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

Visual cue	Narration
Show Slide: Opening Slide	Welcome to the spoken tutorial on “Laying Tracks on Printed Circuit Board”.
Show Slide: Learning Objectives	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.
Show Slide: Systems Requirements	This tutorial is recorded using - Ubuntu Linux OS version 16.04 eSim version 1.1.2
Show Slide: Prerequisites	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. If not, see the prerequisite eSim tutorials on this website.
eSim main window:	I have already opened eSim on my machine.
eSim main window.	Let us open example 7805VoltageRegulator. I have saved this on my Desktop.
	I have already read the netlist, created an outline and set the design parameters.
Click on Open Project Navigate to Desktop location Click on7805VoltageRegulator Click Open	Click on Open Project from the left toolbar. And navigate to the location where you have saved this. I will browse to Desktop. Click on 7805VoltageRegulator. Click on the Open button at the bottom right corner of this window.
eSim main window : Click on Open Schematic	Click on Open Schematic button on the left toolbar, to open the schematic.
eSim Schematic window: Press F1 Click on Tools >> select Layout Printed Circuit Board	Using F1 I will zoom into the schematic. Click on Tools button at the top toolbar, and select Layout Printed Circuit Board. Let me resize this window.
Pcbnew window: Hover cursor over airwires	I have moved and oriented the footprints, such that there is minimum intersection between airwires. Let us see how to convert the airwires into tracks.
Pcbnew window. Hover mouse over B.Cu text >>Click on B.Cu text Hover mouse over blue arrow next to B.Cu	Under the Layer tab on the right side of the Pcbnew window, click on B.Cu once. Layer selected will be indicated by a blue arrow on the left side of B.Cu.
Pcbnew window. Click on Place >> select Track	Click on Place button in the top toolbar, and select Track from the menu.
Pcbnew window. Use scroll keys to zoom in	Let us place tracks for connecting the capacitor C2 to the output terminal J2. I will zoom into the layout screen.
Pcbnew window. Click on node 1 of C2 >> Drag the cursor till node 1 of J2 >> Double click on node 1 of J2	Click on node 1 of C2. Let us drag this track from node 1 of C2 to node 1 of J2, by dragging the cursor till node 1 of J2. Double-click on node 1 of J2 to complete the track.
Pcbnew window. Press Esc key Hover cursor over GND label	Similarly connect all the other nodes except the Ground nodes. Press Esc button to exit the Place Track tool. Ground nodes are denoted by GND designation.
	Let us place a ground plane to connect all the ground nodes.
Pcbnew window. Click on Add filled zones.	Click on Add filled zones button located at the right side of the Pcbnew window.
Pcbnew window: Click once, slightly above the top-left corner of the board outline.	Click once, slightly above the top-left corner of the board outline.
Copper Zone Properties window: Click on B.Cu under Layer column Click on GND under Net column	Let us place the ground plane on Bottom Copper layer. To do so, click on B.Cu under Layer column. Click on GND under Net column.
Click on OK	Click on OK button at the bottom right corner of the Copper Zone Properties window.
Pcbnew window. Drag the cursor towards right, horizontally Click once slightly above top-right vertex of the outline.	Drag the cursor with the pencil icon horizontally towards the right. Click once, slightly above the top-right vertex of the outline.
Pcbnew window. Move the cursor vertically towards the bottom-left vertex of the board >>Click once on the editor after crossing the bottom-left vertex.	Let us move this cursor vertically, towards the bottom-right vertex of the board. Click once slightly below bottom-right vertex.
Pcbnew window. Hover cursor over board outline >> Hover cursor over ground plane outline.	Similarly, we will draw a rectangular ground plane outline around board outline. Please do not confuse board outline with ground plane outline.
Pcbnew window. Hover cursor over ground plane outline >>Hover cursor over ground plane outline and board outline.	I have completed the ground plane outline. Note that the ground plane outline should lie outside the board outline.
Pcbnew window : Right-click inside the board outline. Click on Fill or Refill All Zones Hover cursor over ground plane	Right-click inside the board outline. Click on Fill or Refill All Zones button from the menu. We have added a ground plane to the board.
Press esc key	Press Esc key to exit the Add filled zones tool.
	Let us now perform Design Rule Check i.e DRC, for the layout we created. It checks whether the design created is compliant with the Design Rules set earlier.
Pcbnew window: Click on Perform design rules check	Click on Perform Design Rules check present at the top of the Pcbnew toolbar.
DRC Control window: Click on Start DRC Hover mouse over Error Messages:	Click on Start DRC. This checks if any design element violates the design parameters set earlier. If there are any design errors, they will be displayed in Error Messages window. In my case, there are no errors.
DRC Control window: Click OK	Click OK button at the bottom right corner to exit the DRC Control window.
	Now let us see how to add text on our board.
Pcbnew window. Click on F.Silks from the right toolbar Click on Place from the top toolbar and select Text from the dropdown menu Click once on Pcbnew window	Let us click on F.Silks layer to place text on the Front Silk Layer. Click on Place button from top toolbar and select Text option from the dropdown menu. Click once on the Pcbnew window.
Text Properties window : Type 7805VoltageRegulator in the Text window. Click on OK	I will type 7805VoltageRegulator in the Text window. Click on OK button at the bottom right corner of the Text Properties window.
Pcbnew window: Click once at the bottom right corner of layout screen. Press F2 or use scroll keys to zoom out and hover cursor over the text.	The typed text will be tied to the cursor. Drag cursor to bottom right corner of the layout screen and click once. We can see the text is placed in light blue color.
	Please make sure to click inside the board outline. Now let us see how to add dimensions to our board design.
Pcbnew window. Click on Margin layer from the right toolbar Click on Place from the top toolbar and select Dimension from the menu	Click on Margin layer. Click on Place at top toolbar and select Dimension option.
Pcbnew window. Click once the top-right vertex of the board layout	Click once on either vertex of the board layout. I have chosen the top-right vertex.
Drag the cursor towards the bottom right vertex in a straight line. Press Enter key twice	Let us drag the cursor towards the bottom right vertex in a straight line. Press Enter key twice.
	The dimension will be placed for the vertical edge of the board.
Pcbnew window. Hover cursor over horizontal dimension	We will perform similar steps for placing horizontal dimensions of the layout.
Pcbnew window. Press Ctrl and S key together	Let us press Ctrl and S keys together to save the work. Let us now create gerber file s for this board.
Pcbnew window. Click on Plot(HPGL, PostScript or Gerber format) icon	Click on Plot button at the top of the Pcbnew toolbar.
Plot window. Click on the tab below : Plot format. >> Select Gerber.	Click on the tab below Plot format. Select Gerber out of the 6 options.
>> Hover mouse over Layers tab >> Click on boxes to the left of F.Cu, B.Cu,F.Silks, Edge.Cuts and Margin layers from the provided layer options.	Let us select the layers for which we want the gerber files. I will select F.Cu, B.Cu, F.Silks, Edge.Cuts and Margin layers by clicking on the boxes to the left.
Plot window: Click on Browse button	Click on Browse button at the top right of Plot window.
Select Output Directory window. Browse to desired directory >>Click on Desktop >>double click on 7805VoltageRegulator Click on Open.	Let us navigate to the desired directory where we want to save the gerber files. Click on Desktop, double click on 7805VoltageRegulator. Click on Open button at bottom right corner of Select Output Directory window.
Click on No	Click on No button of Plot Output Directory window.
Plot window. Click on Plot button located at the bottom of Plot window.	Click on Plot button at the bottom of the Plot window.
Messages window : Hover cursor over the messages appeared in the Messages window	Acknowledgement messages will appear in the Messages window.
	Let us generate the drill file in gerber format for our designed board.
Plot window. Click on Generate Drill File	Click on Generate Drill File at the bottom of the Plot window.
Drill Files Generation window: Click on Browse Browse to the desired directory location Click Open	Click on Browse button at top right corner of Drill Files Generation window. I will navigate to Desktop/7805VoltageRegulator Click on Open button at the bottom right corner of Drill Files Generation window.
Plot Output Directory window: Click on No	If Plot Output Directory window appears, click on No button in the middle of Plot Output Directory window.
Plot window: Click on Gerber option at middle of Drill Files Generation window	Click on Gerber option placed in the middle of Drill Files Generation window, if not selected.
	We will leave the rest of the settings as they are.
Drill Files Generation window: Click on Drill File	Click on Drill File option present at the right side of Drill Files Generation window.
Drill Files Generation window : Hover mouse over Messages window	An acknowledgement message will appear in the Messages window.
Drill Files Generation window: Click on Close	Click on Close button at the bottom right corner of Drill Files Generation window.
Plot window : Click on Close	Click on Close button at the bottom right corner of Plot window.
Pcbnew window : Press Ctrl and S key at the same time.	Let us save our work by pressing Ctrl and S keys simultaneously.
System Computer: Press Ctrl, Alt and T keys together	Now we will view the gerbers created. Open the terminal by pressing Ctrl, Alt and T keys together.
Terminal : Type gerbview >> Press Enter	Type gerbview and press Enter key.
Gerbview window : Click on File>> select Load Gerber File	Click on File from the top left corner, and select Load Gerber File option.
Open Gerber File window : Browse to the directory where you saved your gerber files earlier.	Let us browse to directory where we have saved the gerber files. I will click on Desktop, and then double-click on 7805VoltageRegulator.
Press Ctrl and A keys at the same time. Click on Open	Press Ctrl and A keys at the same time to select all the gerber files. Click on Open button at the bottom right corner of the Open Gerber file window.
Gerbview window. Hover mouse over the PCB layout in Gerber Format	We can see the PCB Layout we created in Gerber format.
Show image Image1.jpg	This is the FR4 grade copper cladded sheet on which we will transfer our design to.
Show image Image2.jpg	After etching and drilling appropriate holes, this is how the board will look. Components can now be mounted and soldered on this board.
Show image Image3.jpg	This is how the board looks after components are soldered on it.
	With this, we come to the end of this tutorial. Let us summarize.
Show Slide: Summary	In this tutorial, we learnt to : Place tracks on printed circuit board. Add dimension and text on Silkscreens. Generate Gerber files and view them.
Show Slide: Forum	Please post your timed queries in this forum.
Show Slide: FOSSEE Forum	Please post your general queries on eSim in this forum.
Show Slide: Textbook Companion	FOSSEE team coordinates the TBC project.
Show Slide: Acknowledgment http://spoken-tutorial.org	Spoken Tutorial Project is funded by NMEICT, MHRD, Govt. of India. For more details, visit this website.
Thank you Slide	This is Saurabh from IIT Bombay, signing off. Thank you.

Contributors and Content Editors

Nancyvarkey, PoojaMoolya, Saurabhbansode