Alternate spice models

[lndm]

If I want to sim a valve I don't have a model for, can I use another with similar gm and rp, or two in parallel with a similar combined gm and rp? are there other parameters that need to be considered.

I don't need absolute perfection, and I don't expect this to give accurate HF rolloff information or overload behaviour.


In an unrelated matter, does anyone know whether a 6J7 is a 'pentodised' 6J5, or is it just similar?

 

[Robert McLean]

approximate spice models

You can certainly do what you suggest, ie use the model of a similar tube, if you dont have the model for the exact tube you want, or if you dont have sufficient data to create a model for the precise tube you want.

But there is an alternative alternative. Most spec sheets give at least mu and gm (or rp, or all 3 ), at some particular operating point, ie current I at gid voltage Vg and plate volatge Vp. Given that basic information, and given the approximate equation for a triode of I = K * (mu*Vg+Vp)^x, then with a bit of calculus and algebra values for K and x can be calculated to give the desired values of gm and mu at the operating point I, Vg,Vp.

The formulas for x and K are

x = gm*(mu*Vg+Vp)/(mu*I)
and
K = I * (mu*Vg+Vp)^(-x)

if gm is not given, but rp is, then calculate gm as gm = mu/rp

if mu is not given, then just use x = 1.5, that should be close enough.

here is the resulting spice model. You mention 6J5 in your post, so I use that as an example.

Note that this is a simplified model, mu is perfectly constant, all the plate curves are perfectly parallel, so it is not completely realistic.

********************
*
* approximate model
* given mu and gm at a dc operating point I, Vp, Vg
* then parameters can be calculated for a fit at that point.
* this is useful for tubes for which there is a short form data sheet,
* but no plate curves.
*
* assuming I = K*(mu*Vg +Vp)^x,
*
* then x = gm*(mu*Vg+Vp)/(mu*I)
*
* and K = I * (mu*Vg+Vp)^(-x)
*
* default parameters are for 6J5 with mu = 20 and gm = 2600e-6
* at Vg = -8, Vp = 250, I = 9e-3
*
*
.SUBCKT Tube A G K
+ PARAMS: Mu=20 K= 2.59255e-5 x = 1.3
+ Cak=3.6p Cag=3.4p Cgk=3.4p
Bp A K I={K} * ({Mu}*V(G,K)+V(A,K))**{x}
C1 A G {Cag}
C2 A K {Cak}
C3 G K {Cgk}
.ENDS Tube


When I run this model, and a model derived from published plate curves, I find very close agreement for grid voltages in the range of -5 to -10 volts and currents of 5 to 15 mA. Even outside that range the fit is not too bad.

 

[wa2ise]

If it's a triode you need to simulate, there's "curve captor", a program that takes input from a gif file of a published characteristics curve (you do have to plot by hand many points, but the program takes it from there) and makes a variety of spice models for you. See http://sourceforge.net/projects/curvecaptor/ and this thread http://www.diyaudio.com/forums/showthread.php?s=&threadid=56327&perpage=10&pagenumber=1

But maybe I did it already, see http://home.netcom.com/~wb2jia/tubes/spice3.txt
http://home.netcom.com/~wb2jia/tubes/spice4.txt
http://home.netcom.com/~wb2jia/tubes/spice2.txt
http://home.netcom.com/~wb2jia/tubes/spice.txt

I've been using circuitmaker, a 3f4 spice simulator.

 

[lndm]

Thanks for the explainations Robert McLean, you seem to know your stuff. You've helped me to get a hold on the simplicity of some triode modelling. I'm new to the model files but your example makes it look fairly straight-forward (on a fundamental level, that is) 😉

wa2ise, I'm curious to see you've already compiled some examples. I'd like to learn the language (one day) but I feel I'd get more done if I just used pre-existing models. Can I use your text files as they are, in Circuitmaker 2k? just re-extension them as lib? or do I need to extract the model of interest?

I am initially interested in a 6J7 model and a triode strapped 46. I am inclined to use a 45 model for that, do you think I could?

Also it's good to know I could make models for anything I haven't thought of yet.

 

[lndm]

I think I'll give the tracer a try.

I have had a problem getting your models to work with my version of CM, wa2ise. Well, I've only tried the 45 as yet. It's probably just my inexperience 😉

Spice gave me an error to do with the last (8 parameter) line - parameter value out of range or wrong type.

I tried changing the pin assignments to ensure I didn't get them wrong (all 6 combos) but the message is the same for all.

BTW, I'm assuming the simmed circuit has to treat the 45 as indirectly heated and I can use the standard triode symbol.

 

[wa2ise]

My simulator is a spice 3f4 type, you may have a PSpice version, and there's more than 2 flavors. The code for one doesn't work for the others. I don't know the languages all that well, I just "hack" the code until the simulated curvetracer yields curves that look like those published. That is done by changing some of the numbers in a preexisting working model.