How to prevent pads in inner layers

[Dago]

How can I disable/change pads in inner layers with EAGLE?

I have an extremely dense multi-pin circular connector (0.7mm pitch and 0.5mm+-0.1mm holes) that is impossible to route unless I leave off pads in the inner layers. I tried putting cutouts (there are no restrict layers for inner layers in eagle afaik) on the pads but the pads are still in the gerbers. I don't have a gerber editor available. How do I remove the pads from some of the inner layers?

[MarkL]

I don't see a way to remove individual inner pads.  The "Restring" section of the design rules can control the size of the inner pads, including 0 for no pad, but it only does it for all of them.

The pads are created with a single round flashed aperture, so they're easy to delete with an editor, as you suggest.  Even a simple editor, such as gerbv on linux, can do this.  But of course you'd have to re-edit the gerbers every time you ran the cam processor.

I think I would do this by creating a part with all the layers manually defined.  Any pin that shouldn't have an inner pad on one or more layers I would build using a drill and then place circles on the layers that should have pads.  Likely the DRC won't like this, so be prepared to override the errors for this part.  You would then also need to manually route to the pins after placing the part on the board.  Or, if you have the space, you can create the part with through-hole or SMD pads away from the pins that would serve as connection points (and make the part work normally in the schematic editor).

I would also check with your PCB fab house to make sure they don't have an issue with copper missing on the inner layers when they plate the holes.

[nitro2k01]

Just an idea: Try cloning the component/building it from scratch and then for the pad, open the properties and set the diameter to right above the drill size. Then manually place  round copper poly on the top and bottom layers, and maybe preferably a smaller round poly in the vias layer, to be sure, in case the drill is slightly off. I think this will produce what you want in the resulting gerbers.

[MarkL]

This could work, but be aware the final diameters of the outer and inner pads are influenced by the "Restring" settings in the design rules.  So, even if you set the all the exact diameters you want, they could get overridden.

You could then fiddle with the "Restring" settings to get the desired result for the one part, but since those are global settings, any changes there could have unexpected consequences in other areas of the board.  I would be cautious doing it this way.

Also, looking back at the OP's dimensions of 0.7mm pitch with 0.5mm +/-0.1mm holes, is that the footprint on the board or the mating area of the connector?  If on the board, that's awfully close drilling without breakout between the holes (worst case 0.1mm rib between holes - is that even possible?).

[Dago]

Also, looking back at the OP's dimensions of 0.7mm pitch with 0.5mm +/-0.1mm holes, is that the footprint on the board or the mating area of the connector?  If on the board, that's awfully close drilling without breakout between the holes (worst case 0.1mm rib between holes - is that even possible?).

https://www.hirose.co.jp/cataloge_hp/e12506002.pdf Look for the 20 pin PCB version. Yep it's pretty damn dense... It otherwise works out according to our factory specs (with 0.4mm holes) except the clearance between holes and the tracks in the inner layer is violated (factory spec says 6mil which is impossible to fulfill with 0.4mm holes).

I'm currently waiting for the connectors so I can measure the actual pins and see if I can downsize the hole sizes even more (damn datasheet doesn't mention the actual pin size!) and get it all under spec. If not I'll prolly order them anyway and test each board.

Btw. for designing the actual board with eagle I had to use gerbv for deleting the pads in the inner layers so I could route out the innermost pads.