New (Design Data)

The New (Design Data) dialog is described below. This dialog allows you to create a new PCB design file using the library that is set by clicking File > Configuration > Product Settings > Library. You can create a completely new design, or a design based on a specified schematic design or RINF netlist. Launch the New (Design Data) dialog by clicking File > New on the eCADSTAR PCB Editor ribbon.

Rules

The following details are specified in the Rules section of the New (Design Data) dialog.

Specify number of layers

Item	Description
Number of layers	Select the required number of layers. The values displayed are associated with the design rules in the technology library.

Specify design rule

Item		Description
Design rule		Select a design rule. Design rules are listed that are associated with the number of layers that you select in the Number of layers box.
Technology Information		Displays the technology name that is associated with the selected design rule.
Data resource		Allows you to optionally select an exported data resource file which contains dialog settings from an eCADSTAR design. Selecting a data resource file applies the exported settings to all relevant areas of the new design. This makes the design process more efficient as it allows you to set up a default configuration for the colors, and layer pair display settings. The following settings are not included in a data resource file: Values specified in the Layer Settings panel, Product Settings dialog or Application Settings dialog. Padstack name, in the Add Route dialog. Teardrop mode, in the Reinforce dialog.  Alternate part and Alternate footprint in the Change Part dialog. The names of 3D Model files.
		Select a data resource file by browsing to it in the displayed Open dialog.

 

 

Schematic

The following details are specified in the Schematic section of the New (Design Data) dialog.

Specify schematic

Item		Description
No schematic		If selected, a schematic design is not specified.
Schematic		If selected, the schematic data set and design rule list are extracted from the schematic file that you specify in the Schematic box. If there are variants in the schematic design, then they are automatically added to the design data file. Note Part data is provided by the schematic design, rather than the master library. A license is required to access the variation functionality in eCADSTAR. You can create a new PCB design from a schematic that contains SPICE Attributes. The SPICE attributes are added to the library, but are not added to the PCB design.
	Schematic	Displays the schematic design file (.sdes) from which the schematic data set and design rule list are extracted. Specify the path to this file, or browse to a schematic design file by clicking . Note If you specify a High Speed schematic design file, then a High Speed PCB design is created, regardless of whether you currently have a High Speed license. Whenever you open a new design without a High Speed license, the High Speed commands and constraints in eCADSTAR are made unavailable, and a warning is displayed. There is no impact on the design data. If you open the new design with a High Speed license, then the High Speed attributes are made available.
		Allows you to select a schematic design file (.sdes) by browsing to it in the displayed Open dialog. The schematic data set and design rule list are extracted from the schematic file that you specify.
	Update the association of the PCB design and the schematic	If selected, the design data that is created is associated with the specified schematic design file.
	Sheet range	Set the sheet range in the Sheet range and To boxes. This specifies the schematic sheets that are used in the design.
	Customize variant component suffix	If selected, then you can customize the suffix that is added to variant components in the specified schematic design file. The Suffix of variant component field is made available.
	Suffix of variant component	Allows you to customize the suffix that is added to variant components in the specified schematic design file. This field is made available if Customize variant component suffix is selected. If you do not enter a value in this box, or Customize variant component suffix is not selected, then variant components are displayed as follows: [Variant]_1 [Variant]_2 [Variant]_3   If you enter an alphanumeric value in this box, then it is added before the existing suffix. For example, if you of enter a value of "X", then the names of the variant components are as updated as follows: [Variant]_X1 [Variant]_X2 [Variant]_X3
	Load Clearance Class rules from schematic	If selected, then the clearance classes in eCADSTAR Schematic Editor are added to eCADSTAR PCB Editor. These are specified in the Clearance Class Manager dialog. Note If you specify a High Speed schematic design file, then a High Speed PCB design is created, regardless of whether you currently have a High Speed license.
RINF netlist		If selected, then you can create a new PCB design that electrically matches the RINF source that you specify. Items and nets in the RINF file are added to the design. Unconnected components can be added. The RINF netlist is a standard Zuken file format that can be output from schematic capture tools, including CADSTAR and OrCAD. Parts and footprints that are listed in the RINF file must be in the library, or the New (Design Data) process will fail. Components are not permitted that are specified in the RINF file by footprint only. A part that matches the footprint name must also be available. The Create Parts From Selected Footprints and Create Parts From All Footprints commands allow you to create matching parts for footprints in Library Editor.
	Netlist box	Displays the RINF netlist that is used to create the new PCB design. Click to select the required .frs or .net file in the Open dialog.
		Allows you to browse to a .frs or .net file in the displayed Open dialog. The contents of the RINF netlist is used to create the new PCB design If there is a problem with the specified file then a report dialog is displayed when you click Next.
	Update the association of the PCB design with the RINF netlist	Allows you to link the current PCB design with the RINF netlist that you specify in the Netlist box. The specified file is automatically displayed in the Netlist box when you execute the New (Design Data) command. By deselecting this box, you can execute the command for a different RINF netlist, without updating this link.
	Selected	The RINF netlist displayed in the Netlist box is linked to the current PCB design. The specified file is automatically displayed when you execute the New (Design Data) command. To link to another RINF netlist, click the button and browse to a different .frs or .net file. The specified file is automatically displayed when you next execute this command.
	Not selected	Allows you to execute the New (Design Data) command for the RINF netlist that is displayed in the Netlist box, without creating a link to the specified design. The next time you execute this command, the linked RINF netlist is displayed.

 

 

Board outline

The following details are specified in the Board outline section of the New (Design Data) dialog.

Board outline/Layout area

Item		Description
Create a board outline and layout area		Create a board outline and layout area on the canvas by selecting this check box. If selected, you can specify the creation details in this section of the dialog.
Creation method		Allows you to create a board outline and layout area on the canvas by specifying values in the Width [mm] and Height [mm] boxes, or by browsing to a design data file (*.pdes) to use as a template.
	Width/Height	Select this option to specify values in the Width [mm] and Height [mm] boxes.
	Copy from other design data	If selected, the Design data box is made available. Click by this box to browse to a design data file (*.pdes) to use as a template.
Width/Height		Allows you to specify the width and height of the board outline. This section is made available when Width/Height is selected in the Creation method box.
	Width [mm]	Specify the width of the board outline in millimeters.
	Height [mm]	Specify the height of the board outline in millimeters.
Design data		Specify a design data file (*.pdes) to use as a template. The board outline and layout area are copied from the specified file. This box is made available if you select Copy from other design data in the Creation method box.
		Allows you to select a design data file (*.pdes) to use as a template by browsing to it in the displayed Open dialog. This button is made available if you select Copy from other design data in the Creation method box.

 

Item	Description
Back	Displays the previous section in the New (Design Data) dialog.
Next	Displays the next section in the New (Design Data) dialog.
Finish	Creates a board using the specified details, and displays it on the canvas. If problems are detected when creating the design data, error or warning information is displayed in the New (Design Data) dialog. Click Close to close the dialog and create the board, if this is possible. If the specified technology information contains powerplanes, the Powerplane settings dialog is automatically displayed. Specify a net to assign to each powerplane by clicking in the Net assigned to powerplane column. The Select Net dialog is displayed. In the Powerplane settings dialog, click OK. The new board is created and displayed on the canvas.
Cancel	Closes the New (Design Data) dialog without creating new design data.