How to open up space inside a ground plane in Fusion Electronics

[CaptainMJ]

Hi All,

Almost done with my first PCB card in Fusion Electronics, just need to open up space for a couple of connections inside my ground plane. I'm sure this is easy but i just can't seem to find the way to do it. Can someone here help me out with how to do it?

Many thanks,

Marcus

[Spragnut]

Draw a polygon shape and make sure it's drawn on the tRestrict or bRestrict layers, depending on if you want it on the top or bottom, then re-pour your fill and that area should remain clear of copper.

Or if your wanting to do an opening in the actual PCB itself do the same but draw the polygon on the dimension layer.

Hopefully that helps.

[edwin.robledo]

Hi Marcus,

Greatly appreciate your participation on the Fusion 360 forum. To define cutout areas within a polygon you can draw another polygon and change the property called pour to cut out. This will generate a void within the polygon in the same layer.

[Spragnut]

@edwin.robledo 

Purely out of interest is there any advantage of using this method as opposed to the restrict layers?

I've only completed one design in Fusion/Eagle so far and would like to pick up best practices as early as possible.

Cheers

James

[CaptainMJ]

@Spragnut I did play around a bit with that, but I'm not sure that's quite the thing I needed. What i wanted to achieve was something similar to the attached where I can open up to pull another wire connection through the plane. Is there another way to accomplish this?

Many thanks for your help here,

Marcus

[CaptainMJ]

Hi @edwin.robledo ,

Many thanks, I will try this technique as well!

Best regards,

Marcus

[Spragnut · Accepted solution]

I think what your wanting to do is increase the isolation gap between tracks and fill?

If so click on the pour polygon and in the properties change the "isolate" field

If you want to do it based on net connections go to "Rules DRC/ERC" and create a Net Class, so you might want a bit more isolation around all +5V tracks, create a Net Class for +5V, then switch to the rules tab and you'll be able to increase the "Clearance" field, when you next pour the copper it'll will give you more clearance around +5V tracks/pads.

Hope that helps.

[CaptainMJ]

Brilliant thanks, lots of good tips and yes this should resolve my problem. Many thanks!

[jorge_garcia · Accepted solution]

Hi @Spragnut,

The main advantage of this method is that it works on any layer. If you notice we only have 3 restrict layers one for top, one for bottom and one for vias. On a multi-layer board this is the best way to create voids on inner layers.

Unlike the restrict layers which flag any copper entering their boundaries and control the autorouter's behavior, cutout polygons only affect polygon pours. These cutout polygons do not serve as a restrict to the Autorouter or any of the assisted routing modes.

So it has one big advantage over the restrict layers and few cons against them. There's isn't currently a one size fits all solution that can handle either scenario.

Let me know if there's anything else I can do for you.

Best Regards,

[Spragnut]

@jorge_garcia 

Thanks for the information Jorge, I haven't attempted a 4 Layer board yet but this will help when I do!

Cheers

James