Silkscreen Over Pads

Go To Last Post
13 posts / 0 new
Author
Message
#1
  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Howdy all,

I'm creating a PCB design in Cadsoft EAGLE for eventual fabrication (probably via Sparkfun's BatchPCB service). Since this will be the first PCB I've ever had fabbed by a board house, I wanted to get the sage advice of the gurus here and avoid a potential issue.

The Sparkfun website's tutorial series has this admonishment under their Common Mistakes, Tips and Tricks section:

Quote:
Don't run silkscreen across pads.
As you can see in the image below, I've got "silkscreen over pads" in a few cases (and even a few more not shown). For example, the "1" in the 10-pin header overlays the MCU's pad.

A search turns up this thread: Eagle Silkscreen vs Stop Mask...

Jim Wagner's advice to "smash" the part (in the PCB editor) sounded like just the trick I needed. Unfortunately, I found that when I smash the 10-pin header, only the 'name' text field ("ROT-SW") is movable. The "1" text and the "10" text remain locked to the part outline.

But I really don't care if the silkscreen that overlays the pads gets deleted by the fab house and is not printed. I just don't know how serious this case is and I wouldn't want the board to get rejected.

In fact, the MCU part, which came from the 'atmel.lbr' library, is designed with the chip outline (which I presume many people would include in the silkscreen layer) right over the top of all the pads!

So I suspect this would not be a problem if I just leave everything as shown in the image above. But it never hurts to ask. All advice and comments appreciated!

Regards,
Bill

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

A decent Gerber editor will clip silkscreen.

All part of CAM-ing/ Engineering at a decent PCB shop.

Just tell the PCB shop to not do any DFM checks and make as is.

They will take Your money.

Silkscreen over solder pads is bad for You not the PCB shop. Silkscreen may result in an inferior solder joint.

That is all.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

You could try and see what happens.
the fabs I have worked with in the past all did a cross check on the gerbers and removed or moved silkscreen that we forgot to edit, so it might be that they clip the 1 or move it to another position

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

As an aside, I normally mark pin 1 with a square or rectangular pad. That way you get rid of the pesky '1'.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Thanks for all the info, folks!

I can certainly move the parts to avoid conflict, but that (needlessly?) raises the PCB build cost.

Kartman wrote:
As an aside, I normally mark pin 1 with a square or rectangular pad.
A useful option, indeed. I'm actually surprised how many parts in EAGLE libraries come without that. Along those lines, after a bit of searching, I found a 2x5 pin header part in the Sparkfun EAGLE part library that marks pin 1 with a simple, adjacent "bar" in the silk layer. I somehow missed that when designing this PCB. The 2x5 part in the image comes from 'con-lstb.lbr' (which came with EAGLE, IIRC) but I'm not wedded to it.

I guess I could also learn part editing in EAGLE. I was planning on doing that eventually, just not quite yet! :smile:

ignoramus wrote:
Silkscreen may result in an inferior solder joint.
I think this answers my real concern. Given that, I will probably take the time to fix this properly. No sense starting my PCB creations on the wrong foot. :smile:
ignoramus wrote:
A decent Gerber editor will clip silkscreen.
I've been using the Gerber viewer 'gerbv', but it's just a (fine, IMHO) viewer, not an editor. Any recommendations for a good Gerber editor that runs under GNU/Linux?

Thanks again for the insight, everyone. I really appreciate it!

Regards,
Bill

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

The more PCBs I design and get fabbed the less and less I actually use silkscreen for anything other than logos and product names, I think it looks messy and unprofessional on a production board. Generally users don't need to know if a capacitor is C24 or if it is 0.1uF.
For this reason I always have seperate tSilk and bSilk layers so I can have full control over the silkscreen. You can use the standard tPlace/tNames/tValues but in the majority of cases this can get very messy and there may be some overlaps. The one downside of using seperate custom silkscreen layers is they will not move if you move parts, but the simple solution to this is to make adding the silkscreen the very last thing you do before sending off your gerbers.

As for silkscreen over pads, I have used more than a dozen different PCB fabs over the past 6 years and every single one has always clipped the silkscreen off the pads for me. Some fabs mention that they do, others just do it.
Don't bother editing gerbers, that's the wrong solution. You should be fixing the problem in the actual design files in EAGLE, so that you don't have to do any post processing every time you want to generate come gerbers. Especially if you are sharing your designs to the open source community.

TL;DR: Use custom silkscreen layers for maximum control. Most fabs will clip the silkscreen, ask them if they don't mention it.

Last Edited: Thu. Oct 13, 2011 - 04:17 PM
  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

I wouldn't worry about silkscreen on the top pad of a thru-hole part, since you'll be soldering on the bottom pad. SMT devices would be an obvious problem, however.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Just make sure the fab is not Olimex, as they DON'T clip the silkscreed.

If it is for personal use, I'd also say don't bother, unless there is too much silkscreen on the pads and it messes up your soldering process.

-Pantelis

Professor of Applied Murphology, University of W.T.F.Justhappened.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

I decided to just "bite the bullet" and learn how to edit parts in EAGLE and now I'm glad I did. I fumbled around for a short bit, but that was a 1-time learning curve. The actual changes were quite easy (albeit not always intuitively accomplished).

I created a custom version of that 2x5 header from the 'con-lstb.lbr' by moving the "1" to avoid the MCU pad and changing pin #1's pad from round to square (sort of a "belt and suspenders" philosophy). Here's the new look:

This PCB is just for personal use, but in the future, I'll still undoubtedly be more like Gussy and drop some of the silkscreen, especially as I modify parts to use the "square pin 1" method.

Thanks again for all the advice, oh wise Freaks! I have learned several new things and I'm no longer hesitant to edit (or create) parts for EAGLE libraries.

Regards,
Bill

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Keep in mind that when you've soldered a header on a board you can't see the square pad from the top, so you'll want to keep some form of pin-1 silkscreen indication.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

meteor wrote:
I decided to just "bite the bullet" and learn how to edit parts in EAGLE and now I'm glad I did. I fumbled around for a short bit, but that was a 1-time learning curve. The actual changes were quite easy (albeit not always intuitively accomplished).

It's a good skill worth learning :)

For future reference though, when you want to move text you don't need to edit the part, you can just use the "smash" command on the part and it will separate the Name and Value into separate items from the main part.
From there you can edit their size, ratio, move them around or even delete them if you wish. Hope this helps!

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Good point, kk6gm. Thanks for the reminder!

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

gussy wrote:
For future reference though, when you want to move text you don't need to edit the part, you can just use the "smash" command on the part and it will separate the Name and Value into separate items from the main part.
That's all true, but in this case, the "1" and the "10" are not part of the "Name" or "Value" fields and a "smash" on the part doesn't unlock them, unfortunately. I'm just glad it was so easy to actually edit the part. Thanks for the extra advice, even though Jim Wagner beat you to it in the aforementioned thread from my 1st post. :wink:

Regards,
Bill