1
\$\begingroup\$

I'm designing a board with Eagle and I have placed some LEDs from the led library that comes with Eagle.

LED Properties dialog

With the default layers activated, the LED looks correct in the Board (the anode and cathode can be distinguished by the flat part of the LED) However when Exporting the board for manufacturing, the LED looks different and it's not possible to distinguish the anode from the cathode (which may lead to solder it incorrectly).

After investigating a bit I realized that what I see in the design is actually a combination of the tPlace and tDocu layers (I'm guessing they where added later in a revision but in the incorrect layer). When exporting the board to be manufactured, only the tPlace layer gets printed in the board and the tDocu gets discarded in the physical product.

Both tDocu and tPlace

Only tPlace

Export result

Since it's not a library that I made but a library provided by Eagle I'm wondering if:

  1. Can I modify and correct the libraries provided by Eagle?

  2. Can I force the tDocu layer to be printed in the actual board (to both tPlace and tDocu get printed)

I can of course create my own components, but if I can use the standard components it will save me a lot of time.

\$\endgroup\$
  • \$\begingroup\$ Use the 5mm part. Pin pitch is the same, and the symbol is more recognizable. Or, draw a diode symbol on the board yourself. \$\endgroup\$ – CrossRoads May 2 at 17:27
  • \$\begingroup\$ Or make your own symbol, only takes a few minutes for a simple part like a diode. Or maybe try some of the Sparkfun or Adafruit symbols. \$\endgroup\$ – CrossRoads May 2 at 17:42
  • \$\begingroup\$ If you're looking for a quick fix with a few LEDs, just draw lines on the tPlace layer over the lines on the tDocu layer. \$\endgroup\$ – c10yas May 3 at 6:25
2
\$\begingroup\$

tDocu is not supposed to be printed in most cases. However if you intend to print, you can do so by going to CAM processor and then selecting the template which is used for exporting your gerbers:

CAM

Select Silkscreen Top on the left panel. You can see that mine has only layers 21 and 25 selected.

You can include tDocu layer here by clicking the red circled button and selecting tDocu layer (51).

Save it and generate your gerbers. Before sending to fab house, check the gerbers with a third party gerber viewer tool to ensure that tDocu is included in silkscreen print.

\$\endgroup\$
  • \$\begingroup\$ If there's other stuff on the tDocu layer you don't want printed in the silkscreen see my comment to the question \$\endgroup\$ – c10yas May 3 at 6:26
  • \$\begingroup\$ Thanks, that's something I can do as a quick fix to solve my problem \$\endgroup\$ – Sembei Norimaki May 3 at 10:34

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.