为了布线方便，需要修改Altium Design的规则
设计->规则（R）->
Design Rules->Electrical->Clearance->Clearance->Minimuim Clearance = 5mil
在Clearance下新建规则：右键->New Rule Name=Poly 在Where The First Object Matches 勾选为Advanced（Query） 并在右框Full Query修改为 (INPolygon) Minimuim Clearance = 10mil 此为创建关于覆铜的规则。
在Clearance下新建规则：右键->New Rule Name=Via-Poly 在Where The First Object Matches 勾选为Advanced（Query） 并在右框Full Query修改为 (IsVia) 在Full Query 修改为 INPOLY此为创建关于过孔到覆铜的规则。
Design Rules->Routing->Width->Width 全部修改为6mil
在Width下新建规则：右键->New Rule Name = Pwr 在Where The First Object Matches 窗口中选择电源和地的网络，（可以在Class中创建一个名为PWR的Nets，将电源和地添入Class）勾选Net Class，在Constrains中 将Min Preferred 和 Max Width分别修改为 10、12和60mil。
Design Rules->Routing->Routing Via Style->RoutingVias 中Constrains修改Via Diameter全部修改为16mil Via Hole Size 全部修改为8mil。
Design Rules->Routing->Mask->Solder Mask Expansion->SolderMaskExpansion 中Constrains修改Expansion = 2.5mil
Design Rules->Routing->Plane->Power Plane Connect Style ->PlaneConnect 中Constrains修改 Conductor Width = 10mil，AirGap = 8mil，Expansion = 6mil。
Design Rules->Routing->Plane->Power Plane Clearance->PlaneClearance 中Constrains修改 Clearance = 8 mil
Design Rules->Routing->Plane->Power Connect Style -> PolygonConnect 中Constrains修改 Conductor Width = 15mil
在Power Connect Style下新建规则：右键->New Rule Name = PolygonConnect_via 在Where The First Object Matches 勾选为Advanced（Query） 并在右框Full Query修改为 (isvia) 斌=并在Constraints中 Connect Style 选择 Direct Connect。次规则是为了将过孔和地的连接改为全部覆铜，增加平面完整性。