ESim/C2/Creating-a-Device-Model/English-timed

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

Contributors and Content Editors

PoojaMoolya