Keep Out Pattern

Check routing status from certain components.

If signal pattern under certain components can make electrical or mechanical problem, you can define keep-out area from components.
  • Checking for pattern existence in component area:
    • Item: Specify the item name.
    • Component Group: Select target components from the component group list.
    • Component Boundary: Select component boundary criteria among pad, Component Overlap Checking Area (COC), silkscreen, silkscreen + pad, Measure (definition in component classification dialog), and PAD Inside (Pads’ inside area).
    • Expand Component Boundary: Component boundary expanding area. To define expanding distance, set the expanding distance value.
    • Contitional Layer: Option to define a area which will be recognized as a keepout area that overlapped with the keepout components.
    • Target Layer: Define target layers.
      • Component Placed Layer: Same with component placed layer will be target layer. Meaning, if component placed on top layer, patterns on top layer will be checked.
      • Opposite Layer: Layer which is opposite the component placed layer will be target layer.
      • Inner Layer: Inner layer pattern will be checked.
        • All: Check all inner layers.
        • From Component Placed Layer: Check the specified number of inner layers from the component placed layer.
        • From Opposite Layer: Check the specified number of inner layers from the opposite side of the component placed layer.
    • Target Object Definition: Define target objects for checking.
      • Copper: If copper-pour exists in checking area, it will be detected.
      • Trace: If routing patterns exist in checking area, it will be detected.
        • Minimum Trace Width: Define minimum trace width for checking.
        • Maximum Trace Width: Define maximum trace width for checking.
      • Through Via: If Through Via exists in checking area, it will be detected.
      • Blind Via: If Blind Via exists in checking area, it will be detected.
      • Buried Via: If Buried Via exists in checking area, it will be detected.
    • Target Net
      • Same Net: Patterns with the same net name with pins will be target routing patterns. In this option, different net name pattern will not be checked.
      • Other Net: Patterns with different net name with pins will be target routing patterns. In this option, same net name pattern will not be checked.
      • Specific Net: Option to check specific nets by using string filter.
    • Except Net Name Filter: Option to exclude certain Net from checking by using string filter.
    • Void-Checking Component Group: Select void-checking components with selecting components group list. Void-Checking components would be eyelet components or heatsink.
      Figure 1.


    • Distance from void-checking Comp: For patterns connected to void-checking components within given distance from void-checking components, PollEx DFM skips to check them.
  • Checking for pattern existence between adjacent pins: Check patterns between two adjacent pins.
    • Item: Specify the item name.
    • Comp Group: Select target components from component group list.
    • Target Layer: Define target layers.
      • Component Placed Layer: Same with component placed layer will be target layer. Meaning, if component placed on top layer, patterns on top layer will be checked.
      • Opposite Layer: Layer which is opposite with the component placed layer will be target layer.
      • Inner Layer: Inner layer pattern will be checked. Select the inner layer physical layer number.
    • Same Net: Check patterns with the same net name with connected pins.
    • Other Net: Check patterns with the same net name with connected pins.
    • Copper: If copper-pour exists between two adjacent pins, it will be detected.
    • Trace: If routing patterns exist between two adjacent pins, they will be detected.
    • Via: If via exists between two adjacent pins, it will be detected.
    • Checking Area reduction Ratio(%): Option to reduce the target pin and pin area by the entered ratio from checking.
    • Except Net Name Filter: For void-checking routing net selection, use net name filter. Use net name filtering tool.
  • Clearance between target component nets.
    • Item: Specify the item name.
    • Comp Group: Select target components from component group list.
    • Component Boundary: Select component boundary criteria among pad,Measure (definition in component classification dialog) Component Overlap Checking Area (COC), silkscreen, silkscreen + pad, and COC+Pad.
    • Target Layer: Define target layers.
      • Component Placed Layer: Same with component placed layer will be target layer. Meaning, if component placed on top layer, patterns on top layer will be checked.
      • Opposite Layer: Layer which is opposite with the component placed layer will be target layer.
      • Inner Layer: Inner layer pattern will be checked. Select the inner layer physical layer number.
    • Check Option: Specify the check option.
      • Clearance: The value inputted by the user is recognized as Net Clearance and expressed in the form of "Clearance:Value" in the Check Option column.
      • Set clearance value with the shortest distance between pads: Recognizes the shortest pad distance of the part to be checked as Net Clearance, expressed in the form of "Shortest distance between Pads" in the Check Option column.