5
\$\begingroup\$

I have a few sensors (potoresistor, temp sensor...) that connect to the board indirectly. The PCB will have a connector such as the molex 4pin fan connector that will in turn connect to the sensor/device via a short cable.

How do I show this in the schematic and the PCB layout? If I select sensor schematic I would have to manually add the pcb footprint to the component. If I select schematic for the connector then adding a resistor to a random pin of a connector doesn't seem right either.

\$\endgroup\$
  • 2
    \$\begingroup\$ This really depends on your CAD. Which one do you use? \$\endgroup\$ – venny Aug 22 '14 at 21:27
  • \$\begingroup\$ @venny EagleCAD though am new to it (kicad before). I would like a generalized answer as well so I am not stuck when using different cad software... \$\endgroup\$ – DominicM Aug 22 '14 at 21:31
2
\$\begingroup\$

I normally choose one of these two options:

  1. Draw the sensor as a schematic symbol and have a footprint for the desired connector. The only problem is that the BOM is not complete then (you can either have the sensor or the connector).
  2. Draw a symbol for the connector with two connections for each lead in the schematic symbol (so you draw one "symbol" with both the jack and the plug). You can then make a schematic symbol for the sensor and connect it to the other side of the connector. Finally you only give the connector a footprint, and leave the footprint for the sensor out.

An example of a schematic symbol for a connector can be:

Coaxial connector schematic symbol

Good luck designing your circuit!

\$\endgroup\$
3
\$\begingroup\$

In general, place the connector symbol to schematic and connect it to appropriate nets - it does not have to be in the correct order, because later you can adjust it from layout editor with pinswap command.

For clarity, 'dummy' symbol with no footprint can be placed to schematic, to indicate what will be connected to the wires.

\$\endgroup\$
3
\$\begingroup\$

(For me.)

On the pcb there's the connector footprint and label.
If there are some important pins I might add text. (+V, GND, sig) to help with testing/ trouble shooting.

The schematic tells the story and I'll add in what's on the other end of the connector. (maybe it's a thermistor that is one leg of a Wheatsone bridge.) I figure I want anyone else who looks at the schematic to be able to understand out what's going on.

\$\endgroup\$
2
+50
\$\begingroup\$

In Altium, there are different types of components defined:

enter image description here

"Graphical" parts are included on the schematic but it isn't checked by DRC and isn't added to the BOM or netlist, so it doesnt' appear in the layout.

"Mechanical" parts are included on the BOM, but not the netlist.

You can make your part either Graphical or Mechanical depending whether you want it included on the PCBA BOM or not.

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.