Optional Creation of Copper Planes and Copper Pour Areas

Copper planes are solid copper blocks where airgaps for pads/ traces will not be created. Such copper areas are usually used for shielding and as Keep Off Zones. It is recommended not to use these copper areas for distributing power supply or ground since Pwr/ Gnd Planes mode is used for such purposes. In some cases, it may be necessary to relieve certain areas on the board from copper. This may be done by creating Copper pour areas in any shape. Atleast three vertexes must be defined. These introduced relieve copper on the processed layer.

Creation Of Copper Planes

Copper planes may be added to all layers in the board other than Component Print and Solder Print. Copper areas at any location and of any shape may be created using a combination of open or filled graphic items such as lines, rectangles, circles and arcs. The procedure is similar to creating library elements except that, in this case, items are created directly on the board. By default, copper items created will be assigned to the last net selected or may be assigned by selecting the net from the drop down of select net in the parameter window. It is possible to hange the net assignment made using the Change Item Net Assignment. This change can be viewed using the function tool Display Net Info. It is also possible to create copper planes which are not connected to any net. This may be used to create isolated pockets which may be used later. For this purpose, solid copper areas which are not connected to any net are created using the option tool No net.These areas may be used as Keep Off Zones which provide a hindrance to autorouting operation. Such planes are needed to reserve space for mounting power dissipaters such as radiators on the PCB. Copper areas may also be created in the form of polygons filled with crossed hatch patterns. Such areas are mainly used for shielding purposes. The pitch between the lines may be defined. Hatch patterns may be generated with lines crossing in 45 or 90 degrees using the function tool Hatch copper
Note: Copper planes created in this manner will be solid copper blocks where airgaps for pads/ traces will not be created. Such copper planes are usually used for shielding and as Keep Off Zones. It is recommended not to use these copper planes for distributing power supply or ground since Pwr/ Gnd Planes mode is used for such purposes.

Creation of Copper Pour Areas

Copper Pour Areas are polygons and are presented on normal display only as boundaries, drawn with dashed lines. The color are the same as layer's they are placed on. Copper Pour Areas may be created only on trace layers (from Component Layer to Solder Layer) and each must be logically connected to some reference net. It is possible to change the net assignment made using the Change Item Net Assignment. This change can be viewed using the function tool Display Net Info. The net assigned to a Copper Pour Areas may be changed using the Change net item as in the case of a copper plane. There is no formal limitation regarding the number of Copper Pour Areas. But on single layer they cannot be connected to more than 16 different nets.
Note: There are several editing functions facilitating necessary operation on Copper Pour Areas. Internally, Copper Pour Areas are stored as linked Line items as shown in Fig1 and interpreted by the program as one entity. So functions like for example Move or Delete work on whole area. The effects are visible when Edit/ Artwork is invoked.
On the artworks, Copper Pour Areas are drawn as filled polygons. All traces inside are drawn with airgaps. Pads not belonging to net to which given Copper Pour Area is connected are also drawn with airgaps. Pads which are nodes in reference nets and are inside connected Copper Pour Area are drawn as heat relief pads as shown in Fig2. If they are outside Copper Pour Area, then they are drawn as any other pad.





Note: Copper Pour Areas function as valid net containers as in previous versions. The difference is distinct. You may simply draw boundaries wherever the copper is to be poured and the rest is automatically taken care of by the program. HRF pads will be displayed where needed - but only if Hrf graphic items are present in the padstack, of course. User doesn't have to select which net is reference net either. Program assumes that all nets which have Copper Pour Areas assigned to them on given layer are automatically treated as reference nets.This new technique has profound consequences for generating Gerber data.