# Fixing the Eagle silk screen layer



## mojo

I have been working on a PCB in Eagle, and it's all ready to go except for the silk screen layer.

 Some of the silk screen covers some of the pads, and part of the USB connector outline is off the board (which I want to have panelized and manufactured by Olimex).

 Eagle does not seem to let you edit certain parts of the silk screen, even if you smash the component. I can't find any free Gerber file editors either, so I'm at a loss as to how to fix things. All I can think of is to turn off Eagle's silk screen and draw my own by hand on the document layer, then just export only that.

 I'm probably missing something obvious but any help would be much appreciated


----------



## amb

Can you elaborate for which parts you're having trouble with?
 In some cases the best solution is to create your own library part. This lets you define the silkscreen any way you like.


----------



## mojo

Here is a picture:






 The USB port at the bottom overhangs the edge of the board. The board is 50x40mm, which means Olimex can panellize 8 on to a single board at once 
	

	
	
		
		

		
		
	


	




 If you look closely you can see that the pin headers all have outlines which overlap the pads. Some of the text overlaps other text and holes too (see upper right). It's not a big deal really because all the soldering will be done on the underside of the board, but it certainly doesn't look good.

 PS. I know it's not audio related, but I am working on audio projects as well, I just haven't got beyond the prototyping stage yet!


----------



## amb

I wouldn't worry about the silkscreen on the pin headers. Depending on the fab process they might not actually cover the pads at all.

 As for the USB connector, just make your own library part without the off-board protrusion. You could edit the original part and save it to a new name.


----------



## DaKi][er

Use the Smash command to separate the labels from the parts so you can rearrange them, crosses will appear next to the labels so that you can then move them. There are 2 layers that appear to be part of the silkscreen but are not, so turn off the bottom 2 layers in the layers list, and it'll show what the true silkscreen will look like (I don't have the program in front of me to check what they are named)


----------



## tangent

The white bits you see on the default EAGLE display are not actually the silkscreen layer. It's made of several layers, but only one of them (layer 21) gets output to the Gerber layer by default. The rest of the layers hold things like the crosshairs, the values, etc.

 Another of those layers usually accounts for silkscreen over the pads. A lot of parts in the EAGLE library have annotations and such that cover the pads, or a part outline that continues over the pads, but which will not output that way. This is because part of the part outline (or annotation, or whatever) is on layer 21, and the rest is on another of the layers that EAGLE shows as white. The 3mm LED is a good examples of this.

 If your parts aren't drawn that way, the board house may fix this automatically for you. Ask them. 
	

	
	
		
		

		
		
	


	




 Similarly, the board house should be able to cope with silk going off the board edge. I know for a fact that other board houses do, but my one small experience with Olimex years ago suggests they may not. (They're running a very lean operation.) If the board house can't cope, you can redraw the part to move the problematic sections on to one of the white layers that don't export to Gerber by default. I have a whole series of videos, which includes several on making your own EAGLE parts. Modifying an existing one is more or less a subset of this.


----------



## mojo

Thanks for the repiles everyone, I think I have a solution now. As pointed out, when doing a Gerber export the numbers are not exported. I contacted Olimex and they said that the small amount of remaining overlap would not be an issue.

 There are some weird things about the way Eagle does silk screens. For example, by default the vertical resistors do not have any markings at all so I had to draw little boxes for them.

 I made a new part for the USB header. Thanks for all the advice!


----------



## mojo

*EDIT*

 Don't worry, found the solution...

 For anyone else reading this thread, the trick is to use the "Copy Silk Screen" user program to copy the silk screen to new layers. You can then freely edit those layers, and have them exported when you run a CAM job and produce Gerber files.


----------



## tangent

If you run the script again, it should either toss the contents of the duplicate silk layer, or offer you a way to group the contents of the layer so you can toss it manually. If not, switch to gensik2.ulp, which is very nice. It's available in the contributed files area on cadsoftusa.com.

 This is in my video series, too.

 EDIT: just in case it's not clear, you still make your silk edits on 21, then re-run the script to regenerate the one you use for manufacturing. Because it's a hassle, I generally leave the duplicate one turned off, regenerating it and studying it only right before I got to production.


----------



## mojo

I see. That seems like a better way to do it because the way I was doing it you end up with the silk screen not grouped with the devices any more, making them hard to edit. Thanks for the tip.


----------

