This tab contains some PCB settings.
Settings
Contains the default settings for various PCB elements.
Default styles
- Track
-
Select the default style for the tracks. The default track style is updated when you acquire a track style or when you select a style in the track style panel using the
button available on the PCB toolbar.
The default style for tracks can be used to update the style of tracks via the Copy style command.
Note: The default style for tracks is not used for new tracks or during routing operations. In these cases, the settings for the active routing class are used.
- Pad
-
Select the default style for the pads. The default pad style is updated when you acquire a pad style or when you select a style in the pad style panel using the
button available on the PCB toolbar.
The default pad style can be used to update the pad style via the Copy style command.
- Via
-
Select the default style for the via. The default vias style is updated when you acquire a vias style or when you select a style in the vias style panel using the
button available on the PCB toolbar.
Lo stile di default per le vias può essere usato per aggiornare lo stile delle vias tramite il comando Copy style.
- Filling style of copper areas
-
Select the filling style of the copper areas. Select None for solid copper areas or one of the available hatches.
- Thickness of the filling lines of copper areas
-
Specify the line thickness of the hatched fills.
- Spacing from copper to board outline
-
Specifies the distance to keep between the outline of the copper planes and the edge of the board. This value is used by the command: PCB » Copper » Filling » Copper Plane
.
Wire bridges
These settings define the footprint of wire bridges.
- Designator
-
Specify the prefix of the reference designator.
- Wire
-
Specify the diameter of the wire and whether the sheath is present.
- Assembly style
-
Specify the outline style and fill style.
- 3D Materials
-
Specify the materials to be used for the wire and sheath.
Solder mask
The Solder Resist is a paint, applied on the external sides of the PCB, in which openings are created in correspondence with the welding areas.
The following settings are generic and apply to all pads and vias on the PCB that have the style in which the solder mask mode is set to Subordinate. Locally you can redefine the openings in the solder mask according to the styles of the pads or for each individual pad by assigning it a private style.
Top
Solder mask for the top side of the PCB.
- Mode
-
Select one of the following modes:
Pad
The value of the opening in the solder mask corresponds to the shape of the expanded pad according to the value specified for the parameter Expansion.
Hole
The value of the opening in the solder mask corresponds to the shape of the expanded hole according to the value specified for the parameter Expansion.
Covered
Indicates that this type of pad does not have an opening in the solder mask. The pad is completely covered with the solder resist.
Filled
This indicates that for this type of pad the hole must be completely filled (Via Fill). This is done by covering the pad and the hole with a second layer of solder resist. To display the mask for Via Fill you need to set the relevant option in the properties of the layer (top or bottom solder resist) in the view.
- Expansion
-
Specify how much the shape of the pad or hole should be expanded to create the opening in the solder mask. Typically the shape for the solder mask is larger than that of the pad.
Bottom
Solder mask for the bottom side of the PCB.
- Mode
-
Select one of the following modes:
Pad
The value of the opening in the solder mask corresponds to the shape of the expanded pad according to the value specified for the parameter Expansion.
Hole
The value of the opening in the solder mask corresponds to the shape of the expanded hole according to the value specified for the parameter Expansion.
Covered
Indicates that this type of pad does not have an opening in the solder mask. The pad is completely covered with the solder resist.
Filled
This indicates that for this type of pad the hole must be completely filled (Via Fill). This is done by covering the pad and the hole with a second layer of solder resist. To display the mask for Via Fill you need to set the relevant option in the properties of the layer (top or bottom solder resist) in the view.
- Expansion
-
Specify how much the shape of the pad or hole should be expanded to create the opening in the solder mask. Typically the shape for the solder mask is larger than that of the pad.
Paste mask
The mask for applying welding paste is generally called a stencil. Generally, the shapes shown on the paste mask correspond to the SMD pads, or are slightly smaller. This stencil is used in the automatic SMD assembly welding process to coat SMD pads with tin paste.
The following settings are generic and apply to all PCB pads and vias that have the style in which the paste mask mode is set to Subordinate. Locally you can redefine the paste mask according to the styles of the pads or for each individual pad by assigning it a private style.
- Mode
-
Select one of the following modes:
Free
Indicates that welding paste must not be applied to this type of pad.
Covered
Indicates that for this type of pad the shape for applying the solder paste corresponds to the shape of the pad, expanded according to the value specified for the parameter Expansion. Typically, the shape of the solder paste is smaller than that of the pad.
- Expansion
-
Specify how much of the pad template must be expanded to create the template for the solder paste. Typically, the shape of the welding paste is smaller than that of the pad.
Thermal Relief
Thermal reliefs are used for pads that are positioned in large areas of copper (ground planes, voltage planes, thermal planes) in order to to realize the electrical connection of the pad to the plane providing a good thermal resistance during the welding process. The thermal pad is a normal pad with copper spokes that connect it to the surrounding copper.
The following settings are generic and apply to all pads and vias that have the style in which Thermal relief mode is set to Use project settings.
- Pad and Thermal Offset
-
Specify the distance between the outer contour of the pad and the thermal insulation area.
- Thermal Air-Gap
-
Specify the width of the thermal insulation area.
- Conductors
-
Specify the number of copper spokes that connect the pad to the plane.
- Conductor width
-
Specify the thickness of the copper spokes that connect the pad to the plane.
- Conductor angle
-
Specify the angle of the first copper spoke that connects the pad to the plane.
- Rounded
-
Specify whether the thermal insulation area should be rounded at the ends.
Anti-Pad
The Anti-Pad represents the distance between the outer contour of the pad or hole and the plane.
The following settings are generic and apply to all pads and vias that have the style in which Anti-Pad mode is set to Use project settings.
- Hole to Plane clearance
-
Specify the distance between the outer contour of the hole and the plane. Applies to all internal layers when the pad is not connected to the plane.
- Pad to Copper clearance
-
Specify the distance between the outer contour of the pad and the copper area. Applies to pads not connected to the surrounding copper area.
Plane connection
Specifies how the pad is to be connected to the surrounding copper plane or area.
The following settings are generic and apply to all PCB pads and vias that have the style in which the plane connection mode is set to Subordinate. Locally you can redefine the connection mode to the ground plane, using the pad styles or for each individual pad by assigning it a private style.
- Top copper
-
Specify how the pad should be connected to the surrounding copper area on the top of the PCB. Select one of the following modes:
Direct
Indicates that this type of pad is connected directly to the surrounding copper area.
Thermal
Indicates that this type of pad is connected to the surrounding copper area via thermal reliefs.
- All internal layers
-
Specify how the pad is to be connected to the plane on any internal layer of the PCB. Select one of the following modes:
Direct
Indicates that this type of pad is connected directly to the plane.
Thermal
Indicates that this type of pad is connected to the plane via thermal relief.
- Bottom copper
-
Specify how the pad should be connected to the surrounding copper area on the underside of the PCB. Select one of the following modes:
Direct
Indicates that this type of pad is connected directly to the plane.
Thermal
Indicates that this type of pad is connected to the plane via thermal relief.
Classes
DRC classes
The DRC classes define the electrical design rules for the PCB. A DRC class is a set of rules that define the distances that must be respected between the different elements on the PCB, such as the distance between a pad and a track or the distance between two pads. DRC rules can be assigned to a Net or Layer so that electrical rules can be defined that are only valid for the tracks and pads of a given Net or present on a given layer. See DRC classes.
Routing Classes
Routing classes define track and vias styles for PCB routing. Routing classes can be assigned to a Net or Layer so that you can define styles that are only valid for tracks and vias on a given Net or on a given Layer. See Class Routing.
Net Classes
The Net classes define the Net styles. They include the wire style in the schematic and the DRC and Routing classes for the PCB. See Net Classes.