KiCad/C2/Electric-rule-checking-and-Netlist-generation/English-timed

Time	Narration
00:01	Dear Friends,
00:03	Welcome to the spoken tutorial on Electric rule check and netlist generation in KiCad.
00:09	In this tutorial, we will learn-
00:12	* To assign values to components
00:14	* To perform electric rule check and
00:17	* To generate netlist for schematic created.
00:21	We are using Ubuntu 12.04 as the operating system
00:25	with KiCad version 2011 hyphen 05 hyphen 25 for this tutorial.
00:33	Basic knowledge of electronic circuit is pre-requisite for this tutorial.
00:38	User should also know how to design circuit schematic in KiCad.
00:42	For relevant tutorials, please visit the link: spoken hyphen tutorial.org
00:49	To start KiCad,
00:50	Go to the top left corner of ubuntu desktop screen.
00:56	Click on the first icon i.e. Dashhome.
01:01	In the search tab, write "KiCad" and press Enter.
01:10	This will open the KiCad main window
01:13	Click on EEschema tab.
01:17	An Info dialog-box appears saying it cannot find schematic.
01:21	Click on OK.
01:23	We will use the file 'project1.sch' created earlier.
01:29	Go to File menu and click on Open.
01:33	Select 'project1.sch' from desired directory.
01:44	We will now assign values to components.
01:49	Let us assign value to 'R2' component.
01:54	Keep cursor over 'R', corresponding to 'R2' resistor.
02:01	Right-click and choose Field Value.
02:05	This will open Edit Value Field window.
02:11	Type "1M" and click on OK.
02:17	As you can see '1M' (i.e. 1 mega ohm) value is assigned to the resistor 'R2'.
02:24	I have already assigned values to other components in the similar way.
02:29	Next step is to perform electric rule check on this circuit
02:36	Go to top panel of 'EEschema' window.
02:39	Click on Perform electric rule check button.
02:44	This will open the EEschema Erc window.
02:48	Click on Test Erc button.
02:52	We can see that there are two errors.
02:56	Both errors say that the terminals have no power sources.
03:00	Click on the Close button.
03:03	In the schematic, the error nodes are pointed by arrows.
03:12	Let us connect a power Flag here. So, then KiCad will know that we are going to connect a power supply here.
03:22	For this,
03:24	On the right panel, click on Place a power port button.
03:29	Now, click on the 'EEschema' window to open the component selection window.
03:34	Click on List All button and you can see list of power notations.
03:40	Choose PWR_(underscore)FLAG and click on OK.
03:49	We will place the Power flag near 'VCC' terminal.
03:55	Click on the EEschema to place it.
03:59	We need two such power flags since there are two errors of such type.
04:05	Keep the cursor on the power flag and then press 'c' to copy it.
04:10	Place this power flag near the ground terminal.
04:15	Now, we will connect the power flag with wires. Go to right panel and click Place a wire button.
04:24	Now, connect the power flag to VCC terminal.
04:35	Similarly, connect the power flag to the ground terminal.
04:44	We will now run the Schematic ERC check once again to confirm.
04:49	For this, click on the Perform electric rules check on the top panel of 'EEschema' window.
04:55	This will open the 'EEschema Erc' window.
04:58	Click on Test Erc button.
05:01	We can see that there are no errors.
05:04	Click on Close.
05:07	Now, let us see how to generate netlist.
05:10	Netlist gives information about list of components and nodes that connects them together.
05:16	We will see the use of netlist as we proceed further in this tutorial.
05:20	For generating netlist, go to the top panel. Click on netlist generation button.
05:27	This will open up the Netlist window.
05:31	This window contains tabs which allow you to generate netlist in different formats.
05:38	For KiCad we will use Pcbnew tab.
05:42	Keep Default format option checked and click on Netlist button.
05:48	Note that it saves the netlist file with name 'project1.net'.
05:54	Please note that when the netlist is generated, the file is saved with '.net' extension.
06:00	Click on the Save button.
06:02	Let me resize the window.
06:04	Click on the Save button.
06:06	Netlist file contains information about components in the circuit required for printed circuit board design.
06:14	We will see the use of this netlist file in another tutorial.
06:20	Go to File menu and choose Save Whole Schematic Project to save this schematic.
06:27	Go to File menu and choose Quit to close 'EEschema' window.
06:32	In KiCad main window,
06:34	Go to File menu and choose Quit. This will close the KiCad main window.
06:40	In this tutorial, we learnt-
06:44	* To assign values to components
06:46	* To check and correct for errors in circuit schematic
06:50	* To generate netlist for circuit.
06:53	Watch the video available at the following link.
06:56	It summarizes the Spoken Tutorial project.
06:58	If you do not have good bandwidth, you can download and watch it.
07:02	The Spoken Tutorial project team:
07:04	* Conducts workshops using spoken tutorials.
07:07	* Gives certificates for those who pass an online test.
07:10	For more details, please write to: contact at spoken hyphen tutorial dot org.
07:16	Spoken Tutorial project is a part of the Talk to a Teacher project.
07:19	It is supported by the National Mission on Education through ICT, MHRD, Government of India.
07:25	More information on this mission is available at:
07:28	spoken hyphen tutorial dot org slash NMEICT hyphen Intro.
07:34	This script has been contributed by Abhishek Pawar.
07:39	This is Rupak Rokade from IIT Bombay, signing off. Thanks for joining.

Contributors and Content Editors

PoojaMoolya, Pratik kamble, Sandhya.np14