Workshop - Introduction guide to Altium/Protel
Altium / Protel is a CAD package for the design of printed circuit boards. It comprises two separate packages:
- Advanced schematic, and
- Advanced PCB.
These are completely separate programs, and can be run individually if desired, or combined together to form a complete CAD solution. Each has their own library editor for creating new components.
Advanced Schematic
This is where you draw your schematic diagram. First of all, you need to load a library of parts, then place the appropriate parts on the page. You then connect all the parts with wires. If you only want to draw a schematic diagram, then this is all you need to do. However, if you want to produce a PCB, there are several other tasks you need to do. The two most important ones are:
- Designating a footprint, and
- Annotating the circuit.
What is a footprint?
This is the shape of the component you will use on the board. A single component may have many possible footprints, so it's important that you specify the one you want to use. For example, a surface mount resistor could be a 1206, 0805 or 0603 part.
Annotating the Circuit
This involves giving each part a unique identifier. For example, you may call the resistors R1, R2, R3 and so on. Protel can do this automatically for you using the Annotate option. It is important that you do this, as the PCB software will only recognise single entities, so if two parts have the same name, it will only load the first one it sees.
Having done all this, you then export a netlist. A netlist is a list of all the components, and how they are connected to each other. These connections are called nodes . You have the choice of either naming the nodes yourself, or Protel will number them for you. It is a good idea to name critical nets, so when you layout the PCB, it is clear which tracks are important. Some example node names could be: INPUT, TUNE, PROGRAM etc.
Making your own parts
Usually, the parts you require can be found in one of the libraries. However, sometimes you will need to create your own component. This is what the component editor is for. It is a good idea to first of all, create your own library, then add your new parts to your own library, rather than writing to the exisiting libraries. Creating a new component is simply a matter of drawing it's schematic diagram in a separate window, and saving it to a library.
Advanced PCB
The workshop has certain limitation governing PCB production, and it's important to be aware of these before starting to layout your board. The most important factor is the board size. The workshop provide several different sized templates which you should base your board design around.
After deciding on a template to use, you load the netlist you produced in the schematic software. You should then see the component footprints appearing on the screen, and a whole bunch of lines joining them together. This is the ratsnest, and these lines correspond to the nodes or connections in your schematic. They are used as a guide to assist you in routing tracks between the components.
You should also look closely at any error messages loading the netlist produces. Things like missing footprints or components are critical, and should be attended to before proceeding. Loading the netlist should not cause any errors if you have the appropriate libraries loaded, and all the components were designated properly.
Layers
You should also decide if you want a single or double sided board. A double sided board will have tracks on both the top and bottom, whereas a single sided board only has tracks on one layer, usually the bottom. Protel allows you to use many different layers, and each layer is color coded. The layers you will work with most frequently are:
- Top component overlay, (yellow)
- Top copper layer (red)
- Bottom copper layer (royal blue)
- Bottom component overlay (greenish/brown)
- Ratsnest (greenish/blue)
- Multilayer (grey)
- Pad holes (dark blue)
The component overlays show the footprint of the component, and are usually silkscreened onto the board. The workshop does not produce boards with component overlays on them. However, you should still use these layers, as they assist in producing an efficient design.
The next step is to move the components around to get a neat layout and to minimise track lengths and the number of vias you have. A via is a connection from the top layer to the bottom layer, and is made by drilling a hole through the board, and soldering a piece of wire on both sides. You should avoid using these if possible, as it means you will have to drill more holes, and make more solder joints.
Use the ratsnest to aid in placing components, and optimise all connections frequently.
Routing
Protel claims to have an auto-routing feature. DO NOT use it! You will achieve a much better layout by hand, and you have a far greater level of control. I recommend you manually route all connections. This involves placing a track from one pad to another, following the ratsnest guide-lines. Do this for all the nodes in your circuit.
Design Rule Check
A DRC allows you to check for things like un-routed connections, missing components, wrongly connected components etc. You should do this after routing your board to check it's validity. It will use the netlist you created in the schematic program, so be sure this is correct.
Recommendations
- Any text you place on the bottom layer must be mirrored - that is, backwards, since you are looking at the board from above, but when it's made, you will look from the bottom.
- Work in mil and not mm. The electronics industry works on standard spacings of 100mil which is 1/10th of an inch (2.54mm) .
- Always use the thickest track possible. I recommend 50mil, or 24mil if absolutely necessary. I would certainly not go below 12mil for anything, and even then, only for very short distances. If you need to squeeze a track between IC pads, use thick tracks up to the pads, a thin track between the pads, then step back up to a thick track again.
- Make the pads as large as possible. Remember that you are going to have to drill holes through these pads, then solder components to them, so give yourself plenty of room. As a minimum, I recommend 62mil, but often use 100mil when space is not critical.
- Do not use square corners to join tracks. Use a chamfered corner instead.
- Shrink the size of the text on the component overlay to 30mil, and move the text close to the component so you can identify them easily.
Example Design
This example shows the schematic and PCB for a simple amplifier. You will draw this schematic, and layout the PCB during one of your lab classes. It uses a single sided board (all tracks and pads on the bottom layer) and has a component overlay on the top of the board. All tracks are 50mil except for a small length of 24mil track connecting the transistor. Note that all I/O connectors are grouped together on one side of the board, and the components are nicely spaced apart.
