Generating Gerber files for boards with external modules

Mark,

Like Rob, I have never run across a board house that doesn't remove

silkscreen from areas that don't have solder mask on them.  The end

result is that despite what may be in a set of getber files, silkscreen

is limited to being printed on solder mask.

Double check with your board house, but this may not be an issue.

    - Chuck

On 06/07/2016 03:09 AM, markusbass wrote:

I'm looking for a way to generate Gerber files for PC boards that use external modules (like e.g. LCD display module). The problem is that the external module shape may be printed on pads on the main board (which causes problems when soldering the board).

In KiCAD there is an option "Subtract soldermask from silkscreen" that solves the problem. Is there a similar option in Eagle, or a script that can "fix" generated Gerber files?

 

Mark

 

--

To view any images and attachments in this post, visit:

https://www.element14.com/community/message/198904

On 07/06/16 15:35, markusbass wrote:

Instead, I'm looking for a method of "fixing" the Gerber files (possibly with a script), or creating them correctly (in the same way as KiCAD does). The existence of this solution in KiCAD proves that it is possible. The only question is how difficult is to implement the same solution in Eagle.

The board houses I use all perform this operation themselves as a

post-processing step on the Gerbers. Essentially it's a matter of

masking the silk screen Gerber using the solder mask one.

markusbass wrote:

This is module created by me. But I'm afraid that in general case it is not possible to modify the library in the way that the module shape does not overlay the pads on the main board (which I even don't have when creating the library). Even if I leave the shape of the module, it can overlay the pads on the main board (because I don't know the board in advance). This would force me to modify the library element each time I use it with a different main board. Instead, I'm looking for a method of "fixing" the Gerber files (possibly with a script), or creating them correctly (in the same way as KiCAD does). The existence of this solution in KiCAD proves that it is possible. The only question is how difficult is to implement the same solution in Eagle.

On the tPlace layer (i.e. what will become the silk screen) just put a tiny pin 1 marker or some small but clear orientation marker. Then take that into consideration when you do each of your layouts. The the full body of the module gets drawn on tDocu and this gets used when creating the assembly drawings so you can have all the detail you like on there. I've used this technique for both modules and regular components and it works fine this way.

I imagine you could possibly do something in ULP to try and fix things up before you run the CAM processor but I am not sure how I would go about that one if I were to want to try it.

Best Regards,

Rachael

rachaelp wrote:

Do you mean that for the external modules you are using module vendor supplied or community sourced library parts for the modules? Or is it a part you have created yourself? In either case then just fix the library part so the shape doesn't overlay the pads. Maybe in the library part copy the whole module outline to tDocu so you can put it on an assembly drawing but then on the tPlace layer just put enough info so you can easily identify the correct orientation for the module when you attach it to the board.

This is module created by me. But I'm afraid that in general case it is not possible to modify the library in the way that the module shape does not overlay the pads on the main board (which I even don't have when creating the library). Even if I leave the shape of the module, it can overlay the pads on the main board (because I don't know the board in advance). This would force me to modify the library element each time I use it with a different main board. Instead, I'm looking for a method of "fixing" the Gerber files (possibly with a script), or creating them correctly (in the same way as KiCAD does). The existence of this solution in KiCAD proves that it is possible. The only question is how difficult is to implement the same solution in Eagle.

Mark

Hi Mark,

Do you mean that for the external modules you are using module vendor supplied or community sourced library parts for the modules? Or is it a part you have created yourself? In either case then just fix the library part so the shape doesn't overlay the pads. Maybe in the library part copy the whole module outline to tDocu so you can put it on an assembly drawing but then on the tPlace layer just put enough info so you can easily identify the correct orientation for the module when you attach it to the board.

Best Regards,

Rachael