How to change SMD Solder Mask Size on the Package Editor?

The DRC settings adjust the mask to pad clearance. But some(all) the

board houses have a registration problem with the mask and require the

mask to be larger then the pad. Even if you get a 2 mil sliver of mask

between the pins and not on the pads it does little good. Mask on Fr4 is

about the same as Fr4 when soldering. A little mask on the pad gives a

bad solder joint.

HTH

Paul R.

On 02/27/2013 08:46 PM, Luis Rodriguez wrote:

HI

I was wondering if there's a way to change the value of the solder mask expansion that is automatically added when creating SMD pins in the package editor... for high pitch devices (0.8mm or 0.5mm) the default value is too big and the solder mask overlaps resulting in no solder mask between the SMD pins... I know that I can disable the automatic creation of those objects and then manually adding them in the corresponding layer but this is a really time consuming task for high pin count devices like TQFP144 or BGA256...

 

Thanks in advance

 

--

To view any images and attachments in this post, visit:

http://www.element14.com/community/message/70940#70940/l/how-to-change-smd-solder-mask-size-on-the-package-editor

 

Sorry for being that annoying but... Can you elaborate a bit more?

I got my mask set to min:4mil %:100 max:4mil but and DRC just complains while checking at test footprint I created using this command "smd 0.3x1.2 -100"... I placed two pads with 0.5mm of distance from each other... both in the footprint editor and pcb layout I can see the solder mask overlaping each other and no way how to reduce the solder mask expansion... at least not automatically for this specific footprint (unless I add the solder mask manually)

So... I'm a bit lost

On 03/04/2013 05:57 PM, Luis Rodriguez wrote:

Sorry for being that annoying but... Can you elaborate a bit more?

I got my mask set to min:4mil %:100 max:4mil but and DRC just complains while checking at test footprint I created using this command "smd 0.3x1.2 -100"... I placed two pads with 0.5mm of distance from each other... both in the footprint editor and pcb layout I can see the solder mask overlaping each other and no way how to reduce the solder mask expansion... at least not automatically for this specific footprint (unless I add the solder mask manually)

 

So... I'm a bit lost

So mask width is 4mil +pad width + 4 mil.

If my math is correct

0.5mm = 19.6 mil

0.3mm = 11.8 mil

So 11.844 = 19.8 mil so they touch.

To get clearance set the stop to 2 mil and pay extra to get the mask not

to overlap the pad.

Also with a 0.3mm pad you only have 0.2mm clearance or 7.87mil.

Paul R.

Luis Rodriguez wrote:

Sorry for being that annoying but... Can you elaborate a bit more?

I got my mask set to min:4mil %:100 max:4mil but and DRC just

complains while checking at test footprint I created using this

command "smd 0.3x1.2 -100"... I placed two pads with 0.5mm of

distance from each other... both in the footprint editor and pcb

layout I can see the solder mask overlaping each other and no way how

to reduce the solder mask expansion... at least not automatically for

this specific footprint (unless I add the solder mask manually)

 

So... I'm a bit lost

 

Others have had this issue. Have a read of this it may help you.

https://forum.sparkfun.com/viewtopic.php?f=20&t=32027

You will need to decide if your board house can get solderstop between the

pins or if you will go with the trench idea and limit solder problems with a

cream stencil that limits the solder amount. They talk of a 25% reduction in

the log direction for the cream so that the molten solder has space to move

into without it desiring the next pad.

Either way I believe you will have to turn off stop and cream for the

package and specify them manually.

All the best

Warren

--

Viewed / responded via the newsgroup at

news.cadsoft.de

I took your advice and set the DRC rules for 0mils overlap of xStop on SMD pads.  Indeed, the package editor displays the correct overlap now as being directly in line with the extents of the pad.

However, when the component make it onto the PCB, the solder mask still extends far past the edge of the SMD pad ... as if it is still using the old DRC rules.

I tried reloading the library, closing EAGLE and reopening it.   Same problem persists.  BTW I am on version 6.4.0

Any other clues to solve this overlap customization problem on the board?