ESim/C2/Setting-Parameters-for-PCB-designing/English

Visual cue	Narration
Show Slide: Opening Slide	Welcome to the spoken tutorial on “Setting Parameters for Designing PCB”.
Show Slide: Learning Objectives	In this tutorial, we will learn to -* Read a PCB netlist. Draw outline and setup design parameters for a board. Move and orient footprints.
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 design and simulate a circuit in eSim. To map components with footprints in CvPcb. To create netlist for PCB Design in eSim. If not, watch the prerequisite eSim tutorials on this website.
System Computer: eSim startup window	I have opened eSim on my machine.
Narration only	Let us open 7805VoltageRegulator example.
Slide with no narration This file is available in the Code Files link. Please download and save this file to your Desktop. We will use this file for practise of this tutorial.
eSim main window: Click on Open Project >> Select Desktop location >> Click on 7805VoltageRegulator >> Click Open	Click on Open Project button from the left toolbar. Click on Desktop. Click on 7805VoltageRegulator. Click on Open button at the bottom right corner.
eSim main window : Click on Open Schematic	Click on Open Schematic button from left toolbar, to open the schematic.
eSim Schematic Editor Window: Click on Cvpcb shortcut at the top toolbar.	The schematic will open. Click on Cvpcb shortcut at the top toolbar.
Cvpcb Window: Hover cursor over the components and their mapped footprints.	I have mapped the components with appropriate footprints and generated netlist for it. I will switch back to the eSim schematic editor.
eSim Schematic Window: Click on Tools >> Click Layout Printed Circuit Board Click Yes	Click on Tools at the top toolbar. And Select the Layout Printed Circuit Board. If you get a Confirmation box, click on Yes.
Pcbnew Window: Show empty layout screen	An empty layout screen is seen in the Pcbnew window.
Pcbnew Window: Click on Read netlist	On the top toolbar, click on Read netlist. Netlist window will appear.
Netlist Window : Click on Browse>> navigate to Desktop. Double click on 7805VoltageRegulator >> Click on 7805VoltageRegulator.net >> Click on Open	Click on Browse button, and navigate to Desktop Location. Double click on 7805VoltageRegulator. Click on 7805VoltageRegulator.net. Click on Open button at the bottom right corner of this window.
	The netlist will be loaded.
Netlist Window: Click on Read Current Netlist >> Hover cursor over Messages window >> Click on Close	Click on Read Current Netlist button at the top right corner of Netlist window. If there is an error it will appear in red color in the Messages window. In my case, there are no errors. Click on the Close button at the top right corner of the Netlist window.
Pcbnew Window: Hover mouse over footprints in the Pcbnew window	The footprints mapped with the components appear on layout screen in a bundled manner.
	Let us first draw an outline for the board we are creating.
Pcbnew window: Right-click on the layout screen >> Click on Select working layer Click on Edge.Cuts	To place an outline for the board on Edge.Cuts layer, right-click on the layout screen. Click on Select working layer. Click on Edge.Cuts.
Pcbnew window : Hover cursor over the rightmost panel. >> Hover cursor over Layer. >> Hover cursor over F.Cu, B.Cu Hover cursor over F.Silks, Margin and Edge.Cuts layers >> Click on Edge.Cuts >> Hover mouse over the blue arrow	Alternately, working layer can be selected from the right side of the panel. Under the Layer option, working layers of a board are listed. Front Copper and Bottom Copper layers will be used for placing tracks. Front Silk, Edge.Cuts and Margin will be used for placing text and dimension. Click on the right side of Edge.Cuts, a blue arrow will appear next to the Edge.Cuts.
Pcbnew window: Click on Place >> Click on Line or Polygon from the dropdown menu Click on the layout screen>> Move the cursor horizontally >> Click on the editor >> Hover cursor over the yellow line	Click on Place at the top toolbar of Pcbnew window. Click on Line or Polygon from the menu. A pencil tied to your cursor will appear on the layout screen. We will use this to draw the outline. Click on the layout screen and move the pencil horizontally to a certain extent. Click on the location where we want to finish the line. A yellow line will appear on the layout screen. We will draw a rectangular shaped outline using the method demonstrated.
Pcbnew window : Show completed rectangular border	We have created a rectangular shape as the outline for the board. Press esc key to exit Line or Polygon tool.
	Now let us separate and place the footprints now.
Pcbnew window : Press F1 or use the scroll button to zoom in. >> Right Click on Screw_Terminal_01x02 text >>Select Footprint J1 on F.Cu >> Select the Move option >> hover cursor in circular fashion Move the cursor towards left >> Click once on Pcbnew Window	I will now zoom in to see the footprints on the layout clearly, using the F1 key. Right-click on Screw underscore Terminal underscore 01x02, click on Footprint J1 on F.Cu. And Select the Move option. Move the cursor tied to the footprint horizontally towards left. Click once on the layout screen to place the footprint.
Pcbnew window: Right Click on Screw_Terminal_01x02 Select Footprint J1 on F.Cu >> Select the Rotate + option	To properly orient this footprint, right-click on Screw_Terminal_01x02. Select Footprint J1 on F.Cu. Let us select the Rotate + option.
	Similarly we will move and orient all other footprints, according to our design. All the components should be inside the rectangular outline drawn.
Pcbnew window: Press Shift and ? key together >> Hover mouse over Hotkeys List window	Press Shift and ? keys together. This will open all the keyboard shortcuts available under Hotkeys List window.
	We can use Hotkeys or the demonstrated methods for placing and orienting the footprints.
Click Close	Click on Close button at bottom right corner of the Hotkeys List window.
	You may or may not see white wires, representing interconnected footprints.
Pcbnew window : Click on Show or Hide board ratnest	If you do not see them, click on Show or Hide board ratsnest button at the panel of Pcbnew window. White wires are called as airwires.
Pcbnew window : Show moved and oriented footprints	I have already moved and oriented the footprints to get minimum intersection between airwires.
	Let us set the parameters to place tracks on the layout.
Pcbnew window: Click on Design Rules >> Click on Design Rules from menu	Click on Design Rules option given at the top side of the toolbar. Click on Design Rules from the menu.
Design Rules Editor window : Click on window below Track Width Press backspace key thrice Enter the number 1.2	We will change the default track width from 0.25 mm to 1.2 mm. Click on the window below Track Width. Let us clear the present value using backspace key. Type the number 1.2.
	This will make all tracks placed in future, of 1.2 millimeter width. You can select the track width according to your requirements.
Design Rules Editor Window : Click on Global Design Rules tab >> Click on the tab in front of Min track width. >> Press backspace key thrice >> Enter the number 1.2	Click on Global Design Rules at the top of the Design Rules Editor window. Click on the tab in front of Min track width. Let us clear the present value using Backspace key. Then type the number 1.2 in this space.
	This ensures that any track placed on any layer, is of minimum 1.2 mm width.
Design Rules Editor window: Click Ok	Click on the Ok button at the bottom right corner.
	Now let us check the drill hole size of X1, that is Lm_7805.
Pcbnew window: Place cursor on Node 1 of X1, Press E key.	Place cursor on Node 1 of X1 and press E key.
	Pad Properties window will appear.
Pad Properties window: Hover cursor over Drill block from the top right corner of Pad Properties Window Hover cursor over Size X:	We can see the drill hole properties such as shape, size of this particular pad. We can see the default drill hole size for this particular pad is 1 millimeter.
	The default drill hole size and shape for different footprints may vary. We can change it according to our need.
Click Ok	Click on the Ok button at the bottom right corner of the Pad Properties Window.
Pcbnew window: Press Ctrl and S keys together	Let us press Ctrl and S keys together to save the work.
	With this, we come to the end of this tutorial. Let us summarize.
Show Slide: Summary	In this tutorial, we learnt to :* Read a PCB netlist. Draw outline and setup design parameters for a board. Move and orient footprints.
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