DipTrace Forum

Cover a pad with 'Metal Mask'
Page 1 of 1

Author:  KevinA [ 01 Oct 2017, 11:13 ]
Post subject:  Cover a pad with 'Metal Mask'

I'm looking at part http://www.molex.com/pdm_docs/sd/1042490810_sd.pdf to interconnect with but I believe they want more than half the pad covered with solder mask. They call it 'Metal Mask', they call connector support 'Fitting Nail'. I did the math to create the pattern then placed it on a PCB and tried to draw an area over the pads on the Solder Mask Layer:
The Molex connector:

The DipTrace Pattern

My attempt to place a mask over the pads:

The results as Gerber:

Any suggestions?

Author:  Tomg [ 01 Oct 2017, 11:44 ]
Post subject:  Re: Cover a pad with 'Metal Mask'

Disable the Top Solder Mask for each pad and create your own "blanket" masks to expose the top/bottom edges of the two pad rows. To view the results in 3D Preview, you'll need a Board Outline present. See the attached file named "modified.dip" for an example...

Author:  KevinA [ 01 Oct 2017, 12:39 ]
Post subject:  Re: Cover a pad with 'Metal Mask'

Sweet! I have to think of the 'Mask' I place as an area where the 'Mask' will not be or an anti-mask.... I can deal with that, gets the job done without more bloat. As far as I can see I'll have to use this pattern from the PCB file (copy paste and change the RefDef to match the schematic) or edit the pattern every time I use it? I can't see any means to add the mask to the pattern.

To get the mask between the pads I place 8 .6X.45 in place to the two rectangles:

Author:  Tomg [ 01 Oct 2017, 13:10 ]
Post subject:  Re: Cover a pad with 'Metal Mask'

1) Open the Pattern Editor, insert a copy of the original pattern into one of your custom pattern libraries, rename the "new" pattern to suit your needs, apply the same mask treatment and resave the custom pattern library.
2) Open the Component Editor, insert a copy of the original component into one of your custom component libraries, rename the "new" component, attach the new custom pattern to it and resave the custom component library.
Now the new component with its new pattern is ready for use. Just replace the original component in the schematic with the new one, resave and then renew the PCB.

You can also store the modified pattern from the PCB...
1) Right-click on the component (not its pads), select Ungroup Component, select/highlight all of the original component's objects plus the new masks, right-click on the outline of one of the selected objects (not a pad) and choose Group into Component.
2) Assign the desired RefDes prefix and enter a new name for the newly-modified component.
3) Over on the left side of the screen select the appropriate target custom pattern Library, then right-click on the newly-modified component (not its pads) and choose Save to Library > Save to file... > etc. You will see the name of the newly-modified component appear at the bottom of the target library's patterns list.

Page 1 of 1 All times are UTC - 5 hours [ DST ]
Powered by phpBB © 2000, 2002, 2005, 2007 phpBB Group