Oscad/C2/Designing-Printed-Circuit-Board/English

Title of the Script: Designing Printed Circuit Board using Oscad

Author: Rakhi

Keywords: video tutorial, Oscad, schematic, EDA, PCB, layout, footprints

Visual cue	Narration
Title Slide	Welcome to the Spoken Tutorial on “Designing Printed circuit Board using Oscad”
Show Slide: Learning Objectives: - Create netlist for PCB from schematic - Map footprints to components - Generate PCB layout	In this tutorial you will learn to Create netlist for Printed circuit Board, i.e., PCB, from a schematic Map footprints to components and Generate PCB layout
Show slide: Sequence of Steps adopted Create a new Project. Import and modify RC schematic created in the tutorial. Schematic Creation and Simulation using Oscad. Create PCB Layout for RC circuit.	In this tutorial, we will create the PCB Layout of an RC circuit. The following sequence will be adopted We will first create a new project. We will import and modify the RC circuit schematic file created in the the tutorial Schematic Creation and Simulation using Oscad. Finally, we will create the PCB layout for the RC circuit.
Show Slide: Systems Requirements	Here we will use Ubuntu Linux 12.04 and Oscad version 1.0
Pre-requisites: Knowledge of schematic creation using Oscad Watch the relevant tutorial Schematic Creation and Simulation using Oscad available at http://spoken-tutorial.org RC circuit project files created in the above tutorial.	To practice this tutorial, you should know how to create a circuit schematic using Oscad. If not, please visit our website and watch the relevant tutorial. You should also have the RC circuit project files created in that tutorial.
Open the terminal window Type oscad Press Enter	Launch Oscad by doing the following: Open the terminal window Type oscad and press Enter
Show Oscad window Click on Project >> New	Oscad project window opens up. Click on the Project tab and choose New.
Browse to the desired folder. Click on OK. >> Type RC_PCB in the Enter Project name field >> click Ok	Browse to the desired folder. Click on OK. In the Enter Project name field, type RC underscore PCB. Please note that the file names are case sensitive. Click on Ok.
Oscad tool bar >> click on schematic editor Click on OK on the Info dialog box Minimize Oscad project window	Click on the Schematic Editor tool from the Oscad toolbar. In the Info dialog box that appears, click on OK. Let me minimize the Oscad window.
Click on File >> open	Let us import the RC circuit schematic by doing the following: go to the File menu and click on Open.
Browse to the RC project folder.	Browse to the RC project folder.
Select RC dot sch >> click on Open.	Select RC dot sch and click on Open.
Click on Close.	Click on Close.
Go to File menu >> click on Save Current Sheet as.	Let us now save this schematic in the new project folder, RC underscore PCB. To do so, go to File menu and click on Save Current Sheet as.
Browse to the folder RC underscore PCB. Rename the file as RC underscore PCB. Click on Save.	Browse to folder RC underscore PCB. Rename the file as RC underscore PCB. Click on Save.
	It is required that the name of the schematic file should match the name of the project. This is why we renamed the schematic file. Now this schematic is linked to the new project, RC underscore PCB.
	Some changes need to be made in the schematic, to make it ready for PCB design. Let me zoom in.
	The plot components and sine source were added for simulation. They are not needed for PCB design.
Click on sine source >> delete it by pressing the delete key. Repeat the same for plot components.	Let us delete them by clicking on them and pressing the delete key.
	Let us add a two pin connector to the schematic. This is added so that an external voltage source can be connected to the PCB.
Place the component CONN_2 on the editor.	To add it, place the component CONN_2 on the editor.
Rotate it twice and move it as shown.	Rotate it twice and move it as shown.
Connect it to the circuit using wires, as shown	Connect it to the circuit using wires, as shown.
Menu bar >> click on annotate schematic button .	Annotate the schematic by clicking on Annotate Schematic button from the menu bar.
Click on annotation >> click on Ok >> click on close	Click on Annotation; click on Ok; click on Close.
Menu Bar >> Click on perform electric rules check >> Click on test erc >> Click on close.	To check for electric rules, click on Perform electric rules check from the menu bar. Click on Test Erc. You can see there are no errors. Click on Close.
Menu bar >>Click on generate netlist PCBnew tab >> click on Netlist button >> Click on Save >> Close schematic editor. >> Click on Yes	Let us generate netlist for PCB. To do so, click on Generate netlist button from the menu bar. Click on the button Netlist, under the Pcbnew tab. Click on Save to save the netlist. It has a dot net extension. Close the schematic editor. Click on Yes to save the schematic.
	Now we will assign footprints to each of the components in the schematic.
Oscad tool bar >> Click on foot print editor	To do so, click on Footprint Editor from the Oscad toolbar. This launches the Footprint Editor window.
Click on ok to close the component library error window	Click on Ok, to close the Component Library Error window.
Show the lists on left and right	The list of components in the netlist is shown on the left. On the right, you will see a list of all available footprints for the chosen component.
	Let us first assign footprint to capacitor C1.
select C1 from the list on the left side. double-click on C1 from the right side list	For this, select C1 from the list on the left side. Now, double-click on C1 from the list on the right.
menu bar >> Choose View selected footprint	To view the footprint assigned to C1, select C1 and choose View selected footprint from the menu bar.
	A new window opens up displaying the footprint.
	Let us now view a 3D image of this footprint.
menu bar >> Click on the option 3D display	To do this, click on the 3D Display button from the menu bar.
Click on the footprint shown >> drag the view up or down	This is a top view in 3D. Click on the footprint and drag the view up or down, as shown.
Close the 3D viewer window >> Close the footprint viewer window	Close the 3D viewer window. Close the footprint viewer window.
select the next component P1.	Now select the next component P1.
Scroll down the list on the right >> choose SIL-2 by double-clicking on it.	Scroll down the list on the right and double-click on SIL hyphen 2 to choose it. SIL hyphen 2 is a suitable footprint for the two pin connector P1.
For R1, double click on R3 from the list on the right	Similarly, choose the footprint R3 for the resistor R1.
Menu bar >>Click on Save net list and foot print files button	Now, go to the menu bar and click on Save netlist and foot print files button.
	We will use this netlist to design the PCB layout.
Close the Footprint editor window.	Close the Footprint editor window.
Click on Layout editor from the Oscad tool bar.	Now, let us create the PCB layout. Click on Layout Editor from the Oscad toolbar. This will open the Layout Editor tool.
Click on Ok Minimize Oscad project window	Click on Ok to close this dialog box. Let me minimize the Oscad project window.
Menu bar >> Click on Read netlist	Now we will import the netlist that has footprint mapping. To do so, go to the menu bar and click on Read netlist.
Click on Browse Netist files.	Click on Browse Netlist Files.
Browse to the project folder >> Select the netlist RC_PCB.net >>Click on open	Browse to the project folder. Select the netlist file RC underscore PCB dot net. Click on Open.
Click on Read current netlist.	Click on Read current netlist.
Click on close >> Click on Yes	Click on Close. Click on Yes to save the configuration.
Show top left corner	Note that the component footprints are placed at the top left corner of the Layout Editor window. To get a proper view, we have to zoom in.
Place the cursor near the top left corner Zoom in to the top left corner by pressing F1 key.	Place the cursor near the top left corner. Zoom in by pressing F1 key.
Zoom out by pressing the F2 key.	Zoom out by pressing the F2 key. You can also use the scroll button of your mouse to zoom in and out.
Maximise window. Menu bar >>Click on mode footprint:manual and automatic move and place modules button	Let us now place the footprint modules to the center of the Layout Editor window. For this, I have to maximise the window. Click on mode footprint:manual and automatic move and place modules button from the menu bar.
Place the cursor near the center of window.	Place the cursor near the center of the window.
Right click >> choose Glob move and place	Right click and choose Glob Move and Place.
Choose move all modules	Choose Move all modules.
Click on yes	Click on Yes.
Minimise window	Now let me restore this window.
Show modules at center. Zoom in	Now you can see that the modules are at the center. Zoom in.
	This is the current placement of components.
Place the cursor on top of P1 >> press R	Rotate the connector P1. To do so, place the cursor on top of P1 and press the key R.
Place the cursor on P1>> press M Move C1 as shown	To move it, place the cursor on P1 and press M. Similarly, move the footprint C1 as shown.
Top menu bar >>Click on Design rules>> Click on design rules.	Click on Design rules from the menu bar. Click on first option, Design Rules.
Double-click on the track width field	Double-click on the Track Width field, as shown.
Type 0.8 >> press Enter.	Type zero point eight (0.8) and press Enter. Similarly, other design rules can be edited, if required.
Click on OK	Click on OK. Note that the OK button is not fully visible. This is because I am not recording the entire screen and this window cannot be resized.
Show Layer window. Layer pane >> Click on Back	Now, let us start drawing the tracks. The Layer pane on the right, shows a list of layers. Select the layer Back, by clicking on it.
toolbar on the right >> click on Add tracks and vias button Click on one terminal of R1. Move the cursor down. double-click on the left terminal of C1.	To draw tracks, click on Add tracks and vias button from the toolbar on the right. Click on one terminal of R1. Move the cursor down and double-click on the left terminal of C1.
	A track is formed.
Lay all tracks.	Similarly, draw the remaining tracks as shown.
Layer pane >> Click on PCB_Edges	To draw PCB edges, click on PCB underscore edges from the Layer pane on the right side.
right tool bar >> Click on the 'Add graphic line or polygon' tool	Click on 'Add graphic line or polygon' button from the right toolbar.
Click on top left corner of the layout as shown >> Move cursor horizontally to the right	Click on top left corner of the layout as shown. Draw the PCB edge by moving cursor horizontally to the right.
Click once to change orientation. Draw the edges. Double-click to finish the edges.	Click once to change the orientation. Draw the edges as shown. Double-click to finish the edges.
Menu bar >> Click on Perform design rules check	Click on Perform design rules check from the menu bar, to check for design rules.
Click on Start DRC >> Click on ok.	Click on Start DRC. There are no errors. Click on Ok.
Menu bar >> Click on save board	Click on Save board from the menu bar, to save the layout.
top menu bar >> click on File >> Click on plot.	To generate Gerber files, click on File from the top menu bar. Click on plot.
Choose Gerber as the plot format >> click on plot. Click on Close	Choose Gerber as the plot format and click on Plot. Gerber files are created in the project folder. Click on Close.
Slide: Summary	Let us summarise. In this tutorial, we learnt to create netlist for PCB layout, map footprints to components, lay tracks and create the PCB layout.
Slide: Assignment: Watch the relevant KiCad tutorials available at http://spoken-tutorial.org Reproduce the layout of astable multivibrator using Oscad Oscad uses Kicad for PCB layout creation Footprint editor in Oscad = CvPCB in KiCad Layout editor in Oscad = PCBnew in KiCad	Here is an assignment for you. Watch the KiCad tutorials on PCB design available on our website. Reproduce the layout of astable multivibrator created there, using Oscad. Oscad uses KiCad for PCB layout creation. Footprint editor in Oscad is the same as CvPCB in KiCad. Similarly, Layout editor in Oscad is PCBnew in KiCad. So the procedure to create PCB layout in Oscad will be similar to that of KiCad.
Show Slide	Watch the video available at the following link It summarises the Spoken Tutorial project If you do not have good bandwidth, you can download and watch it
Show Slide	The Spoken Tutorial Project Team Conducts workshops using spoken tutorials Gives certificates for those who pass an online test For more details, please write to contact at spoken hyphen tutorial dot org
Show Slide	Spoken Tutorial Project is a part of the Talk to a Teacher project It is supported by the National Mission on Education through ICT, MHRD, Government of India More information on this Mission is available at spoken hyphen tutorial dot org slash NMEICT hyphen Intro
Remain on previous slide	Hope you found this tutorial useful. This is Rupak and Rakhi from IIT Bombay signing off. Thank you.

Contributors and Content Editors

Nancyvarkey, Rakhiwarriar