| Author |
 Topic  |
|
|
JayDee
United Kingdom
16 Posts |
 Posted - 06 Jan 2026 : 12:26:21
|
Hi,
I have a custom interlaced finger pad, its drawn as a component and is a collection of connected 'open shapes' rather than a single pad.
The whole board will have all pads gold plated but how can I ensure that this whole component is not masked off ?
thanks, j. |
|
|
edrees
United Kingdom
806 Posts |
Posted - 06 Jan 2026 : 13:12:42
|
You could always add a top & Bottom Solder Resist layers to your Design Tech, (if they don't already exist) then add closed, filled shapes on both solder resist layers superimposed on your copper "finger pads".
Make sure you plot both the solder resist layers as well as the other layers! I'm assuming a double sided finger pad. |
 |
|
|
JayDee
United Kingdom
16 Posts |
Posted - 06 Jan 2026 : 14:11:20
|
Thanks, Great idea, I'll give that a go and see what the Gerber derived model looks like from the PCB supplier as it generally shows me what to expect.
Thanks, J. |
|
|
|
JayDee
United Kingdom
16 Posts |
Posted - 07 Jan 2026 : 11:13:00
|
My standard drawing does have a specific resist layer.
I ended up modifying the components PCB symbol in the library.
Once editing the PCB symbol, Added a shape.
Selectd nd Right clicked, selected replicate to layers, top resist.
This then gives me a resist shape.
To get it to export for manufacture, in print&plot I had to deselect the 'Pads-Only' option in the correct Resist Layer.
This does leave vias exposed but that should be OK for this project.
Have sent for manufacture and we shall see! J. |
|
|
|
edrees
United Kingdom
806 Posts |
Posted - 07 Jan 2026 : 14:14:08
|
Jay, it sounds to me as if you do NOT have a specific solder resist layer in Design Tech as the Plot dialogue is (probably) offering you a "TopCopper(resist)" option (as opposed to say a TopSolderResist layer?
Adding the solder resist shapes to your Component is another way of achieving the same thing, but with solder resist layer(s) enabled in your Design Tech you would be able to see the solder resist within the PCB Editor.
You could have unticked the "Normal Vias" within the "Pads Only" plotting option if you wanted the other vias to be "tented-over".
|
Edited by - edrees on 07 Jan 2026 14:19:53 |
|
|
| |
Topic |
|
No Solder Mask for component made of traces