KiCAD has alot of default footprints which place silkscreen over parts of the soldermask, especially with some small footprints. When producing these board with BatchPCB will the silkscreen be printed on areas covered by the soldermask, or must the footprints/silkscreens be modified to remove the silkscreen if its undesirable to have it printed on top of pads?
manderson:
KiCAD has alot of default footprints which place silkscreen over parts of the soldermask, especially with some small footprints. When producing these board with BatchPCB will the silkscreen be printed on areas covered by the soldermask, or must the footprints/silkscreens be modified to remove the silkscreen if its undesirable to have it printed on top of pads?
BatchPCB (actually GP) will fabricate whatever you
submit (within reason). Use a Gerber viewer to
examine the plot flies before you submit them.
BatchPCB (GP) will photo-subtract text from exposed
metal (pads and vias) to improve solderability.
In a PTH (Plated Through Hole) process the solder mask
is used for selective plating of the copper. Scratching
the solder mask on a completed PCB will reveal
unplated copper. It is not wise to delete the solder
mask except in desired exposed metal areas
(pads and vias).
Silk sreen printing is much easier to read when over
solder mask.
I slightly misstated my question - in areas where silkscreen is present over areas which would be exposed by the solder mask, would the silkscreen be printed on top of the exposed copper. Its common in KiCAD footprints that an outline in silkscreen is drawn around the package, covering parts of the pads.
Your response answers my question, BatchPCB / GP will not print sillkscreen on top of exposed pads. Thanks!
bigglez:
In a PTH (Plated Through Hole) process the solder maskis used for selective plating of the copper. Scratching
the solder mask on a completed PCB will reveal
unplated copper. It is not wise to delete the solder
mask except in desired exposed metal areas
(pads and vias).
Does this mean the soldermask has to be removed for vias to be plated through? I’m used to covering vias with soldermask - bad idea?
While I’m at it, what’s the best soldermask clearance to use?
Does this mean the soldermask has to be removed for vias to be plated through? I’m used to covering vias with soldermask - bad idea?
While I’m at it, what’s the best soldermask clearance to use?
Boards are plated well before the soldermask is added. I think the steps they use in making a double sided PCB are as follows:
-
Use board with 1/2 ounce copper
-
Drill the holes
-
Plate the boards to 1 ounce copper, which also plates the holes
-
Apply and expose / develop photoresist on top and bottom layers
-
Etch the PCBs and then remove photoresist
-
Apply soldermask (top & bottom) ie, silkscreen
-
Apply component overlay (silkscreen)
I almost always “tent” vias (ie, cover them with soldermask), except when I want to use them as test points. As for soldermask clearances, I normally use 2 thou, but that is on the low side. Normally this is OK though, since the soldermask accuracy seems a lot better than the silk layer…
MichaelN:
Boards are plated well before the soldermask is added. I almost always “tent” vias (ie, cover them with soldermask), except when I want to use them as test points.
Yes, but from the above it seems that the soldermask is being used to decide where to plate, hence the question. Have you had tented vias come back from BatchPCB plated through? That would answer my question.
As for soldermask clearances, I normally use 2 thou, but that is on the low side. Normally this is OK though, since the soldermask accuracy seems a lot better than the silk layer…
Oh good. I have a QFN-20 package on my board - they only have 9 mil space between pads, so 2 mil is just about the largest padding I can afford!
Cheers
Yes, but from the above it seems that the soldermask is being used to decide where to plate, hence the question. Have you had tented vias come back from BatchPCB plated through? That would answer my question.
The soldermask defines where the FINAL finish plating (solder / tin / silver / gold) is applied, not the copper plating that plates the holes. I have used Gold Phoenix (the people who make the BatchPCB boards) a bunch of times and never had a problem.
As I said, I normally “tent” the vias, to prevent accidental shorts when the boards are soldered. I normally pack the components as tight as possible - it’s kind of an obsession for me…
My latest boards had a bunch of QFNs, and I was very happy with how easily they soldered (I used solderpaste with a stencil from Ryan Ohara). Due to the package geometry, you’re actually less likely to get solder bridges than with something like QFP packages.
MichaelN:
The soldermask defines where the FINAL finish plating (solder / tin / silver / gold) is applied, not the copper plating that plates the holes. I have used Gold Phoenix (the people who make the BatchPCB boards) a bunch of times and never had a problem.
Great, thanks Michael for clearing that up!
I normally pack the components as tight as possible - it’s kind of an obsession for me…
Hahah, same here! My current board is only the size of a DIP-16 :shock: and I stayed up all night squeezing everything in. My definition of a beautiful layout is when it couldn’t possibly be any smaller without failing DRC… 
My latest boards had a bunch of QFNs, and I was very happy with how easily they soldered (I used solderpaste with a stencil from Ryan Ohara). Due to the package geometry, you’re actually less likely to get solder bridges than with something like QFP packages.
That’s very good to hear, I was worried about that. Have you done any QFNs with thermal pad? Not sure how that works - the thermal pad by design has a large amount of copper attached (4 vias directly into the ground plane), so it will sink a lot of heat… won’t the other pads (which are tiny) overheat by the time that solder flows? Is there some trick to it?
Cheers
Have you done any QFNs with thermal pad? Not sure how that works - the thermal pad by design has a large amount of copper attached (4 vias directly into the ground plane), so it will sink a lot of heat… won’t the other pads (which are tiny) overheat by the time that solder flows? Is there some trick to it?
What soldering method are you using? I use either a reflow oven that is made for the task, or an electric frypan (skillet). Both methods heat the entire board, so there should be no issue melting the solderpaste on the thermal pad as long as the heating profile is OK.
One issue you can have is the vias in the center pad “stealing” solder (ie, the molten solder gets wicked down the vias instead of bonding the thermal pad to the PCB). I’ve found that this isn’t really an issue if you “tent” these vias on the other side of the board, since the soldermask resin somewhat fills the vias and prevents too much solder from traveling down them.
If you’re soldering by hand, then good luck. Leon Heller reports success using his Metcal soldering iron (which can pump a LOT of heat into the solder joint when needed). I think he said he used one big via to apply the heat and fine gauge solder.
MichaelN:
What soldering method are you using? I use either a reflow oven that is made for the task, or an electric frypan (skillet).
To date, steady hand & magnifying glass :shock:
Skillet method sounds great, will have to look into it. Wouldn’t have thought that one can heat up the entire board like that without cooking components. Thanks!
One issue you can have is the vias in the center pad “stealing” solder (ie, the molten solder gets wicked down the vias instead of bonding the thermal pad to the PCB). I’ve found that this isn’t really an issue if you “tent” these vias on the other side of the board, since the soldermask resin somewhat fills the vias and prevents too much solder from traveling down them.
My vias in thermal pad are small (20 mil) and tented, so it should be fine. Again, thanks!
If you haven’t already, check out Sparkfun’s tutorials on this:
http://www.sparkfun.com/commerce/tutori … ials_id=58
http://www.sparkfun.com/commerce/tutori … ials_id=59
http://www.sparkfun.com/commerce/tutori … ials_id=60
If you don’t want the expense and delay of a stencil, you can apply solder paste with a syringe & fat needle. Check out the previous thread on this:
As I suggested in the thread, I’ve used this this solder paste (shipped from Hong Kong), and it works well (and cheap - only $3.57 inc shipping):
MichaelN:
Does this mean the soldermask has to be removed for vias to be plated through? I’m used to covering vias with soldermask - bad idea?
While I’m at it, what’s the best soldermask clearance to use?
Boards are plated well before the soldermask is added. I think the steps they use in making a double sided PCB are as follows:
Use board with 1/2 ounce copper
Drill the holes
Plate the boards to 1 ounce copper, which also plates the holes
Apply and expose / develop photoresist on top and bottom layers
Etch the PCBs and then remove photoresist
Apply soldermask (top & bottom) ie, silkscreen
Apply component overlay (silkscreen)
I almost always “tent” vias (ie, cover them with soldermask), except when I want to use them as test points. As for soldermask clearances, I normally use 2 thou, but that is on the low side. Normally this is OK though, since the soldermask accuracy seems a lot better than the silk layer…
I think they say they plate the board after solder mask is applied. This plates only the exposed pads/holes.