This window allows you to set the parameters to define the style of the pads and vias in the PCB.
Padstack
This section describes the shape of the pad for each layer of the PCB. The first line describes the default shape, i.e. the shape the pad takes for all layers for which no specific shape has been defined.
You can add more lines by clicking the Add button. To remove a line: select it and then click the Delete button.
Layer
The first column specifies the layer to which the description of the pad shape refers. The value of this field cannot be changed in the first line and indicates that the shape described applies to all layers for which no specific shape has been defined.
Shape
Select the pad shape from the list below:
Round |
|
The pad takes a circular or ellipsoidal shape depending on the values specified in the fields Width and Height. The value of the field Shape factor is irrelevant and can be zero. |
|||||||||||||||||||||
Rounded |
|
The pad takes a circular, square, rectangular or oblong shape depending on the values specified in the fields Width, Height and Shape factor. The value of the field Shape factor specifies the rounding percentage of all four edges of the pad. |
|||||||||||||||||||||
Semi-rounded |
|
The pad takes a square, rectangular or semi-oblong shape depending on the values specified in the fields Width, Height and Shape factor. The value of the field Shape factor specifies the rounding percentage of two of the four edges of the pad. |
|||||||||||||||||||||
Square |
|
The pad assumes a square or rectangular shape with blunted angles depending on the values specified in the fields Width, Height and Shape factor. The value of the field Shape factor specifies the smoothing percentage of all four corners of the pad. |
|||||||||||||||||||||
Sector |
|
The pad takes the form of a circle or ellipse sector depending on the values specified in the fields Width, Height and Shape factor. The value of the field Shape factor specifies the width of the sector. |
|||||||||||||||||||||
Polygon |
|
If the values specified in the Width and Height fields match, the pad takes the form of a regular polygon. The value of the field Rotation specifies the rotation of the shape. |
|||||||||||||||||||||
Shaped |
|
The basic shape of the pad is a square or a rectangle depending on the values specified in the fields Width and Height. The angles can be at 90 degrees, beved, sunken, or rounded depending on the format string specified in the Corners field. The format string can contain up to 4 characters, each of which describes the shape of a corner starting from the one at the bottom right and continuing counterclockwise. The value of the field Shape factor specifies the amplitude of the angle. The characters are as follows:
|
|||||||||||||||||||||
User |
|
The shape of the pad consists of a polygon centered at the point of coordinates (0.0) and described by a series of vertices and arcs. Vertices are pairs of coordinates (X,Y). The arcs are specified by the character A followed by the coordinates of the center and the angle of sweep (Ax,y,a) or the character C followed by the coordinates of the end point and the angle of curvature (Cx,y,a). Positive angle values draw the arc in the counterclockwise direction. The shape can be rotated by specifying the character R followed by the angle of rotation. The coordinates are specified in the field Vertices. The pad is resized to the values specified in the Width and Height fields. To keep the original dimensions, specify zero for Width and Height. For example, the string:(0,2)(-1,1)(-1,0)(-2,-0.5)(-2,-1)(A0,-1,180)(2,-0.5)(1,0)(1,1) describes the shape represented in the image on the left. |
Hole
The parameters in this group determine the presence and size of the hole.
- No Hole (SMD pad)
-
Specify if the pad has a hole.
- Hole diameter
-
Specify the diameter of the hole. The hole diameter may be larger than the pad diameter to define holes without a copper ring.
- X Offset from pad origin
-
Specify the horizontal offset of the hole to the center of the pad.
- Y Offset from pad origin
-
Specify the vertical offset of the hole from the center of the pad.
- Slot length
-
To create a slot with rounded ends, specify its length.
- Slot angle
-
Specify the rotation of the slot.
- Plated
-
Specify the hole type.
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 Subordinate mode Indicates that the solder mask is adjusted by the value set in the project properties. Settings » Project Properties » PCB » Settings » Solder Mask.
Top
Solder mask for the top side of the PCB.
- Mode
-
Select one of the following modes:
Subordinate
Indicates that for this type of pad the aperture value in the solder mask is adjusted by the value set in the Project.
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:
Subordinate
Indicates that for this type of pad the aperture value in the solder mask is adjusted by the value set in the Project.
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 Subordinate mode Indicates that the paste mask is adjusted by the value set in the project properties. Settings » Project Properties » PCB » Settings » Paste Mask.
- Mode
-
Select one of the following modes:
Subordinate
Indicates that for this type of pad the shape for the paste mask is adjusted by the value set in the Project.
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 the pad outline should be expanded to create the template for the solder paste. Typically, the shape of the solder 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.
- Use project settings
-
Indicates whether the pad uses the local settings or the settings defined in the project. Settings » Project Properties » PCB » Settings » Thermal Relief.
- 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.
- Use project settings
-
Indicates whether the pad uses the local settings or the settings defined in the project. Settings » Project Properties » PCB » Settings » Anti-Pad.
- 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 connect style
Specifies how the pad is to be connected to the surrounding copper plane or area.
The Subordinate mode Indicates that the connection to the plane is regulated by the value set in the Project properties. Settings » Project Properties » PCB » Settings » Plane connection.
- Top copper
-
Specify how the pad should be connected to the surrounding copper area on the top side of the PCB. Select one of the following modes:
Subordinate
Indicates that for this type of pad the connection mode is regulated by the value set in the project.
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 should be connected to the plane on any internal layer of the PCB. Select one of the following modes:
Subordinate
Indicates that for this type of pad the connection mode is regulated by the value set in the project.
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:
Subordinate
Indicates that for this type of pad the connection mode is regulated by the value set in the project.
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.
Keepout
Allows you to specify a keepout area around the mechanical holes.
- Pad to Keepout expansion
-
Specify the width of the keepout area from the outer contour of the pad. Specify zero to not include a keepout area.
Text on Pads
Specifies the position of the pad number.
- X Offset from pad origin
-
Specify the horizontal offset of the text origin from the pad origin.
- Y Offset from pad origin
-
Specify the vertical offset of the text origin from the pad origin.