Wrong default soldermask clearance in footprint editor

AFAIK, the footprint editor shouldn't select any default solder mask
value other than 0 when creating new footprints or pads. KiCad uses
three separate solder mask settings to determine which mask value to use
when plotting with the following order of precedence: pad, footprint,
then board. This way you can use the board wide setting for all pads
and footprints that have a 0 solder mask value rather than define the
solder mask clearance for every single pad and/or footprint.

On 1/4/2017 9:15 AM, Art wrote:
> Public bug reported:
>
> Footprint editor selects an arbitrary default value as a pad solder mask
> clearance (0.2mm) regardless of the value selected in PCBnew. At the
> very least suggest setting this value to the industry standard min value
> for solder mask clearance of 3 mil (0.0762mm). Preferably it should be
> user adjustable.
>
> ** Affects: kicad
> Importance: Undecided
> Status: New
>

If the value is set to zero in the footprint editor, it uses this...

#define DEFAULT_SOLDERMASK_CLEARANCE Millimeter2iu( 0.2 )

from class_board_design_settings.cpp

I just tested this with the dev branch. I created a new footprint and
the footprint solder mask clearance was 0 and I added a pad to the
footprint and the pad solder mask clearance was 0. I saved the
footprint to a file in which neither the footprint or pad solder mask
clearance values were set. When I create a new board, the default
solder mask clearance is set to DEFAULT_SOLDERMASK_CLEARANCE which is
expected. I think the wording of the this bug report is what is
throwing me off. I can change the default board solder mask clearance
to 3 or 4 mils which is would make it a wishlist bug report as the
current behavior is expected. Also, would the bug reporter please
include a copy of the version string information so I know which
version(s) this effects.

On 1/4/2017 4:00 PM, Chris Gibson wrote:
> If the value is set to zero in the footprint editor, it uses this...
>
> #define DEFAULT_SOLDERMASK_CLEARANCE Millimeter2iu( 0.2 )
>
> from class_board_design_settings.cpp
>

I am (and I assume Art is) talking about what is actually displayed on the screen in the footprint editor.

In the footprint editor, if the pad solder mask clearance is set to (say) 0.3mm, it displays the pad with a 0.3mm bigger solder mask. Same goes for any other value. Which is what would be expected. But if the clearance is set to 0, it displays this value of 0.2mm from DEFAULT_SOLDERMASK_CLEARANCE

If it is set to zero by the user, by my way of thinking, it should display it as zero.

I could accept it picking up a value from a setting somewhere else in the user's preferences, but not some arbitrary default value.

What Cris said. It doesn't affect final plotting of the boards. It affects how footprints with solder mask clearance set to 0 are displayed. It is just annoying for fine pitch components because it obstructs the view and is somewhat misleading.

This only occurs in the GAL canvas not the legacy canvas. That's why I
wasn't seeing the problem. In the future please specify which canvas
you are using when filing bug reports. I agree that if both the
footprint and pad mask clearance are 0, there should be no mask
clearance displayed.

On 1/5/2017 9:09 AM, Art wrote:
> What Cris said. It doesn't affect final plotting of the boards. It
> affects how footprints with solder mask clearance set to 0 are
> displayed. It is just annoying for fine pitch components because it
> obstructs the view and is somewhat misleading.
>

It happens is legacy canvas too. I'm watching it do it right now.

I agree that this is annoying. What's the point in having a default global mask clearance for modedit? Pads and footprints with zero clearance inherit from the parent, why can't it just inherit zero? It'd be less misleading and make for a cleaner display for fine-pitched parts, as mentioned.

Fixed in revision 56fbfeeb4aef021410c25d6215ed27c92f9e7a3c
https://git.launchpad.net/kicad/patch/?id=56fbfeeb4aef021410c25d6215ed27c92f9e7a3c

I fixed this problem. Editing a footprint loaded from a board is a slightly different situation. One could argue that the solder mask clearance in footprint editor should be set to the clearance used in board currently being edited so the solder mask will be displayed as it will appear on the board. I took a quick look at doing this but there are so many footprint load paths in the footprint editor that I didn't feel motivated enough to track them all down to set the solder mask clearance accordingly. If someone files a new bug report about that, I'll take a another look at it.