removing bits from tStop

Chris schrieb:

I am laying out a PCB that has a footprint for a module that is a PCB with

side-plated contacts.

 

Underneath the module there are a few vias and I am concerned they might

short with vias on the underside of the PCB module.

 

I thought that I coule edit tStop and remove the stop on the top layer, so

that the vias are completely covered on the top, but open on the bottom.

 

Firstly, is it safe to do this,

Definitely not.

Avoid the vias on your module and/or an the main board, or adjust the

module's position so that no vias or anything else can unintentionally

get in contact. This also applies to tracks etc. - don't ever trust on

solder stop mask to be an insulator.

and secondly, how do I edit the tStop layer.

When I view it, I just see hatched circles where the vias are, but I dont

seem to be able remove them.

They are automatically generated with the vias. However, vias have a

property by which you can turn this function off.

But: I strongly recommend to leave vias open unless it's absolutely

unavoidable to tent them - for reliability reasons.

Tilmann

Chris wrote on Sat, 15 May 2010 11:06

Firstly, is it safe to do this, and secondly, how do I edit the tStop

layer.

Yes, it's perfectly normal to cover vias with solder mask.  You do this in

Eagle in the DRC settings if I remember right (I set this so long ago I

don't remember the details).  Someplace there is a setting for a via size.

Vias below that size will be covered with solder mask.

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.

Olin Lathrop wrote:

Yes, it's perfectly normal to cover vias with solder mask.  You do this in

only for careless board houses. Serious manufacturers know the risks.

Oliver

Quote:

only for careless board houses. Serious manufacturers know the risks.

Take a look at most circuit boards, and you will see the vias covered with

soldermask.  Apparently someone here had a bad day possibly caused by dirt

trapped under the soldermask which then corroded the via.  Yes, I suppose

careless board houses can run into that, but that doesn't make the overall

concept wrong.

I once had a problem with a run of boards that failed months after getting

into the field.  This was eventually traced back to sloppy board

manufacture.  A connector was used with relatively fine pitch, 1.25mm if I

remember right.  The PCB material was not made correctly, so there were

small voids in it.  Chemical residue got stuck in the voids, which over

time either shorted out adjacent pins directly or caused metal atoms to

migrate which then caused shorts.  Some were only a few ohms between

adjacent pins.  A few boards failed by overheating when the power and

ground pins on the connector got shorted.

Anyway, the point is stuff goes wrong, but don't blame it on the wrong

thing or believe in mythological solutions.  What you're saying about the

solder mask is like saying I should never use a 1.25mm connector again

because one board house made bad PCBs that run.  Clearly that would be

silly.

I've also had manufacturing problems with QFN packages.  The manufacturer

did something to leave water soluable flux residue under the QFN package,

and a bunch of pins were essentially shorted together.  Your equivalent

solution would be to never use a QFN package again.

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.

Olin Lathrop wrote:

only for careless board houses. Serious manufacturers know the risks.

 

Take a look at most circuit boards, and you will see the vias covered with

soldermask.

the good ones are not covered with solder resist but plugged (a

separate processing), the bad ones are simply bad.

Apparently someone here had a bad day possibly caused by dirt

trapped under the soldermask which then corroded the via.  Yes, I suppose

Where should "dirt" come from?

If something is trapped in those vias then likely chemicals from the

board processing, uncured resist.

With open vias, the surface finish (HAL, immersion Tin etc.) also

coats and protects the via and drives away the residues of the

previous processing. Solder resist over the via hole prevents this so

you get bare Copper contaminated with some chemicals. And you don't

get reliably closed holes, so it could be that humidity enters the

via, forming some even more critical mixture.

careless board houses can run into that, but that doesn't make the overall

concept wrong.

 

I once had a problem with a run of boards that failed months after getting

into the field.  This was eventually traced back to sloppy board

manufacture.  A connector was used with relatively fine pitch, 1.25mm if I

remember right.  The PCB material was not made correctly, so there were

small voids in it.  Chemical residue got stuck in the voids, which over

time either shorted out adjacent pins directly or caused metal atoms to

migrate which then caused shorts.  Some were only a few ohms between

Maybe "conductive anodic filaments" (CAF) often happening with bad

laminate.

Anyway, the point is stuff goes wrong, but don't blame it on the wrong

thing or believe in mythological solutions.  What you're saying about the

solder mask is like saying I should never use a 1.25mm connector again

because one board house made bad PCBs that run.  Clearly that would be

silly.

It's silly to be reluctant to gather information about the problem and

insist on writing that solder resist covered vias are o.k.

Please do use solder resist covered vias in your products as you like,

but don't tell other people that it is correct to do so.

Oliver

Oliver Betz wrote on Fri, 21 May 2010 02:57

the good ones are not covered with solder resist but plugged (a

separate processing), the bad ones are simply bad.

I see, so this is a religious issue.  I don't think most of the world's PC

boards are bad.  It's time you dropped the attitude.

I've made boards with open vias too.  Most of the time it doesn't matter

and I don't.  If vias were always supposed to be open, there wouldn't be a

setting for it in Eagle.  Various different things need to be done for

various high-rel or unusual environments.  They all have their reasons for

those particular applications.

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.