Sets the Thermal Reliefs.

syntaxSyntax:
DlxPadStyle.SetThermal(mode = DlxApp.THERMALFLAGS_STANDARD, padGap = 0, airGap = 0.3, spokeWidth = 0.3)

Parameters

Parameter Description
mode Specifies how to apply the thermal relief. Use a combination of the following values:
Use one of these values to indicate how the thermal relief should be applied to the top layer of the PCB.
DlxApp.THERMALFLAGS_TOPSTANDARD The pad uses the settings defined in the project.
DlxApp.THERMALFLAGS_TOPDIRECT The pad is connected directly to the plane if the nets coincide.
DlxApp.THERMALFLAGS_TOPISOLATED The pad is always isolated from the plane even if the nets coincide.
DlxApp.THERMALFLAGS_TOPTHERMAL The pad is connected to the plane via the thermal pads if the nets coincide.
Use one of these values to indicate how the thermal relief should be applied to all inner layers of the PCB.
DlxApp.THERMALFLAGS_INNERSTANDARD The pad uses the settings defined in the project.
DlxApp.THERMALFLAGS_INNERDIRECT The pad is connected directly to the plane if the nets coincide.
DlxApp.THERMALFLAGS_INNERISOLATED The pad is always isolated from the plane even if the nets coincide.
DlxApp.THERMALFLAGS_INNERTHERMAL The pad is connected to the plane via the thermal pads if the nets coincide.
Use one of these values to indicate how the thermal relief should be applied to the bottom layer of the PCB.
DlxApp.THERMALFLAGS_BOTTOMSTANDARD The pad uses the settings defined in the project.
DlxApp.THERMALFLAGS_BOTTOMDIRECT The pad is connected directly to the plane if the nets coincide.
DlxApp.THERMALFLAGS_BOTTOMISOLATED The pad is always isolated from the plane even if the nets coincide.
DlxApp.THERMALFLAGS_BOTTOMTHERMAL The pad is connected to the plane via the thermal pads if the nets coincide.
Use one of these values to indicate how the thermal relief should be applied to all layers of the PCB.
DlxApp.THERMALFLAGS_STANDARD The pad uses the settings defined in the project on all layers of the PCB.
DlxApp.THERMALFLAGS_DIRECT The pad is connected directly to the plane on all layers of the PCB if the nets coincide.
DlxApp.THERMALFLAGS_ISOLATED The pad is always isolated from the plane on all layers of the PCB even if the nets coincide.
DlxApp.THERMALFLAGS_THERMAL The pad is connected to all planes of the PCB via the thermal pads if the nets coincide.
DlxApp.THERMALFLAGS_SETGEOMETRY If this flag is specified, the padGap and airGap values are used to set the thermal relief geometry, otherwise the values specified in the project are used.
DlxApp.THERMALFLAGS_ROUNDSPOKES Use a rounded line for the air gap.
DlxApp.THERMALFLAGS_ROTATESPOKES The thermal spokes are rotated.
DlxApp.THERMALFLAGS_SPOKES2 Use only two spokes instead of four.
padGap Specify the distance between the outer contour of the pad and the thermal insulation area.
airGap Specify the width of the thermal insulation area.
spokeWidth Specify the thickness of the copper spokes that connect the pad to the plane.

Return Value

If the operation ends correctly, it returns true otherwise it returns false.

Example

  Copy codeCopy code 
var prj = DlxApp.GetJob().GetProject("Example PCB");
if (!prj.IsValid())
  prj = DlxApp.GetJob().NewProject("Example PCB");
var doc = prj.GetDocument("Examples PCB", DlxApp.DOCTYPE_PCB);
if (!doc.IsValid())
{
  doc = prj.NewDocument("Examples Pcb", DlxApp.DOCTYPE_PCB);
  doc.SetPageFormat("A4", false);
  var page = doc.NewPage("PCB", 0, true);
  page.LoadLayerStack("2 layer pcb stackup.clxlys");
  page.DrawBoard(new DlxRect(10, 10, 290, 200));
  page.SelectView("Draw Copper From Top");
}
if (doc.IsValid() && doc.Activate())
{
  var page = doc.FindPage("PCB");
  if (page.IsValid() && doc.SelectPage(page))
  {
    var layer = page.GetLayerFromType(DlxApp.LAYERTYPE_TOPCOPPER);
    if (layer.IsValid())
    {  
      var padstyle = new DlxPadStyle();
      padstyle.SetShape(DlxApp.LAYERTYPE_ALLPCBLAYERS, DlxApp.PADSHAPE_ROUNDED, 1.5, 2.0, 0.5);
      padstyle.SetHole(0.5, true, -0.45, -0.25, 1, 30);
      padstyle.SetThermal(DlxApp.THERMALFLAGS_STANDARD|DlxApp.THERMALFLAGS_SETGEOMETRY, 0, 0.5);
      layer.DrawPad(new DlxPoint(100,150), padstyle, "1");
    }
  }
}

See also