Altium Power Plane gerber Inverted?

[AJBotha]

Good Day

I used internal power planes for the first time (Altium), and I now want to generate fabrication outputs in the form of Gerbers.

The gerber below illustrates my internal GND plane, to avoid confusion with the fab house I would like to invert the gerber? Currently the voids are supposed to be copper and the copper is supposed to be voids? It looks to me like the whole gerber should be inverted.

Where do I change the settings for this?

Thank you!

[DutchGert]

Power planes are always inverted so they should not give any problems. U can always add a mechanical layer with layerstack, drill table and stuff like this.

On the other hand, be careful with power planes in altium, sometimes u end up with less copper than the min copper with between pads because altium simply not checks it. Personally I just use normal layers with polygons and fills as planes. Much more flexible in my opinion. Only thing u miss is impedance calculations but there are better external tools for that (http://www.saturnpcb.com/pcb_toolkit.htm)

[T3sl4co1l]

Altium's "Plane" support is crappy.

The shapes that will be created are limited: round or square, no ovals.  As mentioned, there is no clearance checking, so you constantly get thermal relief spokes dead-ending against other spokes, and copper necks that are too thin to fabricate.

You get full functionality with a normal positive mid-layer, and a polygon pour.

However, impedance calculation only works when there is a plane present.

So it's stupid.

Fortunately, you only need to know impedance once, and calculate the proper trace width based on that.  So it's not very important to use the built in controlled-impedance features.

Tim

[AJBotha]

Hi Guys

I don't know anything about impedance calculation anyway (and only slow speed stuff so far) so I won't really miss that. I just thought that this is the proper way to do it and tried the power plane thing.

So what you are saying is that I should just state to the fab house that it is inverted (because it's a negative plane?) and double check that I don't have any copper width violations?

Thanks for the answers!

[T3sl4co1l]

Yes.

[DutchGert]

In the image u provided there (probably) are already violations. See the 4 vertical pads in the middle for example. I assume the clearance between them is way to small....

Regarding impedances, it never hurts to put a stackup in the pcb toolkit and calculate impedances for the track with u plan to use. It usually is considered good practice to route everything at aproximately 50 ohm/100 ohm. Even low speed stuff can have fast edges

[AJBotha]

Thanks for the help guys.

For now I have fixed the copper slivers and put text next to the plane to indicate that it is a "Negative Layer" so that it is clearly visible on the Gerbers.

In the future I will go for a normal positive layer with a polygon.

PS. That Impedance Controlled PCBs kept me up all night. I will delve into that soon!

[jmarkwolf]

Hi Guys

So what you are saying is that I should just state to the fab house that it is inverted (because it's a negative plane?) and double check that I don't have any copper width violations?

Precisely.

The board houses are accustomed to this. Just notate in the Readme file that the planes are reverse image. I've been doing it this way for decades.