SMD Silkscreen

[tszaboo]

I would like to get your input on SMD silkscreen. People are using several different method to make the silkscreen for their SMD parts. I'm interested which on you are using and why. Please dont comment "because Eagle default", I'm interested in actual choices.
Some draw a rectangle around the component. I've noticed that a lot of computer equipment does this. Probably it allows better alignment.
Some draw two lines between the pads. This is what I was doing so far, now I have a choice.
Some draw "brackets" around the component.
Some, even agilent sometimes just cannot be bothered to put silkscreen for a resistor.

How do you do it, why?

[Kjelt]

If I had a choice I would choose no silkscreen for tiny components like resistors and capacitors.
Why? Because I think it looks messy esp with tiny components and the silkscreen quality is not always equal between pcb manufacturers.
PS: I would never use it between the pads or under the component since it then has a requirement that the silkscreen thickness has to be lower than the copper thickness, can you guarantee that?

[dmills]

The box variant (PADS PCB default) is a pain both because it hugely lowers the possible placement density and because it can end up confusing the AOI machines. I might, **MIGHT** do it on something very low density where hand assembly was likely, but that is a rare thing these days.

For jellybean non polar R/C/L I usually don't bother with outline silk (Designators are a different issue), larger parts get something, anything polar gets something, and any form of QFN/BGA gets both a full outline and a couple of fids. 

Another question, maximum, nominal or least material footprints for your default stock library? This is a sweary one whatever you decide to do.

Regards, Dan.

[wraper]

I use narrow line in the middle of the part. Gives the least problems if the silkscreen alignment is not good. Also, if component placement is tight enough, rectangle around the part likely will case no space for component designator to be placed without overlapping.

[diyaudio]

If I had a choice I would choose no silkscreen for tiny components like resistors and capacitors.
Why? Because I think it looks messy esp with tiny components and the silkscreen quality is not always equal between pcb manufacturers.
PS: I would never use it between the pads or under the component since it then has a requirement that the silkscreen thickness has to be lower than the copper thickness, can you guarantee that?

I forcefully discovered this, for referencing I enabled the silk for printing.

[m98]

I just switched to no silkscreen at all for such components. It looks ugly and takes up precious space. For hand placing of parts you often anyway need to make a placement plan and a PNP machine doesn't care either.

[jitter]

If I had a choice I would choose no silkscreen for tiny components like resistors and capacitors.
Why? Because I think it looks messy esp with tiny components and the silkscreen quality is not always equal between pcb manufacturers.

From the point of view of someone who has to trace and repair defects, having a good silkscreen is a real timesaver.
But if the stuff becomes too small, than putting it there is no use. So bother only with big enough components and do it well.

PS: I would never use it between the pads or under the component since it then has a requirement that the silkscreen thickness has to be lower than the copper thickness, can you guarantee that?

Since there wil be solder paste applied to the pads before the component is placed, the thickness of the silkscreen isn't really going to be an issue. I have never even remotely suspected problems were caused by silkscreen between pads.

[nctnico]

I have seperate silkscreen shapes for capacitors, resistors and inductors. It makes it very easy to do a visual inspection of a board to see if none of the passives got mixed up. Yes that does happen and some assemblers place components by hand if it is a small production run so it helps the people to keep track of what they are doing. Note that in the example below the smallest components are 0402 so the component reference text isn't in the actual silkscreen.

[T3sl4co1l]

Can't really see it from this height, but I use the lines-between-pads style.

If the pad gap is too small for two lengthwise lines, a single crosswise line goes between the pads.

I use Mechanical 1 for center mark, Mechanical 13 for 3D body (with an optional outline), and Mechanical 15 for courtyard / outline.

Oh, pads are rounded rectangles, too.  It looks better against soldermask and polygon pours.  And probably gives better paste release, give or take if the CM modifies the masks I suppose.

Tim

[tszaboo]

PS: I would never use it between the pads or under the component since it then has a requirement that the silkscreen thickness has to be lower than the copper thickness, can you guarantee that?

I never had problem with it. At least I never had more than more than a few PPM soldering issue to track it to be the problem. SMDs have wraparound terminals, so they are elevated from the board.

Another question, maximum, nominal or least material footprints for your default stock library? This is a sweary one whatever you decide to do.

I use medium density as my default. And I never had to go lower than 0603. Reliability and serviceability was more important than size. This might change in my new job, we will see.

I just switched to no silkscreen at all for such components. It looks ugly and takes up precious space. For hand placing of parts you often anyway need to make a placement plan and a PNP machine doesn't care either.

I usually place silk and designator, even for the smaller components. To be honest I less and less see the reason for the designator. Unless of course I need to debug something. For a 0603, the designator is bigger than the part itself. It is not a big issue for a 4 layer board, but for 6 layers it was already tedious. I noticed that lots of time I just draw a rectangle around a nicely layed out section, with short traces and everything, then the silkscreen is placed on the "between blocks" section of the PCB.

I have seperate silkscreen shapes for capacitors, resistors and inductors. It makes it very easy to do a visual inspection of a board to see if none of the passives got mixed up. Yes that does happen and some assemblers place components by hand if it is a small production run so it helps the people to keep track of what they are doing. Note that in the example below the smallest components are 0402 so the component reference text isn't in the actual silkscreen.

That is kinda like what Rigol does. I even saw 90 degrees rotated components, when the silk wasnt obvious.

I use Mechanical 1 for center mark, Mechanical 13 for 3D body (with an optional outline), and Mechanical 15 for courtyard / outline.

IMHO Mechanical 1 is always board outline, 13 is 3D, 15 is "IPC land" with courtyard of the component and a cross on the component center.
Since I always place small parts, so the courtyard doesnt overlap (ie 1.5mm pad center for 0603) the courtyard might even be on the silk.

[Kjelt]

.

[viji_rookie]

I just switched to no silkscreen at all for such components. It looks ugly and takes up precious space. For hand placing of parts you often anyway need to make a placement plan and a PNP machine doesn't care either.

Agree here. Try to follow exactly same as body size of a package. But if For such smaller package like discrete no witty designer will loose valuable space for an non conductive layer.