Adding an additional PDIP


Running v5.99

I have my schematic completed and started to layout PCB. I want to add an addition PDIP socket to supplement a TSOP that is in Eeshama.

When I add the footprint the PCB editor I am not able to make the connections. I have tried searching for the normal terms in Eeshams (PDIP, DIP, DIL, Socket, connectors etc) but cannot find anything just physical parts.

Other than bodging in the schematic is there a ‘proper’ way to do this simple task in PCB Editor.


It’s not clear from your description, but it sounds you trying to add a PDIP socket in parallel with an existing TSOP package, perhaps so that you can use THT packages, or test it using a TSOP to PDIP adapter. If you add the socket in the PCB editor only the socket connections will not “take”, because its pads are not part of nets. You have to go back to eeschema and add a socket there, then update the PCB. It’s the same story with other parts you may want to add that need to be connected.

Hi Retiredfeline,

Yes that’s exactly what I’m trying to do. I have a number of breakout boards for Vero that I want to use in addition to new components.
I do think this is a limitation - although I understand the reasons for not connecting the new footprint. It would be nice if a local connection could be made in the PCB editor which could override the normal behaviour for such an situation.

I have started making a new Eeschema component which I can parallel up the connections and then assign this to a standard PDIP footprint - messy to say the least


Make sure you put local labels on your original IC. Place a second instance of the IC on the schematic and connect it up using labels only. Annotate it. Change the footprint of this second instance to the alternative footprint and update your board.
You can put the alternative symbol in a separate area on the schematic or even on a different sheet if you use global labels.
Using labels is the best way to keep this sort of thing neat.

There are a few ways to do this, and they’re all quite bad, ugly or relative time consuming. The best option is probably the last one, to do it in the footprint editor.

In the schematic, the easiest way is to just add a aschematic symbol for each of them, and connect them in parallel. Either with wires or with labels.

You can add a layer of abstraction in the schematic by creating a hierarchical sheet for this IC. Then you draw the “Sheet symbol” very much alike your IC, and on the sheet itself you put both instances of the IC.

In Pcbnew you can force the interactive router to allow DRC violations: Pcbnew / Router / Interactive Router Settings and then set t: Mode / Highlicht Collisions and Options / Allow DRC violations

Disadvantage of this is that it’s quite error prone, and they also will be flagged later if you run DRC.

You can directly modify the netlist in Pcbnew (in V5.99, which has become V6.0.0-rc1 a few weeks ago). Right click on a pad of the footprint, edit the properties of the pin and then you can select one of the existing Net names from the drop down list:

These changes seem to persist if the PCB is updated, but I’m not sure how well tested this is.

Another way of doing this is to create a custom footprint. To do this:

  1. Create a custom library and add the PDIP footprint to it. (Because the default libraries can not be edited) Also give it some other name to avoid confusion.
  2. Open the TSOP footprint in the Footprint editor.
  3. Select everything by dragging a box around it.
  4. Copy it to the clipboard.
  5. Open the PDIP again in the Footprint Editor.
  6. Paste the items of the TSOP package in your custom PDIP.
  7. Clean it up and save.

KiCad assumes that pads with the same number have to be connected on the PCB, so this only works properly if the functions for the pins are mapped to the same pin numbers in both packages. If the pin mapping is different between the two packages, then you have to renumber the pins to match the functions between the two packages.

Another example of why starting with modifying the schematic is simply far easier

1 Like

Thank you all for your advice - in the end I made a symbol in the schematic called PDIP, paralleled the connections and assigned the appropriate footprint.

Note to Devs - it would be nice if this could be addressed - wouldn’t the simplest option would be to have the option to assign a different footprint under the RMB > ‘Duplicate’ menu So you’d have - ‘Duplicate’ and ‘Duplicate with New Footprint’ options.
PCB designs are not intrinsically wedded to the schematic in all situations.

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.