ESim/C2/Mapping-Components-with-Footprints/English-timed
From Script | Spoken-Tutorial
| 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. |
