The following information may have errors; It is not permissible to be read by anyone who has ever met a lawyer. Use should also be confined to Engineers with more than 370 course hours of electronic engineering and should only be used for theoretical studies. All content entered becomes and is (C)2007 Transtronics, Inc. the property of Transtronics, Inc. Rest assured that your contributions won't be sold and will be publicly available.

From Transwiki

[edit] TINA - SPICE Notes and Links

[edit] What is TINA

The first Circuit emulator I used was Electronics workbench - an old version 4.x version. It surprised me that it worked so well and I was impressed. I tried to buy a later addition and it appears that the original programmer must have left the company - the current product gave bizarre results (92V out of an opamp that was connected to only a 24 rail!) and the company refused to sell the old one to me. I returned the product and looked at many of the packages mentioned in the news groups.

I decided on TINA after trying some of the 'free' ones and think have found it a good choice. TINA is easy to learn - it has good documentation even some 'moving cursor examples of how do do certain tasks.

While I secretly hoped that TINA was named after someone's true love, it turns out that TINA stands for Toolkit for Interactive Network Analysis". TINA comes from a ten year old Hungarian company called DesignSoft. Lead by by a Dr. Mihaly Koltai, who works with 6 full time engineers plus several part time employees, DesignSoft consists of a powerful team of software end electrical engineers. This team obviously puts their hearts and much work into creating and improving TINA. Reading between the lines, I believe they may be teachers who have created this out of their love for the subject and as a teaching tool. That being said there is nothing that keeps this from being used for very advanced applications.

Dr. Mihaly Koltai was a lecturer at TUB (Technical University of Budapest) for more than 15 years and says:

"Many of the ideas in the program came from that time [at TUB]. As you say I really invented this program out of love for the topic, but TINA was always a teamwork. Today just discussing the new features with my people, reviewing the developments, listening to the customers etc. takes most of my time."

Underneath TINA is the SPICE 3F5 engine. I don't know if it has been modified - this is the same engine used in most SPICE packages today despite the great price disparities. The TINA part of the software is the user interface which you can think of as about one half of the package.

TINA comes with a Pascal-like equation language that works with graphing and will even solve systems of equations.

About the only thing I found confusing was adding parts from internet files or the parameter extractor. That is what motivated me to write this page - my own notes to myself that I share with the web. Part of my problem is that I had no earlier experience with SPICE and found that it has more new file types than I would like to have learned about<grin>.

[edit] Adding Components STEPS TO MAKE TINA ACCEPT A NEW PART

The following steps have been applied only to a discrete BJT, therefore, it is not known how the steps may differ for insertion of a sub-circuit, for example.

• Obtain from some source external to TINA, the new device's SPICE-model as a "*.LIB" file.
• Copy the new_part.LIB file into TINA's SPICELIB directory. Note: Be aware that if you do not complete this process, then try to launch TINA, it will complain of an 'imbalance' in that directory. You may correct the situation by removing new_part.LIB.
• Launch TINA's Library Manager (SLM.EXE).
• Click on its open-folder icon and open new_part.LIB.
• Pull down the LM's File menu and select 'Create TINA Library Description' ---> 'for SPICE models and subcircuits'.
• In the new window, select the appropriate radio-button and click OK. The top button worked for this BJT-task.
• The previous step has created the needed new_part.TLD file, however, the step must be completed by saving (SAVE AS, allows verification the file will be put in the SPICELIB dir) the new file.
• Close all relative windows, and launch TINA.
• TINA will complain, saying "Startup Error:...", it must re-compile the Library--let it re-compile. After that is done, there will be a new file, new_part.IND, in the SPICELIB folder.
• You may then check for the existence of the added device. Use TINA's normal tools to add the wanted shape to a TSC window, then double-click that icon as well as the ellipses at the right end of the device name/number. Find the new part in the pop-up window. This example process placed new_part in the top "Library" list-box.

If you later re-visit the SPICELIB dir, and check the 'new_part' files, you will find three related files: new_part.LIB, new_part.TLD, and new_part.IND.

[edit] How to add a symbol from a given SPICE file using TINA Pro V6? (Updated on September 30, 2007).

But first some important background information:
1. The SPICE Library Manager is SLM.EXE and it is located in the program’s folder under \Program Files\DesignSoft\Tina Pro.

2. The SPICE libraries must reside in the folder SPICELIB. This is a big problem as you cannot just copy the library file into the folder because the symbols need to register with TINA. Why is this a problem: (1) Reinstalling TINA wipes out you library files (2) You cannot transfer library files from one computer to another.
3. The SPICE file (provided by the manufacturer) needs to start with the .SUBCKT statement and end with the .ENDS statement. The SPICE file typical extension is .LIB or .SPI or .SIN or SP2 or SP3 or .MOD. It really makes no difference what the SPICE file extension is. Some manufacturers (On, TI) provide more than one SPICE model files. Given a choice, select the SPICE 2 model.
4. The .SUBCKT statement is important to understand as it defines the symbol’s pins and ties the SPICE model to the graphical shape. The syntax is:
.SUBCKT “name” “node” “node” “node” …
For example .SUBCKT OPA365 3 4 5 2 1
There must be a comment in the SPICE model text to assign the “node” to the pin of the part. In this case the notes say

• PINOUT ORDER +IN -IN +V -V OUT
  
• PINOUT ORDER 3 4 5 2 1
  

There are five steps to establish the new simulation part:
1. Obtain the SPICE model file for the part. Identify the .SUBCKT statement nodes and their pin assignment.
2. Import the symbol into a TINA library file.
3. Make the description file for the library .TLD
4. Assign a shape to the new symbol
5. Tell TINA to register the new library.

Here is the procedure for the On semiconductor part MGSF2N02ELT1 (MOSFET)
1> Obtain the MGSF2N02ELT1 SPICE model files from the manufacturer web site. In this case there are 4 files .LIB, .SIN, .SP2. .SP3.
2> Use a text editor to look inside the .SP2 file and verify that the .SUBCKT statement is there and it is terminated by an .ENDS statement.
3> Activate the application SLM.EXE > File > Collect Subcircuits and Models…> Select the work directory (of the source MGSF2N02ELT1.SP2 file) > Next > Move the file MGSF2N02ELT1.SP2 to the “Selected files:” window > Next > OK >. The SPICE macro text is shown.
4> File > Save > File name MGSF2N02ELT1.lib (save in the SPICELIB directory) > Save.
5> File > Create TINA Library Description > … for SPICE models and subcircuits > Manufacturer MGSF2N02ELT1 > OK. Two windows are displayed, one is the MGSF2N02ELT1.LIB and the other is for MGSF2N02ELT1.TLD (TLD stands for TINA Library Description).
6> File > Save as >Save as type “TINA Library Description (*.tld) > Save. There are still two windows shown.
7> Edit > TLD editor > Category NMOS > In the “Shape and Nodes” window, select the down arrow > Select the NMOS shape. OK. Verify that the pins match in the MGSF2N02ELT1.TLD file. If the do not, activate the TLD editor and move the pin definitions up and down to match them.
8> File > Save all.
9> File > Create TINA Library. This will register the changes with TINA.
10> Exit the library manager by the X icon. Resave files on the exit prompt.
11> In TINA, search for MGSF2N02ELT1.

There are three files for each library. .They all need to be in the SPICELIB directory.
.LIB is the library file made by the library manager SLM.EXE.
.TLD is the TINA Library Descriptor that contains the symbol assignment information.
The .IND in the index file for the library.

[edit] SPICE File Types (or Extensions)

TINA supports the most common standard that of the "original" PSPICE syntax only, which means that you need to find *.CIR and *.LIB file types. I have not found any conversion software for other file types (if you know of some please email me with details). Inside some of the other file types I have found parameter information that can be hand converted into *.CIR or *.LIB files. A *.cir file is a spice macro and is similar to TINA's *.TSM file.

[edit] *.CIR

A *.CIR file contains a circuit and default parameter values while a *.LIB file contains substitute part parameters for the circuit to provide several variations or models of the circuit. Thus a SPICE *.CIR file is a circuit file which contains a full circuit description, which means components (standalone components, macros, and models) along with SPICE commands. I have seen the following variations of the *.CIR naming convention: *.SPI, *.CIR.TXT, *.TXT, *.CKT, *.IN (so far - and note that I've put these in all CAPS for clarity - on many Unix systems I'm sure they are using small letter extensions). The *.CIR is also referred to as a SPICE macro or a deck (SPICE deck) in the literature dating back to when SPICE was a FORTRAN program and your circuit ran as a punch-card-deck on some main-frame.

There are really two forms of *.CIR files: one that starts with a .SUBCKT statement and ends with a .ENDS statement and a complete- circuit- file that starts with a title line and ends with an .END statement with the .SUBCKT section in between. This distinction makes a difference when opening a *.CIR file from the Tools/Netlist Editor menu or File/Import/*.CIR of TINA where it needs to be a complete-circuit-file. If you enter a macro by double clicking or right clicking and selecting enter macro from the list that appears, the Title and .END statement are not required.

Every component that can be found under the SPICE macro models tab is a SPICE subcircuit (.subckt). The other components on the tool bar- under other tabs - are built-in TINA components and some of them - actually those which are under the semiconductors tab - can be considered as SPICE models (.model). Both (.model) and (.subckt) are not to be confused with file types - they are statements found inside SPICE files.

A SPICE LIB file is usually a catalog file which contains subcircuits (.subckt) and models (.model) which can be used in any circuit.

[edit] *.SIN

*.SIN is a proprietary SPICE related file; it doesn't belong to the "original" PSPICE. There are many products on the market which use the SPICE analysis engine, and they often have file types. Some contain parameter information that may be of use in creating .LIB files.

[edit] File types in TINAs working Dir

[edit] *.SCH

SCH: TINA's native schematic file extension. They are aware of that this may conflict with other CAD programs so *.SCH will be replaced by *.TSC in the next version of TINA (V6) due to be launched soon.

[edit] TINA Pro\spicelib\

Things in the spicelib directory get loaded at startup - they can keep TINA from starting if they have errors.

[edit] *.LIB

LIB - SPICE LIBrarys

[edit] *.TLD

TLD: TINA Library Descriptor. Library descriptor files are generated by the Library Manager to add a SPICE subcircuit, model, or an S parameter model to the library. From this file TINA knows how to categorize subcircuits and how to assign a schematic-decal, know as a shape in TINA to a given subcircuit.

[edit] *.IND

IND: Library INDex file. This is a real index file for SPICE subcircuits, models, and S parameter models.

[edit] TINA Pro\CLCC\

[edit] *.LBR

LBR is the LIBrary that is formed when using the TINA parameter extractor.

[edit] *.SRC

SRC: The SouRCe file that is compiled into a CAT file. You can extend this library using the Parameter Extractor tool of TINA. This utility creates or modifies existing SRC files.

[edit] *.CAT

CAT: TINA's CATalog files. These files contain the built-in TINA components and the built-in semiconductor catalogs.

[edit] TINA Pro\

[edit] *.PRM

PRM: Analyses control PaRaMeter file. Used by Analysis. Set Parameters...to save those parameters which control the analysis in TINA.

[edit] *.DDB

DDB: TINA's shape library DataBase. It contains the shapes of the built-in components and SPICE subcircuits. A new shape can be created by the Shape Editor tool of TINA. Using this utility you can modify existing shapes or you can create a new shape for a new macro.

[edit] *.DEF

DEF ???

[edit] TINA Pro\macrolib\

[edit] *.TSM

TSM: TINA Subcircuit Macro is the extension for macros generated by TINA. If you want to create a macro you should use the Tools. New Macro Wizard... command on the main menu. Macros can be considered as SPICE subcircuits (.Subckt).

[edit] COMPREGY.INI

COMPREGY.INI: contains the Tab bar information.

[edit] *.TDR

TDR: TINA Diagram Results

[edit] *.TEQ

TEQ: TINA EQuation: ===*.MPL MPL: Internal file format, used internally for catalog files, you don't need to use an MPL files.

[edit] *.IPR

IPR: InterPReter file. Used by TINA's Interpreter (Tools. Interpreter).

[edit] *.EXA

EXA: Task list file Used in the 2 special EXAmination and training modes In these modes you can solve several exercises to train yourself by practicing problem solving and troubleshooting.

[edit] *.CPL

CPL: Complex Parameter List. Some components in TINA (for example general 2 port blocks under the Special tab) have special parameters which are described by a list of complex parameters in the form of a series of complex numbers.

[edit] *.TLC

TLC: TINA's Logic Converter utility file.

[edit] Library Flow Chart for TINA

[edit] MOSFET model parameters

[edit] Schichman-Hodges model

VTH0 threshold voltage at 27 � C
B0 Beta factor at 27 � C
l channel length modulation coefficient
RD drain resistance
RS source resistance
CGD gate-drain capacitance
CGS gate-source capacitance
JVTH temperature coefficient of the threshold voltage
JB temperature coefficient of the Beta factor

[edit] Spice Level-3 model

VTH0 zero-bias threshold voltage
Kp transconductance coefficient
2Fp surface potential
g bulk threshold parameter
Tox oxide thickness
m0 surface mobility [cm2 / Vs]
nmax maximum drift velocity
d width effect on threshold
Q mobility modulation
h static feedback
L channel length
W channel width
RD,RS,RG,RB serial resistance
RDS drain-source shunt resistance
IS bulk p�n saturation current
N bulk p�n emission coefficient
Fj bulk p�n bottom potential
CJBD0 zero-bias bulk-drain p�n capacitance
CJBS0 zero-bias bulk-source p�n capacitance
Mj bulk p�n grading coefficient
t bulk p�n transit time
CGS0 gate-source overlap capacitance/channel width
CGD0 gate-drain overlap capacitance/channel width
CGB0 gate-bulk overlap capacitance/channel length

[edit] BSIM3

Vth0
k1
k2
k3
k3b
w0
nix
vbm
dvt0
dvt1
dvt2
dvt0w
dvt1w
dvt2w
u0
ua
ub
uc
vsat
a0
ags
b0
b1
keta
a1
a2
rdsw
prwb
prwg
wr
Wint
Lint
dwg
dwb
voff
nfactor
eta0
etab
dsub
cit
cdsc
cdscb
cdscd
pclm
pdibl1
pdibl2
pdiblb
drout
pscbe1
pscbe2
pvag
delta
ngate
alpha0
beta0
rsh
js
jsw
xpart
cgsp
cgdo
cgbo
cj
cjsw
cjswg
mj
mjsw
mjswg
pb
pbsw
pbswg
nj
xti
cgsl
cgdl
cdappa
cf
clc
cle
dic
dwc
wlm
Wl
Wln
Ww
Wwn
Wwl
Ll
Lln
Lw
Lwn
Lwl
ute
kt1
kt1l
ua1
ub1
uc1
at
prt
tox
xj
gamma1
gamma2
npeak
nsub
vbx
xt
vfbcv
Lmin
Lmax
Wmin
Wmax
NoiA
NoiB
NoiC
em
af
ef
kf
mobMod
capMod
nqsMod
noiMod
binUnit

[edit] SymbEnNMOSMod1

Rds
gm

[edit] Abbreviated list of Spice file statements

[edit] Title Line

[edit] Example:

POWER AMPLIFIER CIRCUIT

The title line must be the first in the input file. Its contents are printed verbatim as the heading for each section of output.

[edit] .End line

The "End" line must always be the last in the input file. Note that the period is an integral part of the name.

[edit] Comments

[edit] Syntax:

* <comment>

[edit] Examples:

* RF=1K Gain should be 100
* Check open-loop gain and phase margin

The asterisk in the first column indicates that this line is a comment line. Comment lines may be placed anywhere in the circuit description. Note that SPICE3 also considers any line with leading white space to be a comment.

[edit] .MODEL (DEVICE MODELS)

[edit] Syntax:

.MODEL <model name> [AKO: <reference model name>]
+ <model type>
+ ([<parameter name> = <value> [tolerance specification]]*
+ [T_MEASURED=<value>] [[T_ABS=<value>] or
+ [T_REL_GLOBAL=<value>] or [T_REL_LOCAL=<value>]])

[edit] Examples: =

.MODEL RMAX RES (R=1.5 TC1=.02 TC2=.005)
.MODEL DNOM D (IS=1E-9)
.MODEL QDRIV NPN (IS=1E-7 BF=30)
.MODEL MLOAD NMOS(LEVEL=1 VTO=.7 CJ=.02pF)
.MODEL CMOD CAP (C=1 DEV 5%)
.MODEL DLOAD D (IS=1E-9 DEV .5% LOT 10%)
.MODEL RTRACK RES (R=1 DEV/GAUSS 1% LOT/UNIFORM 5%)
.MODEL QDR2 AKO:QDRIV NPN (BF=50 IKF=50m)

[edit]
Arguments and Options:

<reference model name> The model types of the current model and the AKO (A Kind Of) reference model must be the same. The value of each parameter of the referenced model is used unless overridden by the current model, e.g., for QDR2 in the last example, the value of IS derives from QDRIV, but the values of BF and IKF come from the current definition. Parameter values or formulas are transferred, but not the tolerance specification. The referenced model can be in the main circuit file, accessed through a .INC command, or it can be in a .lib file.

<model name> The model name which is used to reference a particular model, and is one of the following fifteen types:

Parameter values are defined by appending the parameter name followed by an equal sign and the parameter value. Model parameters that are not given a value are assigned the default values given below for each model type.

[edit] SUBCIRCUITS

A subcircuit that consists of SPICE elements can be defined and referenced in a fashion similar to device models. The subcircuit is defined in the input file by a grouping of element lines; the program then automatically inserts the group of elements wherever the subcircuit is referenced. There is no limit on the size or complexity of subcircuits, and subcircuits may contain other subcircuits.

[edit] .SUBCKT

[edit] Syntax:

.SUBCKT <name> [node]*
+ [OPTIONAL: < <interface node> = <default value> >*]
+ [PARAMS: < <name> = <value> >* ]
+ [TEXT: < <name> = <text value> >* ]
...
.ENDS

[edit] Examples:

.SUBCKT OPAMP 1 2 101 102 17
...
.ENDS

.SUBCKT FILTER INPUT, OUTPUT PARAMS: CENTER=100kHz,
+ BANDWIDTH=10kHz
...
.ENDS

.SUBCKT PLD IN1 IN2 IN3 OUT1
+ PARAMS: MNTYMXDLY=0 IO_LEVEL=0
+ TEXT: JEDEC_FILE="PROG.JED"
...
.ENDS

.SUBCKT 74LS00 A B Y
+ OPTIONAL: DPWR=$G_DPWR DGND=$G_DGND
+ PARAMS: MNTYMXDLY=0 IO_LEVEL=0
...
.ENDS

<name> The name is used by an X (Subcircuit Instantiation) device to reference the subcircuit.
[node]* An optional list of nodes (pins). This is optional because it is possible to specify a subcircuit that has no interface nodes. </blockquote>

The last line in a subcircuit definition is the .ENDS line. Control lines may not appear within a subcircuit definition; however, subcircuit definitions may contain anything else, including other subcircuit definitions, device models, and subcircuit calls (see below). Note that any device models or subcircuit definitions included as part of a subcircuit definition are strictly local (i.e., such models and definitions are not known outside the subcircuit definition). Also, any element nodes not included on the .SUBCKT line are strictly local, with the exception of 0 (ground) which is always global.

[edit] .ENDS (END Subcircuit)

[edit] Syntax:

.ENDS &ltSUBNAM;>

[edit] Example:

.ENDS OPAMP

The "Ends" line must be the last one for any subcircuit definition. The subcircuit name, if included, indicates which subcircuit definition is being terminated; if omitted, all subcircuits being defined are terminated. The name is needed only when nested subcircuit definitions are being made.

[edit] Xn (Subcircuit Calls)

[edit] Syntax:

XYYYYYYY N1 <N2; N3 ...> SUBNA
Where

[edit] Examples:

X1 2 4 17 3 1 MULTI

Subcircuits are used in SPICE by specifying pseudo-elements beginning with the letter X, followed by the circuit nodes to be used in expanding the subcircuit.

[edit] .LIB (Library File)

The .LIB command references a model or subcircuit library in another file.

[edit] Syntax:

.LIB [file_name]

[edit] Examples:

.LIB linear.lib
.LIB "C:\lib\bipolar.lib"

[file_name] can be any character string that is a valid file name for the computer system.

Library files can contain any combination of the following:

[edit] comments

[edit] .MODEL

[edit] subcircuit (including .ENDS )

[edit] .PARAM (Parameter) commands

[edit] .FUNC (Function) commands

[edit] .LIB commands

No other statements are allowed.

</blockquote>

[edit] ELEMENTARY DEVICES

[edit] Resistors

[edit] Syntax:

RXXXXXXX N1 N2 VALUE

[edit] Examples:

R1 1 2 100
RC1 12 17 1K

N1 and N2 are the two element nodes. VALUE is the resistance (in ohms) and may be positive or negative but not zero.

[edit] Semiconductor Resistors

[edit] Syntax:

RXXXXXXX N1 N2 <VALUE> <MNAME> <L=LENGTH> <W=WIDTH> <TEMP=T>

===== Examples: =====

RLOAD 2 10 10K
RMOD 3 7 RMODEL L=10u W=1u

must

[edit] Capacitors

[edit] Syntax:

CXXXXXXX N+ N- VALUE <IC=INCOND>

[edit] Examples:

CBYP 13 0 1UF
COSC 17 23 10U IC=3V

The (optional) initial condition is the initial (time-zero) value of capacitor voltage (in Volts). Note that the initial conditions (if any) apply 'only' if the UIC option is specified on the .TRAN control line.

SPICEhome page