Altium designer: Top and Solder masks empty.

[JohnG300c]

top solder layer

Does anyone know why my solder masks are not displayed in AD6 although they are enabled in the "Board Layers and Colors" dialog? I.e. nothing is displayed on screen although the "Top Paste" and "Bottom Paste" tabs are displayed. Also, the paste gerbers display fine.

Also, i have some gold fingers on my board that should not be on the Top/Bottom solder masks. How do i get rid of them? I would assume that i could simply delete them from the TopPaste/Bottom Paste if i only could see these items in the PCB editor...

 

[House_Cat]

top solder top paste

AD doesn't have a special mask for gold fingers. Whatever you think you are seeing, it isn't for gold. You would have to use a mechanical layer to designate any gold finger work that you want to have done - the software doesn't automatically do that.

AD does automatically make a solder mask opening for all pads, unless you have told it to "tent" the pad. So any top or bottom layer surface pad will have a mask opening, as well as all thru-hole pads. You cannot edit the automatically placed mask openings directly - you have to double click on the pad to bring up its properties. There is a portion of the pad properties dialog that lets you control the mask size.

There is a peculiarity in the AD display that requires you to have the surface layers turned on in order to see the mask layers in single layer mode. This has been true for many years in Protel/Altium PCB Editors because the layers are not separately editable - you can add openings to the mask layers manually, but you can't delete the automatically generated openings produced by the primitives on the surface layers. Turn off all layers except top, bottom, top solder, and bottom solder. Now select the tab for the mask layer you want to view, and use "shift S" to cycle through the single layer display. You will see the mask layer displayed in whatever color you have set.

 

[JohnG300c]

paste mask expansion

Thanks House Cat. I will try to "tent" the connector pads to see if they disappear from the solder paste mask.

 

[House_Cat]

golden finger connector altium

NO - YOU DON'T TENT TO REMOVE THE PASTE MASK. Tenting is to remove the SOLDER MASK OPENING.

To remove the paste mask opening, simply double click on the pad that you are interested in (or use Find Similar Objects for multiple pads), then in the "Paste Mask Expansion" area of the dialog you enter a negative value equal to the pad diameter. You can also specify that the paste mask be controlled by a design rule, assign the pads to a pad class, and then write a rule with the proper negative value for the pad class. Negative expansion does just what you might expect - it covers instead of uncovers the mask opening.

 

[JohnG300c]

altium paste remove

Thanks for the warning and clarification House Cat. I have now gotten rid of the paste mask openings over the gold fingers.