Community
Fusion Electronics
Working an electronics project and need help with the schematic, the PCB, or making your components? Join the discussion as our community of electronic design specialists and industry experts provide you their insight and best practices.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

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

9 REPLIES 9
SOLVED
Reply
Message 1 of 10
CaptainMJ
917 Views, 9 Replies

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

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

Best Regards,
Marcus
9 REPLIES 9
Message 2 of 10
Spragnut
in reply to: CaptainMJ

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.

Message 3 of 10
edwin.robledo
in reply to: CaptainMJ

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.

 

polygonCutout.png



Edwin Robledo
Tech Marketing Manager
Message 4 of 10
Spragnut
in reply to: edwin.robledo

@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

 

Message 5 of 10
CaptainMJ
in reply to: Spragnut

@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

Best Regards,
Marcus
Message 6 of 10
CaptainMJ
in reply to: edwin.robledo

Hi @edwin.robledo ,

 

Many thanks, I will try this technique as well!

 

Best regards,

Marcus

Best Regards,
Marcus
Message 7 of 10
Spragnut
in reply to: CaptainMJ

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

 

2020-02-05.png

 

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.

 

Message 8 of 10
CaptainMJ
in reply to: Spragnut

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

Best Regards,
Marcus
Message 9 of 10
jorge_garcia2
in reply to: Spragnut

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,


Jorge Garcia
​Product Support Specialist for Fusion 360 and EAGLE

Kudos are much appreciated if the information I have shared is helpful to you and/or others.

Did this resolve your issue? Please accept it "As a Solution" so others may benefit from it.
Message 10 of 10
Spragnut
in reply to: jorge_garcia2

@jorge_garcia2 

 

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

 

Cheers

James

 

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums