- Muchas notas - Fran Acién

20230301 - Altium advices

Here some advices that I will follow from now on:

  • Components and schematics are in Mills! PCB and footprints in mm Source

A general advice. It is necessary to have a prototype that you can play with before creating the schematics and pcb. Specially in microcontrollers or this SoC, becuase it is necessary to know how it works in a well known environment.

Symbol creation

Schematic creation

  • NEVER NEVER NEVER UPDATE ALL THE COMPONENTS FROM LIBRARY, this will generate that all your parameters are going to be deleted.
  • Units naming:
    • Resistor -> 1K, 2K, 2.2K..… NO 2K2 VALUES! And 1R, 100R, 50R.
    • Capacitor -> 1uF, 1nF, 100nF.… NO 0.1 VALUES!
  • Properties > General > Units
    • Mils always
    • Visible grid 100mil
    • Snap grid 100mil
    • Snap distance 100mil
  • Harness
    • Harness ports in MAYUS, with the name of the connection. For example, if it is a spi bus from a SX1272 the port name should be “SPI_SX1272”
    • Harness types readable, with spaces and minus if necessary, with generic names. Like “SPI bus”, “i2c bus”
    • I prefer to use harness rather than busses. Use harnnes to export the signals of a module. Create a harness bus for every bus of pins with the same purpose.
    • Dont create a harness for a GPIOS, create a harness of signal pins and then connect them in the schematic of the microcontroller.
  • Error report
    • Go to Project > Project options > Error Reporting
      • Nets with multiple names to No Report
      • Nets with no driving source to Error
  • The GPIOS of the microcontroller/CPU needs to be selected so is easy to route. If there are multiple options, go for the easies to draw, then everything is more beautiful and cleaner.
  • The naming convention for the nets in each page will be:
    • When the signal is characteristic of one device, and other is connected to that device, it should be the same name for all and a prefix with the characteristic. For example, a modem that is connected to a ucontroller, the lines will be M_* from Modem.
    • When there are multiple devices accessing a common bus, each device should have a prefix with their device, and connected to the bus. Like for example, ESP_SDA, and then SENSOR1_SDA, SENSOR2_SDA, etc.
  • Put test points of all the voltages and necessary for fast diagnostics on TOP and BOTTOM.
  • Put descriptive names to the test points, no TP21. The way I do it is to put a easy to read identifier (3V3_TP) and then in the PCB, I hide it and add a silkscreen (3V3).

PCB Creation

  • Check two times the orientation of the connectors!
  • A description of the SolderBridges or the TestPoints is always welcome
  • Put solderbridges to change all the modes in all components. For example, if strong pull up is low speed and low pull up is eco mode, put both to test the differences.
  • Check that the solderbridges are correctly placed. They will say is working perfectly but you never know. ALSO. Be careful with the vias that goes to power planes and connected to vias, they are going to be directly connected. Put NO CONNECT to all vias and pads, and then you need to put POLYGON POUR CUTOFF to the vias, so they don connect to ground planes. Check a few times
  • Dont put vias near pads you are going to solder.
  • When you dont want to use the hotspot snap (this is that the component is moved automatically to avoid obstacles or being in the grid), you can press ctrl, and you have full control on the position
  • Be careful with the through holes that are connected to ground planes. You need to put thermal reliefs and also put big pads, otherwise is going to be difficult to solder it.
  • Try not to use BGA
  • In general have in mind that if there is a lot of area of pad then is gonna be difficult to solder it.
  • Be sure that all the components has the mark for its orientation
  • The leds should have the description of what are them
  • The SPDT buttons should have the text when they are ON or OFF.
  • The silkscreen needs to go from the edge of the PCB to the inside, when putting perpendicular letters for ports, is more easy to read
  • Try to keep the same orientation for the labels. A good one is to put all the verticals looking to the right

When doing a PCB the steps are:

  1. Placement. Important the right orientation of the components
  2. Connect the radio tracks
  3. Connect the clocks and high frequency signals
  4. Connect the rest
  5. The last is the voltages
  6. Then Create the repours
  7. Then via stitching

Release