ESim/C2/Laying-Tracks-on-PCB/English-timed

Time	Narration
00:01	Welcome to the spoken tutorial on “Laying Tracks on Printed Circuit Board”.
00:07	In this tutorial, we will learn to - Place tracks on printed circuit board. Add dimension and text on Silkscreens. Generate Gerber files and view them.
00:20	This tutorial is recorded using - Ubuntu Linux OS version 16.04 eSim version 1.1.2
00:31	To practice this tutorial, you should know to: Read a PCB netlist. Draw outline and setup design parameters for a board. Move and orient footprints.
00:43	If not, see the prerequisite eSim tutorials on this website.
00:48	I have already opened eSim on my machine.
00:50	Let us open example 7805VoltageRegulator. I have saved this on my Desktop.
00:59	I have already read the netlist, created an outline and set the design parameters.
01:05	Click on Open Project from the left toolbar.
01:09	And navigate to the location where you have saved this.
01:13	I will browse to Desktop. Click on 7805VoltageRegulator.
01:19	Click on the Open button at the bottom right corner of this window.
01:24	Click on Open Schematic button on the left toolbar, to open the schematic.
01:30	Using F1 I will zoom into the schematic.
01:34	Click on Tools button at the top toolbar, and select Layout Printed Circuit Board. Let me resize this window.
01:45	I have moved and oriented the footprints, such that there is minimum intersection between airwires.
01:52	Let us see how to convert the airwires into tracks.
01:56	Under the Layer tab on the right side of the Pcbnew window, click on B.Cu once.
02:03	Layer selected will be indicated by a blue arrow on the left side of B.Cu.
02:09	Click on Place button in the top toolbar, and select Track from the menu.
02:15	Let us place tracks for connecting the capacitor C2 to the output terminal J2. I will zoom into the layout screen.
02:24	Click on node 1 of C2.
02:28	Let us drag this track from node 1 of C2 to node 1 of J2, by dragging the cursor till node 1 of J2.
02:36	Double-click on node 1 of J2 to complete the track.
02:40	Similarly connect all the other nodes except the Ground nodes.
02:45	Press Esc key to exit the Place Track tool.
02:49	Ground nodes are denoted by GND designation.
02:54	Let us place a ground plane to connect all the ground nodes.
02:58	Click on Add filled zones button located at the right side of the Pcbnew window.
03:04	Click once, slightly above the top-left corner of the board outline.
03:09	Let us place the ground plane on Bottom Copper layer.
03:13	To do so, click on B.Cu under Layer column.
03:18	Click on GND under Net column.
03:22	Click on OK button at the bottom right corner of the Copper Zone Properties window.
03:28	Drag the cursor with the pencil icon horizontally towards the right.
03:34	Click once, slightly above the top-right vertex of the outline.
03:39	Let us move this cursor vertically, towards the bottom-right vertex of the board.
03:45	Click once slightly below bottom-right vertex.
03:49	Similarly, we will draw a rectangular ground plane outline around board outline.
03:56	Please do not confuse board outline with ground plane outline.
04:01	I have completed the ground plane outline.
04:04	Note that the ground plane outline should lie outside the board outline.
04:09	Right-click inside the board outline.
04:12	Click on Fill or Refill all zones button from the menu.
04:17	We have added a ground plane to the board.
04:20	Press Esc key to exit the Add filled zones tool.
04:25	Let us now perform Design Rule Check i.e DRC, for the layout we created.
04:32	It checks whether the design created is compliant with the Design Rules set earlier.
04:38	Click on Perform Design Rules check present at the top of the Pcbnew toolbar.
04:44	Click on Start DRC.
04:47	This checks if any design element violates the design parameters set earlier.
04:52	If there are any design errors, they will be displayed in Error Messages window.
04:58	In my case, there are no errors.
05:01	Click OK button at the bottom right corner to exit the DRC Control window.
05:07	Now let us see how to add text on our board.
05:11	Let us click on F.Silks layer to place text on the Front Silk Layer.
05:19	Click on Place button from top toolbar and select Text option from the dropdown menu.
05:27	Click once on the Pcbnew window.
05:31	I will type 7805VoltageRegulator in the Text window.
05:37	Click on OK button at the bottom right corner of the Text Properties window.
05:43	The typed text will be tied to the cursor.
05:47	Drag cursor to bottom right corner of the layout screen and click once.
05:53	We can see the text is placed in light blue color.
05:58	Please make sure to click inside the board outline.
06:02	Now let us see how to add dimensions to our board design.
06:07	Click on Margin layer.
06:10	Click on Place at top toolbar and select Dimension option.
06:16	Click once on either vertex of the board layout. I have chosen the top-right vertex.
06:23	Let us drag the cursor towards the bottom right vertex in a straight line.
06:30	Press Enter key twice. The dimension will be placed for the vertical edge of the board.
06:37	We will perform similar steps for placing horizontal dimensions of the layout.
06:43	Let us press Ctrl and S keys together to save the work.
06:49	Let us now create gerber files for this board.
06:53	Click on Plot button at the top of the Pcbnew toolbar.
06:58	Click on the tab below Plot format. Select Gerber out of the 6 options.
07:05	Let us select the layers for which we want the gerber files.
07:10	I will select F.Cu, B.Cu, F.Silks and Edge.Cuts and Margin layers by clicking on the boxes to the left.
07:24	Click on Browse button at the top right of Plot window.
07:29	Let us navigate to the desired directory where we want to save the gerber files.
07:35	Click on Desktop, double-click on 7805VoltageRegulator.
07:43	Click on Open button at bottom right corner of Select Output Directory window.
07:50	Click on No button of Plot Output Directory window.
07:57	Click on Plot button located at the bottom of Plot window.
08:02	Acknowledgement messages will appear in the Messages window.
08:06	Let us generate the drill file in gerber format for our designed board.
08:11	Click on Generate Drill File at the bottom of the Plot window.
08:16	Click on Browse button at top right corner of Drill Files Generation window.
08:23	I will navigate to Desktop/7805VoltageRegulator.
08:29	Click on Open button at the bottom right corner of Drill Files Generation window.
08:35	If Plot Output Directory window appears, Click on No button in the middle of Plot Output Directory window.
08:42	Click on Gerber option placed in the middle of Drill Files Generation window if not selected.
08:52	Click on Drill File option present at the right side of Drill Files Generation window.
08:58	An acknowledgement message will appear in the Messages window.
09:02	Click on Close button in the middle of Drill Files Generation window.
09:08	Click on Close button at the bottom right corner of Plot window.
09:13	Let us save our work by pressing Ctrl and S keys simultaneously.
09:19	Now we will view the gerbers created.
09:22	Open the terminal by pressing Ctrl, Alt and T keys together.
09:31	Type gerbview and press Enter .
09:35	Click on File from the top left corner, and select Load Gerber File option.
09:43	Let us browse to directory where we have saved the gerber files.
09:48	I will click on Desktop, and then double-click on 7805VoltageRegulator.
09:56	Press Ctrl and A keys at the same time to select all the gerber files.
10:02	Click on Open button at the bottom right corner of the Open Gerber file window.
10:08	We can see the PCB Layout we created in Gerber format.
10:13	This is the FR4 grade copper cladded sheet on which we will transfer our design to.
10:19	After etching and drilling appropriate holes, this is how the board will look.
10:24	Components can now be mounted and soldered on this board.
10:28	This is how the board looks after components are soldered on it.
10:32	With this, we come to the end of this tutorial. Let us summarize.
10:38	In this tutorial, we learnt to : Place tracks on printed circuit board. Add dimension and text on Silkscreens. Generate Gerber files and view them.
10:51	Please post your timed queries in this forum.
10:54	Please post your general queries on eSim in this forum.
11:00	FOSSEE team coordinates the Lab Migration project.
11:06	FOSSEE team coordinates the Circuit Simulation project.
11:10	Spoken Tutorial Project is funded by NMEICT, MHRD, Govt. of India. For more details, visit this website.
11:17	This is Saurabh from IIT Bombay, signing off. Thank you.

Contributors and Content Editors

Pratik kamble