Add Pads to inner layers

Making PCB Layouts, Manual routing, Auto-routing, Copper pouring, Updating from Schematic, Manufacturing Output
Post Reply
Posts: 30
Joined: 19 Oct 2014, 08:56

Add Pads to inner layers

#1 Post by mbelectronicdesign » 13 May 2020, 08:16

A client is asking for changes to my 10 layer design to allow back drilling to effect lower cost of manufacturing.

There are 4 x layer 1-3 vias and 4 x layer 3-10 vias. Because there are so few blind vias, the PCB manufacturer is proposing to cheapen the cost of production by making the blind vias as through vias initially and then back drilling out the layers where they don't want the via to be so the 1-3 vias would be made as a through vias and then drilled from the layer 10 side such that the drill gets close to layer 3 thus drilling out layers 10-4.

To help in this approach, they have asked that, for layer 1-3 vias, I add 0.5 mm diameter pads on layers 4,5,6,7,8,9,10 at the exact spot of the layer 1-3 via.

I created a pattern that's a 0.5 mm circular pad and then made it a component but that only appears on the top, even if I place it on an inner layer.

Is there a way to do this?

Posts: 1524
Joined: 20 Jun 2015, 14:39

Re: Add Pads to inner layers

#2 Post by Tomg » 13 May 2020, 12:18

Assuming you want a larger pad size on an inner layer than what exists on the Top/Bottom layer, give this workaround a try...
1) Set the Current Shape and Text Layer to "Signal/Plane" and choose one of the inner layers to be the working layer.
2) Select the "Filled Obround" shape in the Place Shape menu and draw the desired pad size over one of the vias.
3) Right-click on the newly-created pad (not the via's pad) and choose "Properties..." in the context menu to bring up the Shape Properties dialog window.
4) In the Shape Properties dialog window's Net: drop-list, select the same net to which the via is connected and click on OK.
5) Repeat as needed for other layers and vias.

Naturally, you can come up with variations of this workaround to suit your needs. For example if the inner layer pad sizes need to be smaller than the Top/Bottom layer pad size, use a via with the pad size that is required for the inner layers and add the larger pad shape to the Top/Bottom layer.

p.s. After re-reading your post it appears you don't need to worry about the electrical connection as the via does not exist in the other inner layers. Just draw the Filled Obround on the other layers without making the net connections. You might even consider drawing a donut-shape to aid in guiding the drill bit.

Hope this helps.

Post Reply