********************************************************** >>Has anyone built up - or knows where I could find - some info on the >>parameters needed to build up audio valve circuits in Spice. I'd try >>myself, but the availability of accurate equivalent circuits rather >>hampers me. I'd like the 'classic' UK triodes ECC81/82/83/88 to start >>then perhaps EL34/84 etc. > >>Any help greatfully received > >>Martin > >I can't point you toward any vacuum tube SPICE models, but if >you're using MicroSim's PSPICE 5.4 or above you should be able to >roll your own using the Analog Behavioral Modeling facility, >provided you have a reference book containing the device curves. >I would imagine a piecewise-linear approximation of the V-I >characteristics would work well enough for most purposes. > >If this is applicable to your situation, and if you can't locate >the models you want directly, e-mail me if you'd like some help >with the details. > >Dave Dilatush Here's an example for the 12AU7 that I pulled of the net. I really would have liked to credit the original poster but I don't have any info saved to that effect. Hopefully we'll all get to share the fruits of the original poster's future labor on this subject. -). 12AU7: G=0.00068, mu=17. The uramp function is used to prevent negative plate current from happening. The parasitic capacitances are straight from the tube manual - and should probably be increased to account for socket and wiring capacitance. tube - a tube curve tracer emulator .options abstol=1n vntol=1n reltol=.001 vd 10 0 vg 50 0 rl 70 10 10K x1 60 50 0 12AU7 * vib is an "ammeter" for plate current (ib) vib 70 60 * * 12AU7 tube model * Connections: Plate, Grid, Cathode .subckt 12AU7 1 2 3 cgk 2 3 1.8pf cgp 2 1 1.5pf cpk 1 3 2.0pf * Grid diode model: Bg 2 3 I=0.0001*uramp(v(2,3)^1.5) * Triode model: * G mu B1 1 3 I=0.00068*(uramp(v(2,3)+(v(1,3)/17)))^1.5 .ends 12AU7 * .dc vd 0 200 1 vg -12 0 1 .end john >>Being a user of the SPICE electronic simulation software, I'm asking >>to the readers of this group if they are aware of any model simulating >>the behavior a triode? I plan to design an "hybrid" preamp, part tube/ >>part solid-state. > >Triodes can be well approximated by a power law: >I = G' x ( V' )^{x} where V' is the "equivalent grid voltage". .. which unfortunately tends to break down on the edges of the characteristic which is the interesting part that I would want SPICE modelling for. However, Marshall Leach at Georgia Tech has an article in a recent JAES in which he details the problems and presents a couple small models. He might be willing to put some sample models up on the net. --scott >Has anyone built up - or knows where I could find - some info on the >parameters needed to build up audio valve circuits in Spice. I'd try >myself, but the availability of accurate equivalent circuits rather >hampers me. I'd like the 'classic' UK triodes ECC81/82/83/88 to start >then perhaps EL34/84 etc > >Being a user of the SPICE electronic simulation software, I'm asking > >to the readers of this group if they are aware of any model simulating > >the behavior a triode? I plan to design an "hybrid" preamp, part tube/ > >part solid-state. > > Triodes can be well approximated by a power law: > > I = G' x ( V' )^{x} where V' is the "equivalent grid voltage". > > I is the total current, G' is the perveance - a constant. > The equivalent grid voltage, V' is the algebraic sum of the > voltage on the grid, V_grid, and the electric field the *plate* > sets up in the space-charge region. The latter is defined > V_plate/mu (mu being the usual amplification factor.) > We have: > V' = V_grid + V_plate/mu. > > The exponent x must be determined experimentally and it will be > in the vicinity of 3/2. No great harm is done by setting it to 3/2 > as far as I know. > > A nonlinear model can then be defined using the built-in capabilities > of Spice. > > By measuring G' and finding other relevant parameters by measuring or > in tables I think you should have enough to get started. > > Have fun. > john 015 Also check out the March 95 AES Journal article on SPICE simulations of Triodes and pentodes. Doug >Hello ! > >following an excellent article in Glass Audio about using the P-SPICE >evaluation version for tube gear, I have the following queries : > >1) Where can I find tube data sheets suitable to create more tube >P-SPICE models ? I need among other parameters : amplification factor, >internal resistance, inter-electrode capacitances, and preferably >curves (to check my model ;-) >Is the RCA manual reprint from Old Colony or others suitable for this >? >The tubes I am looking for are EF86, 5881, KT66, 6SL7, 6SN7, 300B, >you name them ! >Transformer models are also welcome if you did some ... > >2) Are some other guys there involved in *tube* equipment P-SPICE or >other-SPICE simulation ? I will be pleased to get in contact with them >. > >3) Since it was a recent query in this list, hereafter is a pointer >to some free SPICE programs over the net, if it can help someone, >the "URL" for this pointer file is : > >http://www.paranoia.com/~filipg/HTML/FAQ/BODY/F_Free_Spice.html > >Ask for a copy if you do not have a Web browser. > >X-posted to rec.audio.tubes,rec.audio.tech and sci.electronics.cad > >Note: I am just a tube amateur and a very new-bee in SPICE ! > >Regards, >- >Herve DEMARTHE %^) E-Mail: demarthe@alpha.cad.cea.fr >CEA/DSM/DRFC/STEP Tel: +33 42257527 Fax: +33 42252661 >CEN Cadarache Bt 506 13108 St Paul Lez Durance FRANCE > <<< Aprendiz de todo, Maestro de nada ... >>> Consider trying PSPICE's competitive product from Intusoft. I have been using Intusoft's ISPICE product since 1987 and has a reasonable vacuum tube models. For the professional tube circuit designer, Intusoft in conjunction with a European company has developed very accurate models for most of the popular audio tubes. These models are purchased separely for about $500 (US). Intusoft's 12AX7 (ECC83)model is resonably good and can be used for the 6SL7 tube with minor changes. The trick to using the vacuum tube SPICE models is take the bias voltages not so seriously. For example, a 250VDC powered 12AX7 stage with a 100k ohm plate resistor required over 2.2k ohms of cathode resistor bias to center the plate voltage at about half of the supply (125V). This value is higher than usually implemented. The reason for the bias calculation problem is that the characteristic curves generated by the models are not matched over all the range of tube operation. Usually the AC characteristics are good, but the DC characteristic drift depending how close to tube saturation you get. Mark, Re: Spice Models for Tubes From: wkopacz@ict.pwr.wroc.pl (Witold Kopacz) Date: 1995/11/21 Peter Mosinskis (pmosinsk@lmumail.lmu.edu) wrote: : gfp@docunet.mv.att.com (gfp) wrote: : >Has this ever been attempted? Leakage, secondary emission effects, and a : >lot of other stuff would have to be accounted for. Jerry Pulice. : Yes, this has been attempted fairly successfully, from what I understand. : Check out GLASS AUDIO magazine back issues, one has an article called : "PSPICE Models for Vacuum Tubes" or something to that effect. : Hope this helps. : Peter. Hi, I hope ,this informations helps : The Feb. and Apr. '94 "Intusoft Newsletter" had articles on modelling triodes and pentodes. They also footnoted three other references: C. Hymowitz, L.Meares, "SPICE Applications Handbook 2nd Edition", Intusoft, March 1994 Scott Reynolds, "Vacuum Tube Models For SPICE Simulations", Glass Audio, April 1993 Frederick E. Terman, "Electronic and Radio Engineering", McGraw-Hill, 1955 Intusoft also had a vacuum tube spice library for sale ($525 in June '94)-- but the tubes they mentioned didn't include any of the 4CXxxxx persuasion although they say they will develop custom models for any tube. The only articles I've seen were the in the newsletter (which I thought were very good) but I'm unfamiliar with the rest of the references so I can't comment on them. See also : > In article 'Spice model for vacuum-tube amp...' > in march # of the Journal Audio Eng. Soc. > (vol 43 #3 march 1995) I can't find the > 'L5' value in transformer's model . I have done a quick calculus, if I am not too wrong a convenient value of L5 should be around 0.04. The missing line should be: L5 5 S2 0.04 To reach the same results as in the example given by Marshall Leach in JAES you probably have to try different values of L (increase or decrease the L5 value by steps of 0.01). You have to compare your calculated amplitude and phase around 10Hz with the one given by Fig 11 in the paper. Best regards. WitKo. email: wkopacz@sequoia.ict.pwr.wroc.pl Re: SPICE Models for Tubes From: ATEC15X@email.mot.com (John Byrns) Date: 1996/04/05 MessageID: ATEC15X-050496210302@il02ara-ip189.comm.mot.com#1/1 references: <4k2bd4$6ei$1@mhade.production.compuserve.com> organization: Motorola Inc. followup-to: rec.antiques.radio+phono newsgroups: rec.antiques.radio+phono In article <4k2bd4$6ei$1@mhade.production.compuserve.com>, Ken Pedrotti <71643.2452@CompuServe.COM> wrote: > I spend a bit of time doing circuit simulation using the SPICE > circuit simulator in my work. There are, as far as I can tell, no > explicit models for tubes included in SPICE. It occurs to me that > the standard FET models could perhaps be jury rigged to give an > empirical fit to tube characteristics. I think that it would be fun > to simulate some of the old circuits. > > Does anyone know of or have a set of SPICE models that correspond to > standard tubes? > Ken, Check out the March 1995 issue of the Journal of the Audio Engineering Society (Vol.43, No.3). It contains an article by W. Marshall Leach Jr. titled "SPICE models for Vacuum-Tube Amplifiers". Included in the article are models for the 12AX7, 12AT7, and 6L6. This article, and a few data points from the spec. sheet for the tube of interest will give you a very useful model. I have modeled a number of tubes using this article. Another good article is in Glass Audio Magazine, Volume 5, Number 4, 1993, titled "Vacuum-Tube Models for PSpice Simulations", written by Scott Reynolds. In addition to the theory, this article includes models for the 12AX7, 6SN7, 12AU7, 7199, 5879, and 6SL6GC Both articles use a very similar method to model the tube. I think the Glass Audio article would be a little easier for the less technical person to read. I Found the JAES article to be more useful, it is better on the theory, but it doesn't include as many prebuilt models. Of course for antique radio tubes you are going to have to work out the parameters yourself in any case. Please post your results, when you get an old radio running in SPICE. Regards, John Byrns Intusoft has some models for vacuum tubes. Check out http://www.intusoft.com/pr/tubepr.txt Just in case, here's the document: Product: Vacuum Tube Model Library Description: Analog and mixed signal circuit design software Price: $525, directly from Intusoft, available immediately Compatibility: Any SPICE Program Contacts: Charles Hymowitz - Vice President intusoft (310) 833-0710, FAX (310) 833-9658 FAX (310) 833-9658 New SPICE Models for Vacuum Tubes Intusoft announces a new SPICE library with over 40 sophisticated vacuum tube models using a subcircuit topology newly published in Intusoft's SPICE Newsletter. The vacuum tubes models have all been characterized in a laboratory environment using actual devices. The library comes with a number of circuit examples including regulated power supplies, preamps (RIAA), amplifiers (Williamson #1 & Mullard) and vacuum tube test circuits. The library also includes generic versions of the triodes, pentodes, and heater models published in the Intusoft Newsletter, allowing users to input their own model parameters. The models may be used with Intusoft's Berkeley SPICE 3 compatible simulator to simulate RF and audio tube circuits. In addition, a tube modeling service for models not included in the library is available. Please contact Intusoft or Intusoft's distributor in France, Excem (Tel. 1-34-75-1365, Fax 1-34-75-1366), for more information and pricing. The New Vacuum Tube Library includes models for the following tubes: Valves: GZ32/5V4, GZ34/5AR4, 6AL5, 6V4 Triodes: 2A3/6A3/6B4G, 6BX7, 6DJ8/ECC88, 6SL7GT, 6SN7GTB, 6CG7/6FQ7, 6C33C-B, 12AT7/ECC81, 12AU7/ECC82, 12AX7/ECC83, 12BH7A, AB1, ED8000, 45, PX4, PX25, DA30, GL211, WE300B Small Signal Pentodes: EF86, NF2, 6SJ7GT Tetrodes and Pentodes (2 Models each, normal and triode connected): 6l6GWB/5881, 6V6GT/6AQ5, 7581, EL34/6CA7, EL84/6BQ5, KT66, KT88/6550, KT90 ****************************************************************** *EOF* -- ----------------------------------------------------------- merrigan@nyquist.ee.ualberta.ca Electrical Engineering Student University of Alberta Edmonton, Alberta, Canada -----------------------------------------------------------