Demo1    <<-BACK            HOME            UP --^           NEXT-->>  Demo-3
side4linux, a simple integrated development environment!
PCBS Demo-2     Layout the Printed Circuit Board and create the Gerber files for the 'Try1' Project PCB.

Purpose:  To provide a basic introduction to creating a new Printed Circuit Board design using 'side4linux' 'gEDA' and 'pcb'. We will build a Serial Communications input/output Printed Circuit Board from the schematic generated in Demo-1.  Please keep in mind that this is only a Demo, the actual printed circuit board of the Machine Controller is to be presented in a later Demo along with exercises in how to use it so do not attempt to fabricate this board.

Requirements: Make sure that the 'GNOME' build environment is installed correctly, if not then read 'setup C build environment.txt' and also 'setup GNOME build environment.txt'.

 Further requirements: Make sure that the latest PCBS support package is installed correctly.


Pre-Requisites: Read through the Overview and do Demo-1 first.

A photo of the bare PCB is shown next,
Bare Serial1 PCB
Scanshot of the bare Serial1 PCB before the fitting of components. Note copper is on the component side.
So to begin making the PCB we will firstly look at the Sample2 examples,
  1. Open 'side4linux' and click on Project>Open Project in the Main Menue.
  2. Double click on the 'DEMOS' Product Area,
  3. Double click on the 'SIDEdemos' Product,
  4. In the file dialog double click the  'PCBS' folder. This takes you to where PCB projects are kept.
  5. Double click on 'Sample2', this opens the 'Sample2' project folder.
  6. Double click on 'Sample2.prf'. This opens the 'Sample2' project file.
  7. Notice that the left bottom status bar window says 'Project: Sample2' which is the Project Name.
  8. Notice that the next window says 'Ptype: PCBS' which is the Project Type.
  9. Click on the 'File Explorer' 'Files' tab on the left and view what schematic files are actually in the Project ('serial1' & 'serial1_connectors').
  10. Click on 'Tools>PCBS>Run PCB, minimise the 'Component Library' window and maximise the main window of the 'pcb' program.
  11. Load the layout file 'serial1.new.pcb' from the main menue of 'pcb' ('File>Load Layout').
  12. It should look like the graphic below,
Sample2 Layout
Screenshot of the Sample2/Serial1 PCB Component Layout

Now load the file 'serial1.pcb', this is the manually routed printed circuit board. The earlier file is erased when you load a new layout.

Serial1 Manual Routed
Screenshot of the Sample2/Serial1 PCB Manually Routed Layout, a 'single layer' board.

Now load the file 'serial1.autorouted.pcb', this is the automatically routed printed circuit board.

Serial1 PCB Autorouted
Screenshot of the Sample2/Serial1 PCB Auto Routed Layout.
Practical 1: Run 'pcb' and load the Layout file for the 'Serial1' Printed Circuit Board,

Let us try to copy the 'Sample2' examples using Project 'Try1',
  1. Close the 'pcb' board program.
  2. Close the 'Sample2' Project 'Project>Close Project'.
  3. Open your Project 'Try1', Project>Open Project in the Main Menue of the IDE.
  4. Click on the 'File Explorer' 'Files' tab on the left and view what schematic files are actually in the Project ('serial1' & 'serial1_connectors').
  5. Click on 'Tools>PCBS>Run PCB, close the 'PCB Log ' window and maximise the main window of the 'pcb' program.
  6. Load the layout file 'board.pcb' from the main menue of 'pcb' ('File>Load Layout').
  7. Save the layout file as 'try1.pcb' 'File>Save layout as'.
  8. Remember that your are dealing with 'mils', A 'mil' is 1/1000th of an inch and spacing is usually in 10 mill increments.
  9. At this stage all you have is all the components bunched up in the top left hand corner so try clicking on 'Select>Disperse all elements'.
  10. Now drag and rotate the components to match the screen shot of the Sample2/Serial1 PCB Component Layout above.
  11. If you have forgotten how to drag and rotate then re-read the 'Overview'.
  12. Remember to save early and save often during your editing!
  13. Try to get all of the compenents within a 1.6 inch square (use the mouse cusor and read the X/Y values top right of screen).
  14. Now resize the board to 1.6 inches square.
  15. Go to 'File>Preferences>Sizes>Board Size' and set both 'Width' and 'Height' to 1600.0 (1600 mils = 1.6 inches).
  16. At this point you can load the netlist file 'board.net' into the Layout,  'File>Load layout'.
  17. Close the 'PCB Netlist' window.
  18. Type a lower case 'o' that is 'ooh' and not zero!
  19. This should now expose the 'ratsnest' which is the unrouted connections of the board.
  20. Save the file again (keep doing this!).
  21. You should now have something like the following graphic on your screen,
Try1 ratesnest
Screenshot of Try1's Layout with ratsnest.

Practical 2: Route the 'Serial1' Printed Circuit Board tracks and produce output files.
  1. At this point if you require a single layer board you could manually route  by selecting 'Line' mode and draw in the tracks.
  2. We will make this short as it is only a Demo by using the automatic routing facilities, click on 'Connects>Auto route all tracks'.
  3. 'The PCB Log' window should come up with '30 of 30 nets successfully routed. Congratulations!! The layout is complete and has no shorted nets.'.
  4. Close the 'PCB Log' window and try using the autoroute optimisations  'Optimise autorouted tracks'.
  5. End with the 'Miter' optimisation.
  6. Save the Layout again (keep doing this!).
  7. Now for some output,  'File>Export layout>ps' to create a postscript print file of about ten pages.
  8. Now for the  'Gerber' and drill files for the board maker 'File"Export layout>gerber'.
  9. You could now save the layout file and close the 'pcb' program as we are now done with it.
  10. Close the Project and close down the side4linux IDE.
  11. In Practical-3 we will look at the output which could be used to make this demo board.

Practical 3: View the 'Serial1' Printed Circuit Board output files.
  1. You may convert the postscript file from Demo-2 into 'PDF' using 'ps2pdf' (re-read the Overview if you have forgotten).
  2. Open your 'PDF' reader and look at the pages of output, one of these could be used to create a 'master' using your printer.
  3. Open the side4linux IDE and and the 'Try1' Project then select the gerber viewer 'Tools>PCBS>Gerber Viewer'.
  4. Click the 'On' button top right hand side.
  5. Try clicking layers on and off (coloured buttons' below 'On" button) to see what each layer is.
  6. View your work which should look something like the following graphic,
Try1 Gerber View
Screenshot of the output of the Gerber viewer 'gerbv'

If this board was going to a commercial board maker ( and it is only a demonstration exercise so it is not ) you would send along the 'PDF' file that you have created along with the files ending in 'gbr' and the 'Excelon' 'cnc' drill file 'try1.plated hole.cnc'. The 'PDF' so the board maker can see what you want and the rest to manufacture your board. Note that as this is a two sided board, you need to specify to the board maker that you will require plated through holes. Should you actually need a working example of the serial interface then check out the Project 'Serial1' in the PCBS folder, this is the serial interface used with the prototype CPU shown in the 'overview'. Please note that we will not be providing support for any prototype Projects that we are releasing so use prototypes at your own risk!

Real Serial1 PCB
Screenshot of the real Serial1 PCB
(Note the header pins and the connector pins are on the same side to allow for a single sided board.
This means cutting an access hole in the 'mother board' to connect the headers to the serial outlet sockets!)

In Demo-3 we will build and assemble the Machine Controller programming interface PCB and cables.

We will provide other demos as 'side4linux' develops to cover integration into a real world machine controller.