Go Down

Topic: Silk screen on PCB how would you do it? EAGLE (Read 15 times) previous topic - next topic

nickvd

#5
Feb 07, 2011, 04:34 am Last Edit: Feb 09, 2011, 09:40 am by nickvd Reason: 1
You can use the squash tool to separate the part values and names from the parts themselves, that way you can place them where they make sense..

First squash the part (click on it using the squash tool) then use the move tool to move the text around...


Edit:  Um yeah... smash, that's the one... lets just pretend I didn't say 'squash tool'... ;)

westfw

Quote
I can't find a way to reposition names

Use the "Smash" command, or the "run smash_all.ulp"  This "separates" the names and values from the parts, and allows you to move them around, change the layers, change the size, etc.

Another thing I find useful are the silkscreen modifying ULPs.  (I think the most recent is silk_gen.ulp; ftp://ftp.cadsoft.de/eagle/userfiles/ulp/silk_gen.ulp )  Normally, these are for making sure that the silk screen meets the required design rules for line width and so on (silk screen line widths are (were?) frequently not allowed to be as fine as copper layers, and library designers didn't pay much attention, especially with text labels.  So there's a fixup.)  However, the way they work is that they copy all of the elements that would appear on the silkscreen (possibly fixed) to a new layer.  Once that has happened, you can go in and edit that layer as much as you want before exporting IT to the SS gerbers.  (beware that it doesn't stay in sync with parts, so you need to do this AFTER the rest of the board is finalized.)

liudr

#7
Feb 07, 2011, 06:16 am Last Edit: Feb 07, 2011, 03:42 pm by liudr Reason: 1
Thank you very much everyone! Here is what I've found out with your suggestions, just in case others are interested in this topic:

(This paragraph needs changes)If a part has NAME and VALUE in its library with its outline, then the NAME and VALUE show up in tPlace layer just as the part's outline, instead of tNAME or tVALUE layers. If a part doesn't have NAME and VALUE in its library with its outline, then NAME and VALUE only show in tNAME and tVALUE layers.

To move the NAME and VALUE in board view, select the part and show its property then check "Smashed". Now the NAME or VALUE can be moved around. If you move the part, the NAME and VALUE still follow the part around. If you "unsmash" the part, its NAME and VALUE go back to default locations or locations designed in the library.

westfw, I've saved your tips on managing silk screen in my EAGLE tips document, besides "how to duplicate a part in the library" I received from James C4S  ;)

westfw

I don't think the first part of that is true.  It depends on how the library was made.
In theory, you put (when you make the library) ">name" on the tNames layer, and ">value" on the "tvalues" layer, but people tend to be careless and leave them on "tPlace" (the default drawing layer in the package editor), in which case they show up on tPlace.  If you leave them out entirely, you won't get any names on your silkscreen (or in the board editor, or anywhere else.)

liudr

I see. I tried the following. If I design a package and choose the appropriate layer for ">name" it will show up in board view in layer tNames. But if I don't include ">name" in my package, the name will NOT show up in the board view at all. Same thing goes with symbol and schematic view. Did I get it right this time?

Besides, I didn't find how to enable user-definable value for my simple part. The value shows up as device name+variant name. If I attempt to change it, EAGLE asks me "There is no user-definable value, do you want to change anyway?" Can I indicate somewhere in the library that there IS a user-definable value, like a resistor value? Thanks.


Go Up