Power Planes in Protel99

[haytham]

ground plane protel99

Hi all
I want to know how could I make a pcb with power planes using Protel99
Apreciating your response

Haytham

 

[House_Cat]

If you mean real plane layers, you add them in the stack manager - menu Design>Layer Stack Manager. You can then draw plane layer splits by going to the menu Place>Split Plane. Real plane layers are drawn as negative layers - that is, any line placed on that layer indicates copper removed (voids).

If you mean copper pours (polygons), you draw them in by going to the menu Place>Polygon Plane. Polygons are positive objects - that is, anything you draw on the layer is a copper region.

 

[haytham]

Hi
I think I need the first one. I need just to emphasize on what I need and I want your confirmation.
I want the final PCB which I will fabricate to have all unused copper area to be acting as GND or VCC.
Would this option allow me to get this ??
Appreciating your F.B.

 

[House_Cat]

Planes on a PCB are solid copper. They are generally used for power distribution by connecting device pads and vias to the plane from components on the top and/or bottom of the board - you don't route any other signals on the plane. The planes act as the return path for signal traces on the adjacent layers. For a given kind of board material, the impedance of signal traces is controlled by adjusting the thickness of the dielectric between the signal layer and the plane layer, and the width of the signal trace.

Normally, a four layer circuit board would have: Top Signal Layer - Ground Plane - Power Plane - Bottom Signal Layer. Look here for more explanation: http://www.hottconsultants.com/techtips/pcb-stack-up-2.html

 

[haytham]

Hi House_cat
All I want is to make a TWO layers PCB. I want to use all unused routing areas as POWER PLANES connected to VCC or GND. I want to know how to make this using Protel99

Thanks
Haytham

 

[House_Cat]

Then you use polygons. You will find that command in the PCB editor 'Place>Polygon Plane' menu. Filling the unused portion of a routing layer with copper polygons is not the same as using a true "plane" - as I stated above, a true "plane" is a contiuous solid copper layer.

In Protel99SE, first make sure you have defined your board outline on the Keepout layer with a continuous outline. Place and route all components. As a final step, select Place>Polygon Plane. On the dialog that appears after you select the polygon place command, you will choose the layer, net, type of pour, and other connection options. You then draw the outline for the polygon over the board surface. Trace, pad, and object clearances will be done automatically based on the design rules you have set up. The available empty space will be filled with copper.