Go Down

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

liudr

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 :) 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.

RuggedCircuits

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

liudr

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.

RuggedCircuits

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

Graynomad

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
Rob Gray aka the GRAYnomad www.robgray.com

Go Up