DipTrace Forum
http://www.diptrace.com/forum/

Supporting Solder pads /Unconnected Solder Pads missing mask
http://www.diptrace.com/forum/viewtopic.php?f=5&t=11610
Page 1 of 1

Author:  Whyrly [ 01 Jun 2017, 11:52 ]
Post subject:  Supporting Solder pads /Unconnected Solder Pads missing mask

Hello fellow 'diptracers',

I'm working with some JST connectors that have (2) connected pins and two solder pads for support only.

I didn't check my design well enough, but it seems that the two solder pads made it onto the copper layer, but the solder mask went right over it!

Do I need to have three layer objects in the Pattern?
one for the copper
One for the solder mask
one for the paste?

Seems it could all be done with by just using a pad, but if I number them, then they are 'unconnected'.
And since there are multiples, then I'd need to connect multiple numbers, and there is no related schematic 'pin' to connect them to!

How can I tell the part that this is a pad and it also needs a mask and paste?

I always thought using the top layer did this...

(The attached photo is me remaking it using pads as a test - the problem is with the pads numbered 3)


Thanks

Author:  Tomg [ 01 Jun 2017, 12:38 ]
Post subject:  Re: Supporting Solder pads /Unconnected Solder Pads missing

Pads automatically receive soldermask openings and solder paste, other copper does not. If you have a copper plane (not a pad) that you don't want covered by soldermask, cover it with a filled drawing object of the same size and shape* drawn on the Top Mask layer. The Pattern Editor's Top Mask layer will produce custom openings in the top soldermask. The soldermask cannot be seen in the PCB Layout editor, but it can be viewed using the 3D Preview tool or the Gerber export tool's Preview function. You will also have to draw a filled object of the desired shape and size** on the Pattern Editor's Top Paste layer to place custom solder paste on the copper plane. The custom solder paste (not the automatic solder paste) will appear in the PCB Layout editor's Design Area. Both solder paste types (custom and automatic) will show when using the Gerber export tool's Preview function, but neither will show in the 3D Preview tool.

*Note: The default setting for Solder Mask Swell is 0.1mm in the Gerber Export dialog window. This means that automatic soldermask openings are increased by 0.1mm on all sides. The manually placed Top Mask drawing in the Pattern Editor is not affected by the Solder Mask Swell setting, so you will have to similarly increase its size to minimize the chance of a component seating problem during reflow soldering.

**Note: The default setting for Paste Mask Shrink is 0.1mm in the Gerber Export dialog window. This means that automatic paste mask dimensions are decreased by 0.1mm on all sides. The manually placed Top Paste drawing in the Pattern Editor is not affected by the Paste Mask Shrink setting, so the size you create will be the final size.

Page 1 of 1 All times are UTC - 5 hours [ DST ]
Powered by phpBB © 2000, 2002, 2005, 2007 phpBB Group
http://www.phpbb.com/