Norman Koren        SPICE/PSpice tube model package and instructions

---

updated August 28, 2001

These models are available as shareware. All the usual legal disclaimers apply to these models. They were developed with the best efforts of the author, who bears no legal liability for their use or misuse.

The parameters in my tube models are based on published data sheets, and are far from perfect for all cases. Tubes vary from unit-to-unit and batch-to-batch. My chief sources of tube data are Duncan's Amp Pages and Frank's Electron tube Pages.

Several files come with each PSpice model. The .dat files (complete results of a PSpice simulation used as input to Probe) are not included because they're too large and not readable.
 

August 28, 2001:  Some of these files are out of date. I'll be updating and purging them in the next few weeks. The .sch files for individual tubes are older, but should work OK.

Several commercial versions of SPICE run on personal computers, most notably PSpice from Orcad, 888-671-9500. The downloadable Pspice evaluation package has limited capabilities by standards of solid-state circuit design, but it can be amazingly useful in simulating vacuum tube amplifiers, which tend to have fewer components. All examples in this article can be run on the MicroSim Pspice evaluation package. Other well-known SPICE implementations include Electronics Workbench, 800-263-5552, and ICAP/4, from Intusoft, P.O Box 710 San Pedro, CA 90733-0710; 310-833-0710. Duncan Munro's list of SPICE vendors may contain some hidden treasures. WinSpice is a free Spice3F4 Port for Windows 95, 98, 2000 & NT. Very intriguing. It will simulate much larger circuits than evaluation PSpice.

The simulations in the accompanying files can be run on the PSpice evaluation package, which consists of Schematics for entering circuits, PSpice for simulating them, Probe for viewing the simulation results, a set of documentation and tutorials.

I'm still using Pspice version 6.3 because versions 7+ limit the total number of parts more strictly (to 50). In the newer versions, files that contain both the phono preamplifier and line amplifier (such as paspursp.sch) may need to be separated into two separate files. For those of you who run into problems with Paspursp.sch, I have included Pasphon.sch (phono only) and Paspurln.sch (line amp only).

Installing the tube and symbol libraries

After you've installed PSpice on your computer you must install or create the tube models.  Although PSpice is up to level 9.1 as I write this, I use version 6.3 for this example because I'm familiar with it and because you can also get away with a few more parts than newer versions allow. I assume you've downloaded my models. You'll need to install two files: the tube symbols (TUBE.SLB) and SPICE models (TUBE.LIB). Both are installed from the Schematics program. Installing the symbol library (TUBE.SLB)--  From the Schematics screen, click Options, Editor Configuration..., Library Settings. The screen on the right appears. Enter the foll pathname of the file containing the schematics symbols, except for the extension, in the Library Name: window, C:\NORMK\AUDIO\TubeShar\TUBE in the example. Check the box to the left of Symbol to get the .slb file extension. Click OK, OK.

Installing the SPICE model library (TUBE.LIB)-- From the Schematics Screen, click Analysis, Library and Include Files... The screen on the right appears. Enter the full pathname of the SPICE model file (including extension) in the File Name: window, C:\NORMK\AUDIO\TubeShar\TUBE.LIB in the example. Click Add Library*, OK, OK. PSpice should be ready to run with tubes!

Creating your own models

The technique for linking drawings to models is quite complex, and the PSpice tutorial must be studied to grasp it. It would be wise to look it over before continuing! The following steps will bring up a good example that can be adapted for tube models. From Schematics, click on File, Edit Library to get into the Parts Library editor. Click on File, Open..., eval.slb to open a library file that contains some parts useful as examples. (Be patient: Your screen will still be blank at this point.) Click on Part, Get..., IRF9410 to load the drawing for a P-channel mosfet. (Choose another part if you desire, but this MOSFET is as close as you can get to a tube in this library.) Click on Part, Attributes... to see the statements that define this part. For the IRF9410, they are

template=M^@refdes %d %g %s %s @MODEL
refdes=M?

PART=IRF9140
MODEL=IRF9140

template=X^@REFDES %P %G %C @MODEL
refdes=TU?
PART=12AX7
MODEL=12AX7

Parts are entered into PSpice Schematics drawings by clicking on the little box with the "and" gate. You can enter "R", "L", "C", "BUBBLE", etc. for common parts, or click on Browse... to examine a library of parts. I recommend using the rubberband option, which can be set by clicking Options, Display Options..., Rubberband. Named nodes (1G, 1P, etc.), which are created by double-clicking on lines and entering a name, are required for voltages to be examined in Probe. Input files to Schematics have the three character extension .SCH. Clicking Analysis, Create Netlist creates files with extensions .CIR (the control file), .NET (the netlist), and .ALS (an alias file which speeds up analysis) which are used as inputs to Pspice. The .CIR and .NET files contain ASCII text in SPICE format, as described in Paul Tuinenga's excellent text10. Clicking Analysis, Simulate creates the netlist, runs Pspice, and loads Probe to display results. Press the Insert key to select a voltage or current for Probe display. You can use "VDB" or "VP" to display a voltage in dB or its phase in degrees. There are many more possibilities for controlling the display.

Obtaining plate curves

To step the grid voltage, click on Analysis, Setup..., Parametric... Set Swept Var. Type to Voltage Source, Sweep Type to Linear, Name: to VG1, Start Value to 0, End Value: to -75 (or as appropriate), and Increment: to -15 (or as appropriate), then click OK. You may set the plate voltage sweep while the Analysis Setup... box is still open. Click DC Sweep... Set Swept Var. Type to Voltage Source, Sweep Type to Linear, Name: to VP, Start Value to 0, End Value: to 600 (or as appropriate), and Increment: to 5 (or as appropriate), then click OK. The DC Sweep... and Parametric boxes should contain check marks. Finally, click Close. All voltage sources except VG2NOM are set to DC=0 in the schematic diagram. (Attributes can be viewed and changed by double-clicking on the symbol.) Grid and plate voltages are controlled by the DC Sweep... and Parametric... settings.

VG2NOM is the nominal screen grid voltage. It is 300V in Figure 5 (pentode mode) and 450V in Figure 7 (ultra-linear (UL) mode). (It has no meaning in triode mode, where screen grid voltage equals the plate voltage). E2 is an EVAL voltage-controlled voltage source that controls how the screen grid voltage tracks the plate voltage. For Ultra-Linear mode it is set to V(%IN+, %IN-)*.4+V(1P)*.6 . For pentode mode it is V(%IN+, %IN-). For triode mode it is V(1P). VP is set to zero: -I(VP) is the correct polarity for plate current plotted by Probe. When you have completed entering the schematic, click Analysis, Simulate. This will create a netlist, run PSpice, and then run Probe to display the results. Error messages can appear at any one of several stages of this process. They are unavoidable when you start out. Don't get frustrated. This is where real learning happens.

Images and text copyright (C) 2000-2012 by Norman Koren. Norman Koren lives in Boulder, Colorado. Since 2003 most of his time has been devoted to the development of Imatest. He has been involved with photography since 1964.
E-mail Norman Koren | Improved Vacuum Tube Models for SPICE Simulations