Model and Circuit Development
What are TINA and TINA-TI?
TINA is a Spice-based circuit simulator running in the Microsoft Windows Operating system. It can do circuit DC, AC, Transient, Fourier, noise analysis, etc. TINA can be purchased through the vendor's (DesignSoft) web page located at www.tina.com.
TINA-TI is a simple version of TINA with full functionality in circuit simulation, but less circuit development utilities in the package. Also, TINA-TI contains more TI device models and TI part information. TI distributes TINA-TI free worldwide through www.ti.com/analogelab.
|Schematic entry and edit||Yes||Yes|
|Automatic/Manual wire routing and drag support||Yes||Yes|
|Instruments as standard schematic symbols||Yes||Yes|
|Integrated Net list Editor||Yes||Yes|
|Excitation Editor for arbitrary waveforms||Yes||Yes|
|Schematic Symbol Editor||Yes||Yes|
|Component Toolbar Editor||Yes||No|
|PCB export to major packages||Yes||No|
|Hierarchical and Team Design with version control||Yes||No|
|Parameter Extractor/Model Maker||Yes||No|
|Max. number of external nodes and nodes in macros||No limit||No limit|
|DC, AC, Transient, Digital, Mixed mode simulation||Yes||Yes|
|Number of components and models||20,000||837 TI IC models and 236 National models plus other supporting devices|
|Analysis directly from Net list||Yes||Yes|
|Steady State Solver (SMPS analysis)||Yes||No|
|RF models given by S-parameters||Yes||No|
|RF, Digital, VHDL, MCU Simulation||Yes||No|
|VHDL external debugger||Yes||No|
|Circuit changes while a simulation is running||Yes||No|
|Symbolic Analysis (Closed formulas)||Yes||No|
|Fourier Analysis (harmonics)||Yes||Yes|
|Fourier Analysis (spectrum)||Yes||No|
|Monte Carlo, Worst Case||Yes||Separate MC from Noise|
|Stress (Smoke) Analysis||Yes||No|
|Number of optimization targets & parameters||No limit||No|
|Number of parameters in parameter stepping||No limit||1|
|Drawing tools to enhance diagrams||Yes||Yes|
|Post processing tools||Yes||Yes|
|Smith, Nyquist, Pole-Zero Diagram||Yes||No|
|Built-in DTP tools||Yes||No|
|MathCAD and Excel export||Yes||No|
|XY Recorder, Oscilloscope, Function Generator, Multimeter, Signal Analyzer/Bode Plotter||Yes||Yes|
|Network, Spectrum, and Logic Analyzers||Yes||No|
|Digital Signal Generator||Yes||No|
|Real-time Test and Measurement||Yes||No|
What are the main differences between TINA-TI versions 7 and 9?
TINA-TI version 9 is a major upgrade of version 7. The main upgrades are in the following areas:
Can I continue using TINA-TI version 7?
Version 7 will continue to be supported on a limited basis for a short period of time. Users are encouraged to download the latest version of TINA-TI to get all the benefits of version 9.
Circuits in TINA-TI version 7 will work on version 9. But, when a circuit is saved in version 9, it cannot be opened in version 7, unless the option to save as TINA v7 Schematic is selected in the File Save dialog box, as shown below.
Back to top
Where do I get the full version of TINA version 9 or upgrade TINA-TI version 9 to the full version of TINA?
The full version of TINA can be purchased from DesignSoft on the website located at www.tina.com. Users who currently have TINA-TI version 9 installed will receive a discount on the purchase of the full version.
NOTE: Please load the program within 7 days of purchase to avoid an expired download link.Back to top
What are the minimum system requirements to run TINA-TI version 9?
The minimum hardware and software requirements for running TINA-TI version 9 are:
Where do I get TINA-TI help?
There is basic help information in the tool that is accessible through the "Help" menu.
For TI device model related questions, post your question to TI E2E Community Simulation and Models Forum.Back to top
How do I check for tool updates?
In order to check for updates, you must have TINA-TI version 9 or later.
From the menu:
The download site will appear. Follow the instructions to complete the update.Back to top
Where do I find TI device models and application circuits?
TI device models and application circuits distributed with TINA-TI. From the installation directory, TI device circuits can be found in directory (tool installation directory)\examples\. Circuits in the directory are classified by applications. For example, directory\examples\SMPS\ contains TI switchmode power supply application circuits. Directory\examples\TI test circuits\ contains all TI linear device model test circuits.
TI device models are in the "Spice Macros" tab of the upper part of the main window (device bar). See video on how to insert a device model in a circuit. (NOTE: Video viewer needed to view example.)Back to top
Can TINA-TI run a circuit from another simulator?
Yes, TINA-TI can import a circuit from another Spice simulator, but only in the form of a Spice netlist circuit. To run a Spice netlist circuit, open TINA-TI netlister from TINA's menu. Select "Tools", then "Netlist Editor". Open the circuit and run circuit analyses.
Can TINA-TI export its circuit to another simulator?
Yes, TINA-TI is PSpice compatible. A Spice netlist created in TINA-TI can run in PSpice.
From the tool's menu, select "File", then "Export", then "Netlist...". A netlist file can be created of a TINA-TI circuit and then run in PSpice.Back to top
How do I perform parametric analysis?
Step 1: Before running a parametric analysis, add desired components as parametric analysis objects. Click "Analysis" from the menu, then "Select Control Object". Mouse click the selected component, for instance, R2 and see this window:
Click the "..." button, and complete the parametric values from the next window:
Click "OK" after completing the fields in the window. The selected component is set as a parametric analysis object.
Step 2: Run circuit analysis simulation. You will see the circuit performance varies based on the selected parametric object values. See a video on how to perform parametric analysis. (NOTE: Video viewer needed to view example.)
Step 3: You can remove the component as a parametric object after running the parameter analysis by invoking the "parametric stepping" window and clicking the "Remove" button.Back to top
How can I control the simulation accuracy and speed?
Many factors affect simulation accuracy and speed. Generally, "sharp edge" signals, high error restrictions, or low GMIN will slow the simulation speed. There is a trade-off between simulation accuracy and speed. You can control simulation speed and accuracy balance by adjusting simulation parameters in the program. From the main menu, click "Analysis", then "Set Analysis Parameters...". This window will appear:
As a general rule, this setting can be used. For a circuit working at approximately 100 KHz, set "TR maximum time step" to 100ns. For a switching mode or digital circuit, TR maximum value relative error[%]" to about 1.0% to speed up simulation.
Reducing the value of "Max. no. of saved TR points" will degrade waveform display resolution but will not affect simulation accuracy. However, the simulator will save less data so the analysis waveform will display more quickly.
Click the hand button from the above window to save setting, load previous saved setting, or view the full analysis parameter list.Back to top
Can I probe a node voltage if I did not use a voltage meter prior to running the simulation?
Yes, by choosing "Save all analysis results" from the "Analysis Options" window. From the menu, select "Analysis", then "Options...". See a video on how to probe signals after simulation. (NOTE: Video viewer needed to view example.)
How do I change the simulation progress message mode?
During a simulation, TINA-TI will show the simulation progress status by percentage, message, or detailed information. You can choose one mode from the "Analysis Options" window by clicking "Analysis" from the menu, and then "Option...". In the "General" tab, select from "Trace Mode". See a video on how to choose a simulation progress message bar. (NOTE: Video viewer needed to view example.)
Does TINA-TI have a waveform measurement tool?
Yes, TINA-TI can do waveform calculation. Open the "Postprocessing" window by clicking the "add curves" icon on top of the waveform diagram window. Select the kind of function needed and the signals involved. See video on how to do waveform calculation. (NOTE: Video viewer needed to view example.)
How do I calculate a loop gain?
There are several ways to calculate a loop gain in TINA-TI, but here is a simple one. See video on how to calculate a loop gain. (NOTE: Video viewer needed to view example.)
Step 1: In the schematic window, inject a voltage source in the feedback loop with a Voltage Generator from the main menu, and set its properties as:"Signal" = "Sine wave"
Step 2: Place two Voltage Pins at the Voltage Generator terminals - Pin 1 at the positive terminal and Pin 2 at the negative terminal.
Set the Voltage Pin properties as:Pin 1: "IO state" = "Output"
. . . and . . .
Step 3: Run AC simulation. The loop gain from the positive terminal to the negative terminal of the Voltage Generator is calculated and shows the waveform display window.Back to top
How do I scale waveform in the display window?
From the waveform display window, double-click on one axis to invoke the Set Axis window.
At the bottom of the window, locate the "Round axis scale". The check box controls the signal scale display.
If the check box is unchecked, the tool calculates the scale by the entries of the upper limit, lower limit, and ticks from the Set Axis window with the following formula:
("Upper limit" - "Lower limit")
If the check box is checked, the tool sets the scale automatically to rounded numbers and ignores the entries of the upper limit, lower limit, and ticks from the Set Axis window.
For example, when the "Round axis scale" check box is unchecked in the Set Axis window, the waveform will display 7 ticks with upper limit = 86 and lower limit =
-82 as they are entered from the Set Axis window:
If the "Round axis scale" check box is checked in the Set Axis window, the waveform will display with rounded numbers and ignore the entries of the uppler limit,
lower limit, and ticks from the Set Axis window.
Can I use my own device models in TINA-TI?
If you have a Spice model, you can create a macro model for the device and use it in TINA-TI. See the question How do I create a TINA macro model from a netlist (text format) model?".
How do I create a TINA macro model from a netlist (text format) model?
TINA's full version can create a macro model from a schematic circuit (*.TSM file) and a netlist circuit (*.CIR file). TINA-TI can only create a macro model from a netlist model (*.CIR file).
Step 1: Create a Spice format sub-circuit netlist file and save as "*.CIR" file. Here is an example of a Spice sub-circuit (for a B340A diode):
subckt b340a 1 2
* model content
*... ... .ENDS
Step 2: Create a macro model with TINA's "New Macro Wizard" from the "Tools" menu.
This will open a dialog box:
Fill in the fields in the above window. In the text box for "Macro Name", enter the macro model's name. It will appear on the schematic when the model is used in a
schematic. Enter or navigate to the .CIR file for the macro. You may instead select the “From the Web” option, and use a file directly found on the Internet, for example,
from a vendor’s website. When the .CIR file is identified, click “Next” to arrive at the dialog box shown below:
Select the "Load shape from library" button to select a specific symbol from the TINA symbol database (*.DDB files) if it exists. You may then scroll through all of the
existing symbols if one applies to your part. You can filter the selections by checking “Show suggested shapes only” or by selecting “Number of pins” and “Shape type”. Or,
you can always use the auto-generated symbol for your device by selecting "Auto-generate shape". When you’ve found the symbol you want, click “Next”. You will now be
presented with this dialog:
Below the shape, you see pins that are in your macromodel netlist that are unassigned. You then associate those pins with the symbol by clicking on the pin number and
dragging it to the pin on the symbol that you want to associate with that pin number. For our example, we’ve connected the pins as shown.
When you click “Next”, you will be presented with a file dialog so you can save the macromodel where you like.
Once saved, you'll see this dialog:
Step 3: Either press the “Insert” button on the last dialog box, or, from the TINA menu anytime, select "Insert", and then "Macro...". Browse to the model file previously saved and place the macro model in the circuit.Back to top
How do I edit a device model symbol?
A device model symbol is editable by a user after it is placed on a schematic. Right click the mouse when the pointer is on the device symbol, and you will be able to edit it by selecting the edit symbol option.
The modification will only affect the current instance of the model. It has no effect on a new instance of the model from the database.Back to top
Can I create a TINA library from TINA-TI?
No, the utility is only available in the full version of TINA.