up a schematic using paper, pen, and a tube manual
    Model the schematic in LTSpice, and take note of any gross defects, fixing them as I go
    Construct the best version of the amplifier drawn up in LTSpice on the bench
    Run a battery of tests on the bench amplifier, and modify the LTSpice schematic according to all changes made on the prototype
    Move back to LTSpice and run Monte Carlo simulations to identify matching between critical components, make any final tweaks, and draw up a parts list for the final build

The Ayumi models are about the best for triodes, and are passable for some (but not all) of the pentodes and beam tetrodes modeled, provided that under absolutely no circumstances do you have a tube that draws meaningful current on the G1 control grid (basically anything >> than a few microamps or tens of microamps at most). Unfortunately, many of us do need to model behavior in Class AB2, Class B2, Class A2, etc

While the Ayumi models tend to give results rather close to actual tubes, they fall flat when it comes to grid current draw, which has been a problem for most tube models. In particular, the Ayumi 6F6, 6V6, and 6L6 models are garbage, and I've stopped using them.

This model for the 6L6 (I've renamed it 807 because that's my output tube of choice) is about the absolute best I've been able to find. THD from Fourier analysis, plate current draw, screen current draw, grid current draw all seem to match the published data for the 6L6 family remarkably well. As a bonus, it converges much faster than Ayumi's. Here's the code:
Code:
.subckt 807 Ax Sx Gx Kx
Ga 0 a Ax Kx 1
Ca 0 a 1n Rpar=1
Gs 0 s Sx Kx 1
Cs 0 s 1n Rpar=1
Gg 0 g Gx Kx 1
Cg 0 g 1n Rpar=1
Ba Ax Kx I= uramp(0m92*tanh(V(a)/50)*( V(a)*V(s)/7.7/(V(a)+V(s)/200) + V(g) + V(a)/140/(1+uramp(V(g)/-4)) )**1.5)
Bs Sx Kx I= 36u*uramp(V(g)+V(s)/7.9)**1.5*uramp((V(a)+64.8)/(V(a)+26.3))**3
Bg Gx Kx I= 200u*uramp(V(g))**1.5
Cak Ax Kx 7p5
Cag Ax Gx 0p2
Csg Sx Gx 6p0
Cgk Gx Kx 6p0
.ends 807

I can not, for the life of me, remember where exactly I found this model on the internet, but when I find it again I will be certain to give credit where it is due. It is not my model.

I also strongly recommend this model for triode strapped 6L6-oids; just tie the screen to the grid with a small resistance like one would in a real amplifier. The Ayumi 6L6T model is no better than the standard pentode model with regard to accuracy. I suspect he had either a bad tube, or a flaw with his tracer when gathering the curve data for his 6L6 model.


Top
 Profile  
 
 Post subject: Re: Tube Amplifier Modeling Software
PostPosted: May Thu 23, 2019 11:02 pm 
Member
User avatar

Joined: Mar Sun 11, 2007 6:55 am
Posts: 10919
Location: Mission Viejo, southern California
It is understandable that most of the focus is on designing transistor integrated circuits, but it seems odd that better tube circuit modeling software has not yet been written. Some tubes are still being made, and there quite a few thousands or tens of thousands of people world-wide interested in tube devices. Perhaps it never will be written.

_________________
many of my radios http://s269.photobucket.com/user/FSteph ... t=3&page=1


Top
 Profile  
 
 Post subject: Re: Tube Amplifier Modeling Software
PostPosted: May Fri 24, 2019 4:11 am 
Member
User avatar

Joined: Jan Thu 01, 1970 1:00 am
Posts: 5008
Location: Perrysburg, OH, U.S.A.
FStephenMasek wrote:
It is understandable that most of the focus is on designing transistor integrated circuits, but it seems odd that better tube circuit modeling software has not yet been written. Some tubes are still being made, and there quite a few thousands or tens of thousands of people world-wide interested in tube devices. Perhaps it never will be written.

The modeling software isn't the big problem. LTspice works well for this. It's the models that determine how closely the software models the actual circuit behavior. The earlier example of Vac * Gm = Iac would model a vacuum tube's behavior, but not very well. Hence the more complex example models you see posted above.

Something as simple as an incandescent lamp filament could be modeled as a simple resistor whose value is the rated voltage divided by the rated current. A standard 120v, 60W lamp could be represented by a resistor of 120v x 120v / 60W = 240 ohms. That may be good enough for certain purposes. But what if you want to model a circuit that flashes a 120v, 60W lamp? Then you'd need to have a model that took into account the cold resistance (typically one 10th of the hot operating value for a Tungsten filament) and the time constant to achieve 'full brightness'. Would, then, this be accurate enough? Or, do you need to consider that the filament supports wick away some of the heat after voltage is applied and, hence, the resistance of different parts of the filament increases at different rates? And what about radiated heat loss through the bulb itself? You can account for these things using SPICE. How accurately you can account for them is a function of the model that you use, not the program itself.

John

_________________
“Never attribute to malice that which can be adequately explained by stupidity.”
― R. A. Heinlein


Top
 Profile  
 
 Post subject: Re: Tube Amplifier Modeling Software
PostPosted: May Fri 24, 2019 4:36 pm 
Member

Joined: Apr Tue 17, 2012 7:58 pm
Posts: 113
Location: Metamora MI, 48455
To go along with previously made points, I've attached the plate characteristic of the 6L6 model I use.

Image

Compare that to the curves from the Ayumi model, and then to the published curves, and it should be immediately apparent which model is more accurate. Both models still have a major flaw though, even though the 6L6 is a "kinkless tetrode" there is still a kink in the plate characteristic, and this kink also exists for all similar tubes. Look at the 6V6, 6Y6, and 6AR6 tube data if you don't believe me. Neither model contains this "kink" which helps contribute to unrealistic THD figures. But to accurately model this "kink" would created a bloated model that isn't very useful, which leads me to my next point... The more complex the model, the more accurate it typically is, and the more computation time required. There are exceptions to this relationship between complexity and accuracy, but in general this holds.

At a certain point, the model becomes useless if the computation time becomes so long as to render simulations pointless. I deal with this all the time in my research; even using Fortran for the numerical operations and with models constructed ab initio, computation times are often extremely long, requiring hours or days, and in some cases weeks, to complete on the hardware available to me. Trying to introduce "fudge factors" to fit the results of the model to empirical data just makes the situation worse. The same can be said, albeit on a different scale, for tube models. Nobody wants to wait around for 15 minutes while a transient analysis runs on LTSpice. The tube models must converge very quickly or else the tube models themselves become useless for our needs.


Top
 Profile  
 
Post New Topic Post Reply  [ 19 posts ] 

All times are UTC [ DST ]


Who is online

Users browsing this forum: No registered users and 4 guests



Search for:
Jump to:  




























Privacy Policy :: Powered by phpBB