Designing PCB in Altium

• Clicking next will bring Choose Board Units window. Select Metric and click next. Choose Board Profiles will be next, [Custom] is highlighted by default so click next. Choose Board Details is next, Outline Shape is by default Rectangular, from Board Size set Width and Height as 77 mm (roughly equal to 3" x 3" board). For most of your designs it should be enough but if you feel it is small you can increase it to your desired dimensions (Do not use more space than required but use enough so that the components can be soldered in). Keep rest of the settings as it is and click next. This will bring Choose Board Layers next. By default Signals Layers are 2 and Power Planes are 2 as well. You only need Signal Layers right now so make Power Planes equal to 0. Clicking next will bring Choose Via Style, by default Thruhole Vias only is selected so click next. This will bring Choose Component and Routing Technologies next, by default The board has mostly: Surface-mount components selected and Do you put components on both sides of the board: as No. Clicking next will bring Choose Default Track and Via Sizes, click on Minimum Track Size and change it to 0.25 mm, similarly change Minimum Via Width to 1.2 mm, Minimum Via Hole Size to 0.6 mm and Minimum Clearance to 0.25 mm (Although the milling machine can go as low as 0.2 mm for Minimum track width and Minimum Clearance values but try to use suggested values if possible, it makes milling easier and less error prone). Click next and click finish.

2. Layout of Your Design

• A good idea to do before laying out the board is to draw out the major and critical components on paper. This will help you determine the overall orientation of the design.
• We used to prefer single sided boards. The reason was our old way of creating PCB’s was a very delicate process. It was fairly difficult to create a complex single sided board. Creating a complex double sided board was not enjoyable. Making sure all of the drill holes were perfectly lined up and the traces didn’t wash away. Wasted multiple boards.
• Now, it doesn’t matter. It’s just as easy to create a double sided board as a single.
• Grouping similar components is an easy way to lower noise and power losses.
  1. Place individual systems in separate locations on the board.
  2. Separate sensitive components away from “noisy” components. Keep analog away from power supplies.
  3. Separate components with different frequencies. Analog and Digital.
  4. The same goes for different input/output components. Analog and Digital.
  5. Different problems that systems can have: Grouping Components
• Use Ground planes instead of intertwining traces. However, don’t place a component smack in the middle of one. Try to create one in a large open section of your board.
• Ground traces should be as short and thick as possible.
• Major Power traces can be thick if possible, but not as necessary as Grounds.
• Ground and Power planes and traces should be in close proximity to each other if possible, don’t send them in opposite directions around the board. This lowers loop inductance of your power system.

3. Traces – Make them look GOOD

• By intelligently placing the components on the board you can try to minimize the cross overs. Then from toolbar select Interactively Route Connections. Lay the copper route to join all the components, it will replace the routing net which was brought into PCB from Schematics.
• If you want to try the Autoroute, go for it. Then you can adjust the traces if you don’t like them.
• While manually routing
  1. Try to keep the distance as short as possible. The longer your traces are the greater it’s resistance, capacitance and inductance.
  2. Traces should only have angles 45 degrees. Try to avoid right angles and under no circumstances use an angle greater than 90 degrees. This is important to give a professional and neat appearance to your board. That’s really the only major reason for this.
  3. Forget nice rounded trace corners, they are harder and slower to place and have no real advantage.
  4. Make sure the traces go through the exact center of the pads and components. Again, looks and gives you the most clearance.
  5. “Neck down: between pads where possible. Changing your trace from large to small and then back to large again if you need to go between pads.
• If you Power and Ground traces are critical, then lay them down first.
• Symmetry is very professional. It’s all about the looks.
• Don’t place vias under components.
• Try to use through hole components to connect top tracks to bottom tracks. This cuts down the number of vias needed. Less holes, less time to assemble.
• After raouting is complete click Tools >> Design rule Check. It will show you if you missed something or made some mistake will routing. Do check this before finalizing your design. Remove all the Errors and try to remove (if no possible then minimize) all the warnings as well.
• Now is the time to cover remaining of the board with copper so that minimum of etching is required. For this click Place >> Polygon Pour . This will bring up a window in that use Fill mode as Solid(Copper Regions) and set Remove Islands less than as 3 sq. mm, leave other two values as default. Set Connect to Net as Ground and set Layer as Top Layer. A big + sign will appear use it to draw and cover whole Top Layer it will cover everything on Top layer leaving only route traces. An easy way of doing it is to click on top most left corner of the board and go towards bottom most right corner. A 90 degree triangle will be forming covering half of the board (if it is not then while drawing press shift+space on key board it will change shapes and when it becomes triangle click on bottom most right corner) then click top most right corner and then press Escape. Do same for Bottom Layer as well for this first select the bottom layer from bottom menu (typically blue color with bottom caption) and follow the same procedure used for top layer.

4. Finishing

• Review all of the traces and connections. Make any changes that may need it.
• Is there anything that could be done better?
• Make sure that you have poured copper on both layers to fill unnecessary gaps.

5. Exporting

• Select File >> Fabrication Outputs >> Gerber Files
• Select Units as inches and Format as 4:2
• Click below Layers.
  1. Top Layer (GTL),
  2. Bottom Layer (GBL),
  3. Mechanical 1 (GM1)---This is optional
• Click OK. It will generate CAMStatic file as well. This is only for viewing and is not required for milling.
• Now you have to generate the drill files for that File >> Fabrication Outputs >> NC Drill Files. Select Units as Millimeters and Format as 4:2. This will generate drill file in *.TXT format.The available sizes of the drill bits we have in stock (mm): 0.5,0.6,0.8,0.9,1.0,1.1,1.2,1.4 1.5,1.8,2.0,2.95 & 3.0.Please make sure your drill hole size is available.Otherwise change the hole size according to the availability.

6. Final Step

Please follow Requirement