ESim/C2/Mapping-Components-with-Footprints/English-timed

Time	Narration
00:01	Welcome to the spoken tutorial on “Mapping components with footprints”.
00:06	In this tutorial, we will learn to : Add connectors to a schematic. Map components with footprints using CvPcb. Generate netlist for PCB design.
00:20	This tutorial is recorded using- Ubuntu Linux OS version 16.04 and eSim version 1.1.2
00:32	To practice this tutorial, you should know: The basic concepts of electronic circuits. To create circuit schematic in eSim. To simulate the netlist in eSim.
00:45	If not, watch the prerequisite eSim spoken tutorials on this website.
00:51	I have already opened eSim on my machine.
00:55	Let us open example “7805VoltageRegulator” from the Examples folder of eSim.
01:02	Click on the Open Project button from the left toolbar.
01:07	Then browse to the directory where you have installed eSim.
01:11	I will double-click on Downloads. Double-click on eSim hyphen 1.1.2.
01:19	Double-click on Examples. Click on 7805VoltageRegulator.
01:22	Click on Open button at the bottom right corner.
01:32	To open the schematic, click on Open Schematic button on the left toolbar.
01:38	The eSim Schematic Editor opens. I will zoom into the schematic.
01:44	This circuit uses AC sine wave as input and Lm_7805 subcircuit as a voltage regulator.
01:54	I will switch back to the eSim main window.
01:58	Click on Simulation button from the left toolbar.
02:02	We have given the AC signal as input.
02:06	We can see the rectified 5 volts DC output.
02:10	Let us learn how to map footprints with components.
02:15	I will switch back to eSim Schematic Editor.
02:19	The schematic contains plots, labels and sources, which are essential for simulation.
02:27	These components are not required for PCB designing.
02:31	Let us delete the components that are not required for PCB designing.
02:36	Right-click on sine source and select the Delete Component option.
02:43	Right-click on plot_v1 that is U1 component and select the Delete Component option.
02:51	Similarly, we will delete the remaining plots, labels and components which are not required.
02:58	I have deleted other components and their connections.
03:02	Let us now add a connector for the output of the circuit schematic.
03:07	Click on Place Component button from the right toolbar.
03:12	Click anywhere on the schematic.
03:15	Type Conn in the Filter field.
03:19	Click on Conn underscore 01x02.
03:26	Click on OK button at the bottom right of the Component Selection window.
03:32	Conn underscore 01x02 will appear to be tied to the cursor.
03:38	Let us place the Conn underscore 01x02 on the right side of the schematic.
03:45	Click once to place the connector on the right side of the schematic.
03:50	We also need a connector at the input to connect the external power supply.
03:56	We have already selected Place component tool.
04:00	Click anywhere on the eSim Schematic Editor window.
04:04	Type Screw underscore Terminal in the filter box.
04:09	Click on Screw underscore underscore 01x02 from the list.
04:18	Click OK button at the bottom right corner of Component Selection window.
04:24	Click once to place the connector on the left side of the schematic.
04:29	Let us rotate Screw underscore Terminal underscore 01x02.
04:35	Right-click on Screw underscore Terminal underscore 01x02 component.
04:42	Select Orient Component from the drop-down menu and select Mirror II (two) option.
04:50	Now, let us connect the connectors using wires.
04:54	We have learnt to place wires earlier in this series.
04:59	You can refer to the prerequisite tutorials, if required.
05:04	Let us connect pin 1 of Screw_Terminal underscore 01x02 to the wire connecting D3 and D4.
05:16	I have connected rest of the nodes to their respective connectors.
05:21	All the components are connected.
05:24	Let us annotate the schematic and perform ERC for the circuit schematic.
05:31	Please refer to the prerequisite tutorials to learn how to perform Annotation and ERC.
05:38	Let us now save the schematic.
05:41	Press Ctrl and S keys together to save this schematic.
05:46	We will now learn how to map the components with their footprints.
05:51	Footprint is the layout of a component which is placed on the Printed Circuit Board.
05:57	Click on the Run CvPcb to associate components and footprints button at the top of the eSim Schematic Editor.
06:06	This opens Cvpcb window.
06:09	If you’re using Cvpcb for the first time, you will get a confirmation box.
06:15	Here, click on the OK button.
06:18	If you get another dialog box titled Confirmation, click on No button.
06:25	The Cvpcb window is divided into three panels.
06:30	The left panel shows the Libraries of the footprints.
06:35	The middle panel is divided into 3 columns.
06:39	The first column in the middle panel shows the serial number.
06:44	The second column in the middle panel shows the reference ID of the components used in the schematic.
06:51	The third column in the middle panel shows the values of the corresponding components, if any.
06:58	The right panel gives a list of footprints available in the libraries.
07:03	The top menu of Cvpcb window has 3 options to filter the footprints.
07:09	This will filter the footprints by keywords.
07:13	This will filter the footprints by pin count.
07:17	This will filter the footprints by the library.
07:21	Now we will map the components with their appropriate footprints.
07:26	Click on the option Filter footprints list by library from the top menu.
07:33	If any other filters other than Filter footprints list by library are selected, please uncheck them.
07:41	Please note that we are designing a board for Through Hole components.
07:46	Footprints which are meant for Through hole components, will have THT in their description.
07:53	Footprints which are meant for Surface Mount Device components, will have SMD in their description.
08:00	Click on C1, the first row C1 will be highlighted.
08:05	Click on Capacitors_THT from the leftmost panel for selection of footprints of Through hole capacitors.
08:15	The list of Capacitors underscore THT footprints for selected component C1 will be available.
08:24	We can also view the selected footprint.
08:26	To do so, select any footprint from the right panel.
08:32	Click on View selected footprint from the top panel.
08:37	This will open footprint window which displays the image of the selected footprint.
08:43	Now let us map the associated footprint for component C1.
08:48	Let us locate the footprint with D 5.0 mm and P 2.50 mm.
08:55	Double-click on it to assign this footprint.
08:59	For J1 connector: Click on J1, click on Connectors underscore Terminal underscore Blocks from the leftmost panel.
09:10	Locate TerminalBlock underscore Altech underscore AK300 hyphen 2 underscore P5.00mm in the rightmost panel.
09:24	Double-click on it to assign this footprint to J1.
09:28	For J2 connector: Click on J2, click on Pin_Headers from the leftmost panel.
09:36	Locate Pin underscore Headers colon Pin underscore Header underscore Straight underscore 1x02 underscore Pitch2.54mm . Double-click on it.
09:52	For Lm_7805: Click on Lm_7805
09:56	Click on TO underscore SOT underscore Packages underscore THT from the leftmost panel.
10:11	Locate T0 hyphen 220 hyphen 3 underscore Vertical from the rightmost panel.
10:20	Double-click on it to assign this footprint.
10:24	I have mapped rest of the components with their appropriate footprints.
10:29	Now we will save this footprint association.
10:33	Click on Save footprint association in schematic component footprint fields at the left corner of the top toolbar.
10:41	This is a very important step and should not be skipped.
10:45	It assigns the selected footprints to the components present in the schematic.
10:50	Let us now generate the netlist for circuit schematic required for PCB layout.
10:56	I will go back to the eSim Schematic editor window.
11:00	Click on Generate netlist button at the top of eSim Schematic Editor window.
11:06	Click on Pcbnew tab Check the option Default format.
11:12	Click on Generate button. Then click on Save button at the bottom right corner.
11:20	dot net netlist file contains information about components and footprints assigned.
11:26	This is crucial for Printed Circuit Board designing.
11:30	With this, we come to the end of this tutorial. Let us summarize.
11:36	In this tutorial, we learnt to : Add connectors to a schematic. Map components with footprints using CvPcb and Generate netlist for PCB design.
11:48	Please post your timed queries in this forum.
11:52	Please post your general queries on eSim in this forum.
11:57	FOSSEE team coordinates the Lab Migration project.
12:02	FOSSEE team coordinates the Circuit Simulation project.
12:07	Spoken Tutorial Project is funded by NMEICT, MHRD, Govt. of India.
12:13	This is Saurabh from IIT Bombay signing off.Thank you.

Contributors and Content Editors

Pratik kamble