Pages: [1]   Go Down
Author Topic: Silk screen on PCB how would you do it? EAGLE  (Read 14462 times)
0 Members and 1 Guest are viewing this topic.
Central MN, USA
Offline Offline
Tesla Member
***
Karma: 72
Posts: 7171
Phi_prompt, phi_interfaces, phi-2 shields, phi-panels
View Profile
WWW
 Bigger Bigger  Smaller Smaller  Reset Reset

So I am in the final stage of my Phi-1 shield revision, I'm looking at my first version, there are many things on the silk screen. The names are all printed on the board, along with texts I put on the board as directions. Since I can't find a way to reposition names other than moving the parts around, I resolved in adding texts and they overlap with the names.

My questions would be
Do you include part names on your PCB?
Do you use text tool to add descriptions to your board instead of using part names?
How do you not export those names to the Gerber file?
What would you rather do?

BTW, I'm confined by the EAGLE Lite license at $55 smiley I'd be able to lay larger boards, if I can make $1,000 in 10 years to purchase a full license. So till then everything is on tight quarter.

Here is a picture, the red is from part names and the blue is my addition.


* silk screen question.JPG (31.48 KB, 521x212 - viewed 389 times.)
Logged


0
Offline Offline
Faraday Member
**
Karma: 16
Posts: 2857
ruggedcircuits.com
View Profile
WWW
 Bigger Bigger  Smaller Smaller  Reset Reset

Quote
Do you include part names on your PCB?

Part references (e.g., R1, J2, etc.) yes, but not part names.

Quote
Do you use text tool to add descriptions to your board instead of using part names?

Yes, generally placed on tPlace or tNames layer (part references are on tNames).

Quote
How do you not export those names to the Gerber file?

In the CAM file select the tNames/tPlace layer but not the tValues layer (also not tDoc layer as that generally overlaps pads).

--
The Rugged Motor Driver: two H-bridges, more power than an L298, fully protected
Logged

Central MN, USA
Offline Offline
Tesla Member
***
Karma: 72
Posts: 7171
Phi_prompt, phi_interfaces, phi-2 shields, phi-panels
View Profile
WWW
 Bigger Bigger  Smaller Smaller  Reset Reset

RuggedCircuits,

Thanks a lot! I was comparing my boards made by three places. It seems BatchPCB doesn't have tNames or bNames selected in its CAM file. I sent in my brd file to the other two places and they must have both put the names layers in silk screen so both printed out all names, very busy. I'll email the persons in charge next time to not include Names layers in their silk screen.

BTW, I just checked on EAGLE, there are two things I can change, Name, and value. If you're using EAGLE, you would use both, right, like Name=R1, Value=2K.
Logged


0
Offline Offline
Faraday Member
**
Karma: 16
Posts: 2857
ruggedcircuits.com
View Profile
WWW
 Bigger Bigger  Smaller Smaller  Reset Reset

Quote
I'll email the persons in charge next time to not include Names layers in their silk screen.

It's tempting to just send BRD files to board houses but, as you've seen, you're never quite sure what you're going to get. I'd recommend putting a little time into some Eagle tutorials on using the CAM processor and generate your own Gerber files. Then you know exactly what you're getting!

Quote
BTW, I just checked on EAGLE, there are two things I can change, Name, and value. If you're using EAGLE, you would use both, right, like Name=R1, Value=2K.

Right. The Name shows up on the tNames layer (should be on the silkscreen) and the Value shows up on the tValues layer (should NOT be on the silkscreen....generally...it's always up to you).

Now that's if the part has been drawn properly. There are a lot of "hobbyist libraries" out there that do not follow this standard, so be warned.

--
The Aussie Shield: breakout all 28 pins to quick-connect terminals
Logged

nr Bundaberg, Australia
Offline Offline
Tesla Member
***
Karma: 126
Posts: 8472
Scattered showers my arse -- Noah, 2348BC.
View Profile
WWW
 Bigger Bigger  Smaller Smaller  Reset Reset

I would not normally put the component value or part name, just it's designator (R1 etc).

If there's room and a good reason then maybe the value of a resistor, cap or coil or a chip type (under the chip), that can make loading the board a bit easier.

______
Rob
Logged

Rob Gray aka the GRAYnomad www.robgray.com

Southern Ontario
Offline Offline
Sr. Member
****
Karma: 2
Posts: 279
Arduino rocks
View Profile
 Bigger Bigger  Smaller Smaller  Reset Reset

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'... smiley-wink
« Last Edit: February 09, 2011, 03:40:00 am by nickvd » Logged

SF Bay Area (USA)
Online Online
Tesla Member
***
Karma: 124
Posts: 6652
Strongly opinionated, but not official!
View Profile
 Bigger Bigger  Smaller Smaller  Reset Reset

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; http://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.)
Logged

Central MN, USA
Offline Offline
Tesla Member
***
Karma: 72
Posts: 7171
Phi_prompt, phi_interfaces, phi-2 shields, phi-panels
View Profile
WWW
 Bigger Bigger  Smaller Smaller  Reset Reset

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  smiley-wink
« Last Edit: February 07, 2011, 09:42:22 am by liudr » Logged


SF Bay Area (USA)
Online Online
Tesla Member
***
Karma: 124
Posts: 6652
Strongly opinionated, but not official!
View Profile
 Bigger Bigger  Smaller Smaller  Reset Reset

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.)
Logged

Central MN, USA
Offline Offline
Tesla Member
***
Karma: 72
Posts: 7171
Phi_prompt, phi_interfaces, phi-2 shields, phi-panels
View Profile
WWW
 Bigger Bigger  Smaller Smaller  Reset Reset

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.

Logged


0
Offline Offline
Faraday Member
**
Karma: 16
Posts: 2857
ruggedcircuits.com
View Profile
WWW
 Bigger Bigger  Smaller Smaller  Reset Reset

Quote
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?

Yes, I think so!

Quote
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.

It's perfectly fine to "change it anyways". It depends on how the part was drawn in the library.

Resistors do have a value. Just use the Value tool, click on the resistor, give it a value, and this should show up on the tValues layer on the PCB.

--
The Quick Shield: breakout all 28 pins to quick-connect terminals
Logged

SF Bay Area (USA)
Online Online
Tesla Member
***
Karma: 124
Posts: 6652
Strongly opinionated, but not official!
View Profile
 Bigger Bigger  Smaller Smaller  Reset Reset

There's a "value" checkbox in the "device" pane of the library editor.  Check the non-default value to cause the device to have a use-settable "value"
Logged

Pages: [1]   Go Up
Jump to: