1
\$\begingroup\$

I made a schematic for a 5 band analog EQ. I used OP Amps to make active bandpass filters for various frequencies within the human hearing range which means when I made my schematic I drew 5 OP Amps in total (one for each frequency) as shown here:

enter image description here

The actual IC I'm using for the OP Amps is the LM 833 which actually has two amps inside it per chip:

enter image description here

I made a custom footprint for the LM833 but I want to associate it with two of the OP Amp symbols I made on my schematic so that when I generate the netlist only 3 LM833 ICs are generated and the correct connections are automatically made according to my schematic. How do I do this?

\$\endgroup\$
2
  • \$\begingroup\$ Search: does kicad support heterogeneous symbols. I expect it does but it may call them something else. \$\endgroup\$ – Andy aka Jan 19 at 19:27
  • 1
    \$\begingroup\$ you can assign whatever footprint you want to the same symbol in the schematic. The connection between the symbol and footprint is the pin numbering. This works just as well for "multiple units" such as dual/quad devices, except all the "unit" symbols of the part share the definition of various properties, including footprint. \$\endgroup\$ – Pete W Jan 19 at 20:42
3
\$\begingroup\$

Due to architectural limitations in Kicad, it is impossible to associate multiple symbols with one footprint. This is because the symbols carry the pin mapping information directly. In other CAD packages, there is a mapping layer in between that can remap the symbol pins to the footprint pins. In Kicad, what you have to do is make one symbol with two sub-symbols, one for each of the two amplifiers in the device, and with the appropriate pins assigned on each sub-symbol. Then, you need to make sure to instantiate both sub-symbols in the schematic for each IC.

\$\endgroup\$
6
  • \$\begingroup\$ will it be possible to re-use the same pin number for multiple sub-symbols though? Since, for example, two OP Amp symbols will share pins 4 and 8 since they power the IC \$\endgroup\$ – Andrew Jan 20 at 2:31
  • \$\begingroup\$ No. There are generally two solutions for that: either put the power pins on one of the amplifier sub-symbols, or add a separate sub-symbol for power. Also note that kicad has another related architectural limitation: the refdes information must be placed in the same location on all sub-symbols. \$\endgroup\$ – alex.forencich Jan 20 at 2:42
  • \$\begingroup\$ As to the second method: but the separate sub-symbol for power still has to have pin numbers associated with it (to match the footprint) and so will end up being used with multiple symbols that have the same reference value. Wouldn't this mean I have two OP Amp symbols on my schematic which are both U1 (for eg) but if I make the power sub-symbol, C (for eg), then I'll have two symbols which have U1C on them (in attempting to associate two symbols with one reference U1)? KiCad gives me an error when I try to assign the same pins on different symbols to the same reference value as in my example. \$\endgroup\$ – Andrew Jan 20 at 3:21
  • \$\begingroup\$ Why would you try to instantiate the power sub-symbol more than once? \$\endgroup\$ – alex.forencich Jan 20 at 3:23
  • \$\begingroup\$ simply to show the connections of each OP Amp. It would be strange to have one symbol on a schematic with all the connections visible and then another one with fewer connections visible. It's a loss in continuity. Maybe I want to present the schematic and be functional for PCB creation for example \$\endgroup\$ – Andrew Jan 20 at 3:24
2
\$\begingroup\$

Symbols can have multiple units, the one for the LM855 should have unit A and unit B, these then map to the appropriate place on the footprint.

If you chose a generic opamp rather than a dual part when making the schematic this may not be an option. The pin out of the part you show is standard for a dual opamp so if you don’t want to make your own symbol you should be able to find something suitable.

\$\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.