ESim/C2/Creating-a-Device-Model/English-timed
From Script | Spoken-Tutorial
| Time | Narration |
| 00:01 | Welcome to the spoken tutorial on Creating a Device Model in eSim. |
| 00:08 | In this tutorial, using eSim we will learn - |
| 00:12 | To create a Germanium Diode from an existing Device Model and |
| 00:17 | To edit a current Device Model. |
| 00:21 | To record this tutorial, we will use- |
| 00:25 | Ubuntu Linux OS version 16.04 and |
| 00:30 | eSim version 2.0 |
| 00:34 | To practice this tutorial, you should know to-
create a circuit schematic and simulate the netlist file in eSim. |
| 00:43 | If not, watch the prerequisite eSim tutorials on this website. |
| 00:49 | The device model file begins with a dot model statement. |
| 00:54 | mname indicates the model name like diode model N4007, 1N4148. |
| 01:04 | Component type indicates the type of model used. |
| 01:09 | For example: D is used for Diode, M for MOSFET,and NPN or PNP for BJT. |
| 01:19 | pname is the parameter name and |
| 01:22 | pval is the parameter value. |
| 01:26 | The model components are already added in eSim. |
| 01:31 | They are referred to as templates. |
| 01:34 | The templates are in a tabular form with parameter names and values. |
| 01:40 | The Device Model libraries are used for the components present in eSim underscore Devices. |
| 01:48 | To launch eSim, you need to double-click on the eSim icon on your Desktop. |
| 01:54 | I have already opened eSim. |
| 01:57 | Let us now create a Device model of a Germanium diode 1N34A. |
| 02:04 | On the eSim window, click on the Model Editor button from the left toolbar. |
| 02:11 | The Model Editor tab opens. |
| 02:15 | Click the New button in the Model Editor tab. |
| 02:19 | A New Model pop-up window appears. |
| 02:23 | Type the Model Name as Germanium underscore Diode.
Click on the OK button. |
| 02:31 | A list of model components appears on the left corner of the Model Editor tab. |
| 02:38 | These are the models you can choose from. |
| 02:42 | Since we are creating a new model of a Diode, click on Diode. |
| 02:48 | The diode model opens up in a tabular form with the Parameter name and value. |
| 02:55 | You can see the default values. |
| 02:59 | Let us now add the spice parameters of Germanium diode. |
| 03:05 | The parameters of Germanium Diode model 1N34A can also be downloaded from the Code File section. |
| 03:14 | Download and open the file in a text editor. |
| 03:18 | Copy-paste the parameter values in the respective text-box in the Model Editor window. |
| 03:26 | Here I am entering the values. |
| 03:29 | To enter a value, click on the value field. |
| 03:34 | Enter Rs as 7. |
| 03:36 | Enter Cjo as 0.5 exponential minus 12. |
| 03:42 | Enter N as 1.3. |
| 03:46 | Enter Ibv as 0.018. |
| 03:52 | Enter tt as 144 exponential minus 9. |
| 03:59 | Enter M as 0.27. |
| 04:04 | Enter Vj as 0.1. |
| 04:09 | Enter Is as 2.0 exponential minus 7. |
| 04:15 | Enter Bv as 75. |
| 04:19 | The sequence of parameters may vary. |
| 04:23 | You can also add or delete the parameter. |
| 04:28 | After the parameters are entered, click on the Save button in the Model editor tab. |
| 04:35 | An information pop-up window, 'Model saved successfully' is displayed. |
| 04:41 | Click on the OK button. |
| 04:44 | These libraries will be saved in the Diode folder of deviceModelLibrary directory. |
| 04:52 | If the component model was chosen as BJT, then the library would be saved in the Transistor folder. |
| 05:02 | Each template chosen will be saved in their respective folders of deviceModelLibrary directory. |
| 05:11 | Now let us simulate the characteristics of Germanium Diode. |
| 05:16 | We will open the Diode characteristic example from the Examples folder of eSim. |
| 05:24 | On the eSim window, click on the Open Project button from the top menu. |
| 05:31 | Locate the directory where the eSim is installed. |
| 05:36 | Double-click on the Examples folder. |
| 05:40 | Scroll down and select the Diode underscore characteristics. |
| 05:45 | Click on the Open button. |
| 05:48 | The Diode characteristics example is added to the eSim window under Projects. |
| 05:55 | To see the schematic, select Diode characteristics. |
| 06:00 | Click on the Open Schematic button from the left toolbar. |
| 06:05 | It directs us to the schematic editor. |
| 06:09 | Press F1 key to zoom in the schematic. |
| 06:14 | Let us go back to the eSim window. |
| 06:18 | Select the Diode underscore characteristics. |
| 06:22 | Click on the Convert Kicad to Ngspice button from the left toolbar. |
| 06:28 | Select DC in the Analysis tab. |
| 06:33 | Scroll down to enter values. |
| 06:37 | Enter Source as V1. |
| 06:41 | Enter Start as 0. |
| 06:45 | Enter Increment as 0.1. |
| 06:50 | Enter Stop as 2. |
| 06:53 | In the Source Details tab, enter value as 1. |
| 06:59 | Skip the Ngspice Model tab. |
| 07:02 | Click on the 'Device Modeling tab, click on the ADD button. |
| 07:08 | Double-click on the Diode folder. |
| 07:11 | Select Germanium underscore Diode dot lib file. |
| 07:16 | Click on the Open button. |
| 07:19 | This adds the Germanium Diode library file from the Diode folder. |
| 07:25 | On the Kicad to Ngspice tab, click on the Convert button. |
| 07:31 | Click on the OK button in the Information dialog box. |
| 07:36 | Now, let us simulate the Ngspice netlist. |
| 07:41 | On the eSim window, click on the Simulation button from the left toolbar. |
| 07:48 | An Ngspice terminal and plot window opens along with a Python plot window. |
| 07:55 | The plot waveforms show DC analysis of the Germanium Diode model 1N34A. |
| 08:04 | This diode has a knee voltage or turn-on voltage around 0.3. |
| 08:10 | The forward current is around 1.7 milliampere. |
| 08:15 | Close the Ngspice plot and Ngspice terminal windows. |
| 08:20 | In the Python plot window, check the In node and Out node.
And click on the Plot button. |
| 08:28 | You can see the forward characteristics of the Germanium diode. |
| 08:33 | Close the Python plot window. |
| 08:36 | The Shockley diode equation relates the diode current I with the diode voltage Vd. |
| 08:43 | The main spice parameters that determine the DC analysis are
emission coefficient n, saturation current Is and ohmic resistance Rs. |
| 08:59 | For an ideal diode, N is equal to 1. |
| 09:03 | This factor mainly accounts for carrier recombination. |
| 09:09 | Now let us learn how to edit a model library. |
| 09:14 | On the eSim window, click on the 'Model editor button from the left toolbar. |
| 09:20 | We will edit the Germanium diode parameters. |
| 09:25 | On the Model editor tab, click on the Edit button. |
| 09:30 | Double-click on the Diode folder. |
| 09:34 | Select Germanium underscore diode dot lib file. |
| 09:39 | Click on the Open button. |
| 09:42 | A tabular form of Germanium Diode parameters and its corresponding values will appear. |
| 09:50 | Let us now change the value of the parameter N . |
| 09:55 | Click on the parameter N Value field and enter 4. |
| 10:01 | Click on the SAVE button in the Model editor tab. |
| 10:06 | In the Information dialog box, click on the OK button. |
| 10:11 | Let us now simulate the characteristics. |
| 10:15 | On the eSim window, select Diode underscore Characteristics. |
| 10:21 | Click on Convert Kicad to Ngspice button from the left toolbar. |
| 10:27 | Let us keep the default values for the Analysis tab and the Source Details tab. |
| 10:35 | Skip the Ngspice Model tab. |
| 10:39 | Click on Device Modeling tab. |
| 10:42 | Click on the ADD button. |
| 10:45 | Double-click on the Diode folder. |
| 10:49 | Select Germanium underscore Diode dot lib file and click on the Open button. |
| 10:58 | This step was done because we have edited the Germanium diode library file. |
| 11:05 | On the Kicad to Ngspice tab, click on the Convert button. |
| 11:11 | Click on the OK button in the Information dialog box. |
| 11:16 | Let us now generate the plots. |
| 11:19 | On the eSim window, click on the Simulation button from the left toolbar. |
| 11:26 | The Ngspice terminal and plots opens along with the Python plot. |
| 11:32 | Notice a decrease in the forward characteristics. |
| 11:37 | The knee voltage is around 0.5 volts, which is similar to a Silicon diode. |
| 11:45 | The forward current is 1.1 milliampere. |
| 11:50 | Close the Ngspice terminal and plots. |
| 11:54 | In the Python plot window, check the In and Out nodes. |
| 11:59 | Then click on the Plot button. |
| 12:03 | You can see the input and output plot. |
| 12:08 | Now close the Python plot window. |
| 12:12 | Let us summarise.
In this tutorial, we learnt: To create a Germanium Diode from an existing Device Model and |
| 12:22 | To edit a current Device Model. |
| 12:26 | Do you have questions in this Spoken Tutorial? |
| 12:30 | Choose the minute and second where you have the question. |
| 12:35 | Explain your question briefly. |
| 12:38 | Someone from the FOSSEE team will answer them.
Please visit this site. |
| 12:45 | For any general or technical questions on eSim, visit the FOSSEE forum and post your question. |
| 12:54 | The FOSSEE team coordinates the Circuit Simulation project. |
| 13:00 | We give Certificates and Honorarium to the contributors.
For more details, please visit this site. |
| 13:09 | The FOSSEE team coordinates the Lab Migration project.
For more details, please visit this site. |
| 13:18 | Spoken Tutorial Project is funded by NMEICT, MHRD, Govt. of India.
For more details, visit this site. |
| 13:30 | This is Gloria N from IIT Bombay signing off.
Thank you |
