EDAImporter_Dlg-ImporterManagerFormImport Wizard_AD

Created: 九月 12, 2016 | Updated: 二月 15, 2020 | Applies to versions: 17.0 and 17.1

您正在阅读的是 17.1. 版本。关于最新版本，请前往 EDAImporter_Dlg-ImporterManagerForm((Import Wizard))_AD 阅读 22 版本

The Import Wizard will quickly and easily convert your design files from other vendors to Altium Designer files. The Wizard walks you through the import process, handling both the schematic and PCB parts of the project, as well as managing the relationship between them.

To make use of the importer technologies available in Altium Designer, you must install the relevant functionality as part of the Altium Designer Platform itself. The core design functionality for your installation can be modified at any time after installation and directly from within the Extensions & Updates view (DXP » Extensions and Updates). From the Installed page, click the Configure control at the top-right of the Platform region. This accesses the Configure Platform page that presents the core feature set for the software and is identical in content to that found on the Select Design Functionality page of the Altium Designer Installer. Enable the required functionality in the Importers\Exporters region of this page.

Using the Import Wizard

The Import Wizard is launched by clicking File » Import Wizard from the main menus.

Wizard Navigation

Click Cancel to close the Import Wizard.
Click Back to navigate to the previous screen.
Click Next to navigate to the next screen.
Click Finish to close the Import Wizard. This option is available only on the final page of the Wizard.

Selecting the Type of Files to Import

Use this page of the Wizard to select the types of files you want to import into Altium Designer. The Import Wizard can be used to import the following types of design files:

File Types	Description
Protel 99SE DDB Files	99SE DDB (*.ddb)
Cadence® Allegro® Design Files	Allegro binary PCB (.brd), Allegro ASCII PCB (.alg)
Zuken CADSTAR® Designs and Libraries	CADSTAR Schematic Archive (.csa), CADSTAR PCB Archive (.cpa), CADSTAR Part Library (*.lib)
CircuitMaker 2000 Schematics and Libraries	CircuitMaker Schematics (.ckt), CircuitMaker User Libraries (.lib), CircuitMaker Device Libraries (*.lib)
Mentor Graphics® DxDesigner® Designs and Libraries	DxDesigner Designs, DxDesigner Libraries
Mentor Graphics® Expedition® Designs and Libraries	Mentor Expedition files (.pcb, .lib).
Cadence® OrCAD® Designs and Libraries	OrCAD Capture Designs (.dsn), OrCAD Layout PCB documents (.max), OrCAD Capture Libraries (.olb), OrCAD PCB Libraries (.llb)
Cadence® OrCAD® CIS Configuration Files and Libraries	OrCAD CIS Configuration file (.dbc) in binary format, OrCAD Library files (.llb, *.olb)
Mentor Graphics® PADS® Layout and PADS® Logic Designs and Libraries	PADS Layout ASCII Design files (.asc), PADS Layout ASCII Decal Libraries (.d), PADS Logic ASCII Design files (.txt), PADS Logic ASCII CAE Decal Libraries (.c), PADS Logic ASCII Part Type Libraries (*.p)
Cadence® OrCAD® and Mentor Graphics® PADS® Designs and Libraries	OrCAD Capture files (.dsn), OrCAD Schematic Library files (.olb), PADS Logic ASCII Design files (.txt), PADS Layout ASCII Decal Libraries (.d), PADS Logic ASCII CAE Decal Libraries (.c), PADS Logic ASCII Part Type Libraries (.p)
P-CAD Designs and Libraries	P-CAD V16 or V17 Binary Schematic design files (.sch), P-CAD V16 or V17 ASCII Schematic design files (.sch), P-CAD V15, V16, or V17 Binary PCB design files (.pcb), P-CAD V15, V16, or V17 ASCII PCB design files (.pcb), P-CAD V16 or V17 Binary Library files (.lib), P-CAD V16 or V17 ASCII Library files (.lia)
Autodesk® EAGLE™ schematic, PCB and Libraries	EAGLE design files saved with EAGLE version 6.4.0 or later. These files are XML-format – EAGLE binary-format design files cannot be imported using the EAGLE Importer; they must first be saved in XML-format in EAGLE.
Zuken CR5000 Design Files	Zuken CR5000 PCF Files (.PCF), Zuken CR5000 FTF Files (.FTF), Zuken CR5000 EDS Files (*EDS). Zuken binary files must be converted to ASCII files before importing.

Click Get More Importers to open the Extensions & Updates page from where you can add additional extensions if needed.

The subsequent pages of the Wizard change depending upon the file type you selected. Find your file type in the following list and click on the link to access the information regarding that file type.

99SE DDB Files

The 99SE DDB import process requires all files, projects and design workspaces currently open in Altium Designer to be closed. A dialog will open asking for confirmation.

Click Yes to close all open files and projects; click No to exit the Wizard.

Choosing Files to Import

Use this page of the Wizard to select the 99 SE folders or files you want to import. Use the Add button under the Folders To Process region to import all DDB files within the specified folder. Use the Add button under the Files To Process region to import individual DDB files. The Remove button under both regions can be used to delete a selected entry from either region.

Setting File Extraction Options

This page of the Wizard allows you to control how your files are extracted. Use the Browse Folder icon to search for and select the location of the output folder. All files will be extracted into a sub-folder of the same name as the DDB.

Setting Schematic Conversion Options

Use this page to control how the schematic designs will be converted.

Enable Convert Schematic documents to current file format if you want the current format to be used. If this option is enabled, locked (manual) junctions will be imported as is. Use the following options to select how to import non-locked (auto) junctions:

Lock All Auto-Junctions - select this option to lock all auto-junctions.
Lock X-Cross Junctions Only - select this option to lock only X-Cross junctions.
Convert X-Cross Junctions - select this option to convert X-Cross junctions.

The 'preview' region on the right dynamically updates depending upon your selection. Locked junctions display as red.

Miter Size (in DXP units) - If Convert X-Cross Junctions is selected, enter the miter size in the text box.

Setting Import Options

Use the Project Mapping Options on this page to control how projects will be mapped into your database files.

Create one Altium Designer project for each DDB - select if you typically use one DDB for each board design.
Create one Altium Designer project for each DDB Folder - select if your DDB contains more than one board design.
Include non-Protel files (such as PDF or Word) in created Projects - select if you also want to include other file types.

Selecting the Design Files to Import

On this page of the Wizard, a list of DDB files appear that Altium Designer has found according to your import settings on previous pages of the Wizard. Enable the checkboxes of the design files you want to import. If you want to import all the displayed files, you also can click Import All to check all boxes. If you want to not import any of the listed files, click Import None to uncheck all boxes.

Review the Project Structure

This page of the Wizard can be used to fine tune how your projects will be created. This page displays the assumptions that the Wizard has made about how it should build projects based on the contents of the DDB. Take time to configure these options to ensure you achieve the best result at the completion of the import process. Click in the Mapping column as shown in the following image, then select from a list of available options to change how the selected folder/file is created. Options include:

Do not create project - select to not create a project.
Create PCB project - select to create a project.
Create Integrated Library package - select to create an integrated library package.
Add files to parent project - select to add the files to the parent project.
Add files to all projects in DDB - select to add the files to all projects in the DDB.

Click in the Documents to Add column to select from a list of available documents to add.

Review the Import Summary

This page of the Wizard shows a summary of the import. The Source Files region shows the number of DDB designs that will be imported. The Output region lists the files that will be created during the import process. This page is useful for ensuring that you have configured your import settings correctly. You can use the Back button if any changes are required.

Click Next to run the import process.

Select the Workspace

The import process has completed and you can choose whether to open the imported designs on this page. Select Open Selected Workspace, then choose from the listed designs to open a workspace. If you do not want to open the imported designs, select Don't Open Imported Designs.

Closing the Wizard

The Wizard has completed successfully. Click Finish to close.

99 SE CAM Manager (*.cam) and Power Print Configuration (*.ppc) files are not recognized by Altium Designer, so outputs will need to be reconfigured for imported designs.

Allegro Design Files

The Import Wizard handles both Allegro PCB Design files (*.brd) and Allegro ASCII Extract files (*.alg). If you have Allegro PCB Editor versions 15.2 or 16 installed, you can directly translate Allegro PCB Design files (*.brd) into Altium Designer PCB files (*.PcbDoc).

Selecting the Files to Import

Click Add to choose which Allegro design files to import. You can delete a selected file by clicking Remove. The Analyzing Files page will appear as shown below and display a green bar to show the progress of the analysis. The next page of the Wizard will appear once the analysis is complete.

Setting the Reporting Options

Use the Reporting Options page to set up general log reporting options. A Log Report in ASCII file format (*.LOG) is generated for each translated Allegro PCB file. This log is saved in the \Imported sub folder of your original Allegro files. Open the Log Report after translation in a text editor to examine the details.

Under General Settings, enable the desired options: Log All Errors, Log All Warnings, and Log All Events.

Setting PCB Specific Options

This page of the Wizard is used to specify options specific to the PCB import process.

Select the desired Polygon Connect Options: either Use direct connect for default polygon connect style or Use relief connect for default polygon connect style.

Select the Plane Connect Options: either Use direct connect for default plane connect style or Use relief connect for default plane connect style.

Enable Import Auto-Generated Copper Pour Cutouts to import the voids that are auto-generated in the Allegro PCB Editor as cutouts when the file is translated.

Editing the Layer Mapping

This page of the Wizard is used to review and edit the layer mapping for each Allegro PCB. Default mapping is provided by the Wizard to build the layer mapping for each PCB. Layer mapping can be customized for each of your designs to be imported. You may wish to import multiple Allegro PCB designs and map the same Allegro layer to the same Altium Designer layer. You can set your layer mapping once and use this layer mapping for all of your files to be imported. The advantage of importing in this manner is that batch layer management can save time when importing multiple designs. The disadvantage to using this is that Default Layer Mapping is not always intelligent with differing structures in designs, and therefore, some manual changes may be required.

The Allegro Layer Name, Allegro Layer Type, and Altium Designer Layer are listed in the grid region. Use the drop-down arrow () on the right-hand side of each region to filter the displayed list of that region.

Use the Menu button to manipulate the layer mappings.

Invert Selection - select to invert the items that are selected to not selected, and those that are not selected to selected.
Set Selection To - select to access a sub-menu of layer types from which you can choose the desired layer.
Load Layer Mapping - select to open the Load Configuration dialog to load the desired mapping files.
Save Layer Mapping - select to open the Choose File to Save Layer Mapping dialog and choose the path in which to save the layer mapping.

Right-clicking in the grid region gives access to the same menus and sub-menus as clicking the Menu button.

Specifying the Output Directory

Use this page of the Wizard to review the output project structure and specify the output directory in which to import the files. Use the Browse Folder icon to search for and choose the Project Output Directory.

Click Menu to access options to edit the project structure:

Create Project - click to open the Create Project dialog to add a project.

Use the Create Project dialog to add a new project.

Rename Project - click to rename the selected project. This option is available only when a *.PrjPcb file is selected.
Remove Selected Projects - click to remove the selected project from the PCB Projects structure.
Reset Structure to Default - click to reset the PCB Projects structure to the defaults.
Add Designs to Project - click to add a design(s) to the project. This option is available only when a *.PrjPcb file is selected.
Remove Selected Designs - click to remove the selected design files.

Right-clicking in the PCB Projects region gives access to the same menus and sub-menus as clicking the Menu button.

Closing the Wizard

The Allegro Import Wizard has completed. Click Finish to close the Wizard.

Imported Allegro files:

Allegro files translate as follows:

Allegro Binary PCB Design files (*.brd) translate to Altium Designer PCB files (*.PcbDoc).
Allegro ASCII Extract Files (*.alg) translate to Altium Designer PCB files (*.PcbDoc).

CADSTAR Designs and Libraries

The Import Wizard supports the following CADSTAR file type:

PCB design
PCB component library
Schematic design
Part library and schematic symbol library

The Import Wizard does not support binary CADSTAR file. The binary CADSTAR file must be converted to CADSTAR archive file before importing to Altium Designer. The CADSTAR archive file usually has the extension .cpa or .csa.

Importing CADSTAR Design Files

This page of the Wizard is used to select which CADSTAR design files to import. You can import CADSTAR PCB designs (*.cpa) or CADSTAR schematic designs (*.csa).

Click Add to choose which CADSTAR design files to import. You can delete a selected file by clicking Remove.

Selecting CADSTAR Library Files

This page of the Wizard is used to select which CADSTAR library files to import.

Click Add to choose which CADSTAR library files to import. You can delete a selected file by clicking Remove.

Setting the Reporting Options

Use the Reporting Options page to set up general log reporting options.

Under General Settings, enable the desired options: Log All Errors, Log All Warnings, and Log All Events.

Editing the Layer Mapping

This page of the Wizard is used to review and edit the layer mapping for each CADSTAR PCB design or library. Default mapping is provided by the Wizard to build the layer mapping for each PCB. Layer mapping can be customized for each of your designs to be imported. You may wish to import multiple CADSTAR PCB designs and map the same CADSTAR layer to the same Altium Designer layer. You can set your layer mapping once and use this layer mapping for all of your files to be imported. The advantage of importing in this manner is that batch layer management can save time when importing multiple designs. The disadvantage to using this is that Default Layer Mapping is not always intelligent with differing structures in designs, and therefore, some manual changes may be required.

The CADSTAR Layer Name, Altium Designer Layer, and CADSTAR Layer Type (Sub Type) are listed in the grid region. Use the drop-down arrow () on the right-hand side of each region to filter the displayed list of that region.

Use the Menu button to manipulate the layer mappings.

Invert Selection - select to invert the items that are selected to not selected, and those that are not selected to selected.
Set Selection To - select to access a sub-menu of layer types from which you can choose the desired layer.
Load Layer Mapping - select to open the Load Configuration dialog to load the desired mapping files.
Save Layer Mapping - select to open the Choose File to Save Layer Mapping dialog and choose the path in which to save the layer mapping.

Right-clicking in the grid region gives access to the same menus and sub-menus as clicking the Menu button.

Specifying the Output Directory

A page showing a green progress bar opens and displays the document that is currently being processed with a green bar to show the progress of the import.

Closing the Wizard

The CADSTAR Import Wizard has completed. Click Finish to close the Wizard. The output project/file structure will display in the Altium Designer workspace panel.

CADSTAR files translate as follows:

CADSTAR pcb design (layout) archive (*.cpa) files will be translated to Altium Designer pcb documents (*.pcbdoc).
CADSTAR schematic archive (*.csa) files will be translated to Altium Designer schematic documents (*.schdoc).
CADSTAR part library (*.LIB) and symbol archive (*.csa) files will be translated to Altium Designer Schematic Library files (*.schlib).
CADSTAR pcb archive file (*.cpa) will be translated to Altium Designer PCB Library files (*.pcblib).

CircuitMaker 2000 Schematics and Libraries Files

Importing CM2000 Design Files

Click Add to choose which CircuitMaker schematic files to import. The added files will be imported as Altium Designer schematic documents and will be grouped into Altium Designer PCB projects. You can delete a selected file by clicking Remove.

Selecting CM2000 Library Files

The Wizard requires valid standard devices library files (DEVICE.LIB), user library files (USER.LIB), and models. The Wizard also requires those libraries and models to be imported first before the .CKT files can be processed. The libraries and models need to be imported only once. If the Altium Designer libraries and models paths are set correctly on this page of the Wizard, the import process will make use of the cached result.

CircuitMaker libraries / models path(s)

Use the Browse folder icons to set the desired paths for CircuitMaker 2000 Standard Devices Path (DEVICE.LIB file), CircuitMaker 2000 User Library Path (USER.LIB file), and CircuitMaker 2000 Models Path (MODELS directory).

Enable Import for each library and/or model path you want to import.

Altium Designer Libraries / Models Path

Use the Browse folder icons to set the Libraries Path and Models Path.

Setting Reporting Options

Use the Reporting Options page to set up general log reporting options.

Under General Settings, enable the desired options: Log All Errors, Log All Warnings, Log All Events.

Specifying the Output Directory

Every PCB project will reside in a separate directory within a specified output directory. Note that each project can contain only one CircuitMaker .CKT file. Use this page of the Wizard to review the output project structure and specify the output directory in which to import the files. Use the Browse Folder icon to search for and choose the Project Output Directory.

Click Menu to access options to edit the project structure:

Create Project - click to open the Create Project dialog to add a project.

Use the Create Project dialog to add a new project.

Rename Project - click to rename the selected project. This option is available only when a *.PrjPcb file is selected.
Remove Selected Projects - click to remove the selected project from the PCB Projects structure.
Reset Structure to Default - click to reset the PCB Projects structure to the defaults.
Add Designs to Project - click to add a design(s) to the project. This option is available only when a *.PrjPcb file is selected.
Remove Selected Designs - click to remove the selected design files.

Right-clicking in the PCB Projects region gives access to the same menus and sub-menus as clicking the Menu button.

A page opens and displays the document that is currently being processed with a green bar to show the progress of the import.

Closing the Wizard

The CircuitMaker 2000 Import Wizard has completed. click Finish to close the Wizard.

Imported CircuitMaker 2000 files translate as follows:

CircuitMaker 2000 schematics (*.CKT) translate to Altium Designer schematic documents (*.SchDoc).
CircuitMaker 2000 user and device libraries (*.LIB) translate to Altium Designer schematic libraries (*.SchLib).

DxDesigner Designs and Libraries Files

Importing DxDesigner Projects

Click Add to choose which DxDesigner project folders to include in the import process. You can delete a selected file by clicking Remove.

Importing DxDesigner Libraries

Click Add to choose which DxDesigner library folders to include in the import process. You can delete a selected file by clicking Remove.

Setting Reporting Options

Use the Reporting Options page to set up general log reporting options.

Under General Settings, enable the desired options: Log All Errors, Log All Warnings, Log All Events.

Configuring Import Options

General Options

DxDesigner projects can contain links to other libraries. Enable Add Linked Libraries to the List of Libraries for Import to import these libraries. This option can be customized on a project-by-project basis on another page in the Wizard.

Boxes in Altium Designer only support hollow or solid drawing modes. Use the Convert Gridded and Hatched Boxes to drop-down to select how gridded or hatched boxes are translated: Hollow or Solid.

Class Attribute Options

In the No BOM and No ECO textboxes, enter the Class attribute value(s) for the component that will not appear in either the BOM or ECO or both. You can enter multiple values separated by a comma.

Setting Linked Library Options

For each project folder listed, enable Import to import linked libraries.

Review Output Project Structure

Review the project structure listed on this page of the Wizard. Every workspace document will reside in a separate directory within the specified output directory. The PCB projects and schematic documents imported from the DxDesigner designs also will be placed in the folder. Use the Browse Folder icon to search for and select the desired Output Directory.

Closing the Wizard

The DxDesigner Import Wizard has completed. Click Finish to close the Wizard.

Imported DxDesigner project paths and schematic files translate as follows:

Project paths have an equivalent Altium Designer PCB (*.PrjPCB) project automatically created for them. Once translated, files are grouped into that PCB project. For example, if you specified C:\my_projects\LED_Matrix_Display as the DxDesigner project path, the Import Wizard will create LED_Matrix_Display.PcbPrj in Altium Designer.
Schematic files (Name.N) translate to Altium Designer schematic files (*.SchDoc). Each schematic file will be imported as a single Altium Designer schematic file. Design hierarchy is maintained, including complex hierarchy.

EAGLE Projects and Designs

Importing EAGLE Design Files

Click Add to choose which EAGLE design archives (BRD and/or SCH) to include in the process. You can delete a selected file by clicking Remove.

Importing EAGLE Library Files

Click Add to choose which EAGLE library files (LBR) to include in the process. You can delete a selected file by clicking Remove.

A progress window will open and close quickly before the next page of the Wizard appears.

Reporting Options

Use the Reporting Options page to configure the reports manager.

Under General Settings, enable the desired options: Log All Errors, Log All Warnings, Log All Events.

Schematic Settings

Recognize powerports - enable to recognize schematic powerports. Ensure that the default values in the Power port designators textbox are correct. If not, enter correct designators directly in the textbox.
Recognize ports - enable to recognize standard ports. Ensure that the default values in the Port designators textbox are correct. If not, enter correct designators directly in the textbox.

If power ports in your EAGLE designs are named using the format P+?, then accepting the default setting for the recognition of standard ports (with Port designators set to PORT?;P+?) will result in those power ports being incorrectly translated as standard ports, leading to shorts in the circuitry. In such a case, change the Port designators setting to "PORT?".

Ignore document templates - enable to ignore any document templates.
Hide default sheet template - enable to hide the default sheet template.
Do not translate hidden net name - enable to not translate hidden net name(s).
Create bus entry - enable to create a bus entry.

Library Settings

Add libraries to PCB project if one exists - enable to add libraries to the project.

Executing Import Process

You have full control over where the generated Altium Designer project(s) and associated documents are to be located by specifying the Output Directory. Use the Browse Folder icon to search for and select the desired location for the output.

By default, the output directory will target the location of the original source EAGLE design/library files.

The proposed Output Structure is also displayed, so you can see exactly the files and structure tree that will be generated. If everything is correct, proceed with the import by clicking Next.

Executing Import Process

The Executing Import Process page displays the document that is currently being processed with a green bar to show the progress of the import.

Closing the Wizard

The EAGLE Import Wizard has completed. Click Finish to close the Wizard.

Imported EAGLE files:

The result of the import can be seen in the Projects panel and can be summarized as follows:

An Altium Designer PCB Project (*.PrjPcb) is created per EAGLE .sch, .pcb and .lbr involved in the import.
An EAGLE schematic design archive (*.sch) is imported into an Altium Designer Schematic document (*.SchDoc).
An EAGLE PCB design archive (*.pcb) is imported into an Altium Designer PCB document (*.PcbDoc).
An EAGLE library (*.lbr) is imported as Altium Designer Schematic (*.SchLib) and PCB (*.PcbLib) library documents. In addition, an integrated Library (*.IntLib) is compiled based on these source libraries.
A Log file (*.log) is generated for each imported file that shows the results of analysis on the original EAGLE file as well as any errors and warnings (if enabled for inclusion).

Mentor Expedition Designs and Libraries

Altium Designer can import binary format PCB and PCB Libraries that have been designed in Mentor Expedition.

The following summarizes the import functionality:

In Mentor Expedition, a PCB design or library does not exist as a single file, but rather, as a structure of interdependent folders and files. Altium Designer's importer requires the entire folder/file structure to be intact to successfully import a PCB or library.
To import a PCB design file, select the *.pcb file in the design structure's top level folder. To import a library file, select the *.lmc file in the library's top level folder.
The strategy for application of design rules is completely different between Altium Designer and Mentor Expedition. Because of this, Altium Designer's PCB design import process does not translate Mentor Expedition PCB design rules. Instead, all of the Mentor Expedition rule definitions are clearly enumerated in a section of the *.log file. The user can then examine this list and create appropriate rules in Altium Designer.
Problems during import are detailed in the *.log file report.

Importing Mentor Expedition Design Files

Click Add to choose which Mentor Expedition design files to include in the process. You can delete a selected file by clicking Remove.

Importing Mentor Expedition Library Files

Click Add to choose which Mentor Expedition library files (*.lmc) to include in the process. You can delete a selected file by clicking Remove.

Current User Layer Mappings

If desired, you can edit the layer mapping for any or all Mentor Expedition PCB designs or library files on this page of the Wizard. To group by a column, drag the column header into the area at the top of the table specified.

Menu
- Set Selection To - select to access a sub-menu of layer types from which you can choose the desired layer.
- Load Layer Mapping - select to open the Load Configuration dialog to load the desired mapping files.
- Save Layer Mapping - select to open the Choose File to Save Layer Mapping dialog and choose the path in which to save the layer mapping.

Right-clicking in the grid region gives access to the same menus and sub-menus as clicking the Menu button.

Since the Signal, Plane and Mask layers are automatically mapped into Altium Designer, they are not shown on this page of the Wizard.

Output Projects

Executing Import Process

On this page of the Wizard, a green progress bar shows the progress of the import process while also listing each file at the process continues.

Closing the Wizard

The Mentor Expedition Import Wizard has completed. Click Finish to close the Wizard.

Orcad Designs and Libraries Files

Importing Orcad Designs

Click Add to choose which OrCAD design files to include in the import process. You can delete a selected file by clicking Remove.

Importing Orcad Libraries

Click Add to choose which OrCAD library files to include in the import process. You can delete a selected file by clicking Remove.

Reporting Options

Use the Reporting Options page to set up general log reporting options.

Under General Settings, enable the desired options: Log All Errors, Log All Warnings, and Log All Events.

Schematics General Options

Use this page of the Wizard to control how OrCAD component rectangles are imported. Enable Convert Orcad Component Rectangles to Altium Designer Rectangles if desired.

Schematics Sheet Options

Use this page of the Wizard to control how OrCAD pages are imported.

Title Blocks - OrCAD title blocks are imported as schematic components. In Altium Designer, title blocks are limited to two types: Standard and ANSI, and the graphics for them are not editable. Templates can be used if you desire a more flexible solution. Templates allow any graphical data to be placed onto a schematic sheet.

Strip Orcad Title Blocks - enable to strip the OrCAD title blocks.
Enable AdvSCH Title Blocks - check to enable AdvSCH title blocks. Use the drop-down to select Standard or ANSI.

Pin-to-Pin Spacing

The OrCAD pin-to-pin spacing feature is currently not available in Altium Designer. Use the following options to specify the desired spacing ratio and sheet resizing.

Pin-to-Pin Spacing - enter the desired spacing ratio.
Resize Sheet - enable to resize the sheet based on the pin-to-pin spacing entered in the above textbox.

Schematics Parameter and Net Connectivity Options

Use this page of the Wizard to control how OrCAD properties and junctions are imported.

Properties - OrCAD properties are generally imported as schematic parameters, with the exception of wire properties, which are imported as texts.

Auto-position Parameters - enable to automatically place schematic parameters out of the way after rotation or other movements.
Disable "Mark Manual Parameters" - manually-positioned parameters will be marked with blue dots. Check this box to disable this feature.

Junctions - The two types of junctions in Altium Designer are manual and auto-junctions. Auto-junctions are automatically calculated depending on the design and they cannot be manually placed or removed. However, users can place and remove manual junctions and the system will not try to remove them, even if the design has changed.

Import Orcad Junctions - use the drop-down to select which junctions to import. Choices include: Only Cross Junctions and All.

Output Library Options

Use this page of the Wizard to control how the imported libraries are grouped.

Library Import Options - select one of the following options for how to group output libraries.

Output Libraries as PCB Project - select to minimize the integration between PCB and schematic libraries. The imported libraries will only be grouped as a PCB project. They can be added to the list of libraries in the library panel later. This setup is most advantageous for those who wish to operate in the same environment as they did in OrCAD.
Output Libraries as Library Packages - select to group the libraries into library packages. You can then select to compile the library packages as integrated libraries by enabling Compile as Integrated Libraries. Integrated libraries combine both PCB, schematic and PSpice libraries, enabling better interactions. Errors in the compilation are shown in the Messages panel.

Output PCB Projects

Each project can only contain one OrCAD DSN file.

Click Menu to access options to edit the project structure:

Create Project - click to open the Create Project dialog to add a project.

Use the Create Project dialog to add a new project.

Rename Project - click to rename the selected project. This option is available only when a *.PrjPcb file is selected.
Remove Selected Projects - click to remove the selected project from the PCB Projects structure.
Reset Structure to Default - click to reset the PCB Projects structure to the defaults.
Add Designs to Project - click to add a design(s) to the project. This option is available only when a *.PrjPcb file is selected.
Remove Selected Designs - click to remove the selected design files.

Right-clicking in the PCB Projects region gives access to the same menus and sub-menus as clicking the Menu button.

Output Libraries

The output directory for the imported libraries are shown on this page of the Wizard. Use the Browse Folder icon to search for and choose the desired Library Output Directory.

Executing Import Process

On this page of the Wizard, a green progress bar shows the progress of the import process while also listing each file at the process continues.

Closing the Wizard

The OrCAD Import Wizard has completed. The Messages panel appears with any relevant messages. Click Finish to close the Wizard. If any warnings were generated during the import process, a *.LOG file opens showing the warnings.

Imported OrCAD files translate as follows:

OrCAD Layout (*.MAX) files translate to Altium Designer PCB files (*.PcbDoc).
OrCAD Capture (*.DSN) files translate to Altium Designer schematic files. Each page within a .DSN file will be imported as a single Altium Designer schematic file (*.SchDoc). Design caches within a .DSN file will be imported as a schematic library (*.SchLib). Design hierarchy is maintained, including complex hierarchy.

OrCAD .OLB (schematic library) files will be translated into Altium Designer schematic library files (*.SchLib).
OrCAD .LLB (PCB library) files will be translated into Altium Designer PCB library files (*.PcbLib).
Translated OrCAD libraries are automatically grouped into one PCB project.

Orcad CIS Configuration Files and Libraries

Altium Designer currently only supports OrCAD CIS .DBC files in binary format.

Locating the Database

Use the Browse Folder icon to search for and select the location of your OrCAD database. Your database will be opened in a read-only state in order to validate the mappings between parameter names and tables/columns.

Locating Configuration Files

This page of the Wizard is used to specify the location of your CIS Config file. Use the Browse Folder icon to search for and select the CIS Config File. Use the Database Library Browse Folder icon to specify the location you want the database library document to be saved.

Locating OrCAD Libraries

Use this page of the Wizard to specify the OrCAD schematic and/or PCB libraries that are referenced by the database. The libraries will be converted into Altium Designer libraries and saved in the Destination Folder specified.

Click Add to open the Select Library Path dialog to select the desired library path.

Use the Select Library Path dialog to specify the desired path.

Library files found within the specified path will populate the Wizard page as shown below.

Click Remove to delete selected files. Click Clear to delete all files.

Click Finish to close the Wizard. The Database Library (*.DBLib) that was generated during the import process will open.

OrCAD CIS files translate as follows:

OrCAD OLB (schematic library) files will be translated into Altium Designer schematic library files (*.SchLib).
OrCAD LLB (PCB library) files will be translated into Altium Designer PCB library files (*.PcbLib).

PADS ASCII Design and Library Files

The PADS designs imported by the Wizard are captured as documents in individual PCB projects that are created automatically after the translation in Altium Designer. Errors in the translation are reported in a log file with the extension *.LOG.

The Wizard only translates PADS ASCII versions 5.2 and above and does not read PADS binary files. If you only have binary PADS files, you will need to export these binary files into ASCII format from your PADS application, preferably in the ASCII 2005.2 format.

Importing PADS Designs

Click Add to choose which PADS design files to include in the process. You can delete a selected file by clicking Remove.

Importing PADS Libraries

Click Add to choose which PADS library files to include in the process. You can delete a selected file by clicking Remove.

Reporting Options

Use the Reporting Options page to set up general log reporting options.

Under General Settings, enable the desired options: Log All Errors, Log All Warnings, and Log All Events.

Enable Do not translate hidden net names if desired.

Default Options

The Default Options page is used to set default options that pertain to both the PCB and PCB library import process.

Enable the options under Design Rules to specify which (if any) design rules to import.

Enable any desired Keep Out Options.

Specify the desired Plane Pullback Distance in the textbox. Enable the checkbox to Rebuild All Internal Planes.

Enable the checkboxes of any additional Options.

Default PCB Specific Options

This page of the Wizard is used to set default options that are specific to the PCB import process.

Click Edit Mapping to open the PADS PCB Library ASCII File Import Options dialog.

All used PADS PCB layers must be mapped to an Altium Designer layer prior to import. The PADS PCB Library ASCII File Import Options dialog allows the user to map PADS PCB layers to an Altium Designer layer. The dialog also gives access to the Importer Settings dialog in which the user can control design rules, missing vias and keep-out conversions during the import process.

Current PCB and PCB Library Options

Use this page of the Wizard to review the output project structure and specify the output directory in which to import PADS PCB and PCB library files. Use the Browse Folder icon to search for and choose the Project Output Directory.

Click Menu to access options to edit the project structure:

Create Project - click to open the Create Project dialog to add a project.

Use the Create Project dialog to add a new project.

Rename Project - click to rename the selected project. This option is available only when a *.PrjPcb file is selected.
Remove Selected Projects - click to remove the selected project from the PCB Projects structure.
Reset Structure to Default - click to reset the PCB Projects structure to the defaults.
Add Designs to Project - click to add a design(s) to the project. This option is available only when a *.PrjPcb file is selected.
Remove Selected Designs - click to remove the selected design files.

Right-clicking in the PCB Projects region gives access to the same menus and sub-menus as clicking the Menu button.

Output PCB Projects

Closing the Wizard

The PADS Import Wizard has completed. Click Finish to close the Wizard.

Imported PADS Files:

One Altium Designer schematic document is generated by the Wizard for each PADS Logic sheet within a logic file. Each translated logic file is grouped into automatically created Altium Designer PCB projects with an *.PrjPCB file extension.

Imported files translate as follows:

PADS ASCII Schematic Logic sheets within a Logic file with a *.TXT extension translate to Altium Designer schematic files with an *.SchDoc file extension.

Orcad and PADS Designs and Libraries Files

Many PADS users use a combination of PADS Layout for their PCB layout and OrCAD Capture for their schematic capture. This section assumes this combination.

All used PADS PCB layers must be mapped to an Altium Designer layer prior to import. There are additional options through the pages of the Wizard to control the automatic creation of design rules, missing vias and keep-out conversions.

It should be noted about how the layers are mapped on import for PCB designs. Layer Mapping is simply a mapping between the names of the PADS PCB layers and Altium Designer PCB layers. Of course you can change as many mappings as you want as only suggested default mappings are given. This mapping is used by the Import Wizard to build the layer mapping for each PCB that can then be individually customized. The rationale here is that should you wish to import ten PCB designs and you want to map the layer Assembly 1 to Mechanical Layer 1, you would not have to customize each of the ten PCB designs in order to get the right layer mapping.

The advantage to importing in this manner is that batch management of layer mapping can save a lot of time when importing multiple designs. In this instance, the default layer mapping will be saved to your Preferences. The disadvantage to using this is that Default Layer Mapping is not always intelligent with differing structures in designs, and so some manual changes may be needed afterwards.

Selecting the OrCAD and PADS Design Files

Use this page of the Wizard to add the OrCAD and PADS design files you want to import. Click Add to search for and select the desired files. Click Remove to delete a selected file.

Selecting the OrCAD and PADS Library Files

Use this page of the Wizard to add the OrCAD and PADS library files you want to import. Click Add to search for and select the desired files. Click Remove to delete a selected file.

Setting the Reporting Options

Use the Reporting Options page to set up general log reporting options.

Under General Settings, enable the desired options: Log All Errors, Log All Warnings, and Log All Events.

Setting the Schematic Options

Use this page of the Wizard to control how OrCAD DSN (design) and OLB (library) files are imported.

Enable Convert OrCAD Component Rectangles to Altium Designer Rectangles if desired.

Usually, OrCAD properties are imported as schematic parameters (with the exception of wire properties) and are imported as texts. Schematic parameters can be set to auto-position by enabling Auto-position Parameters, which will automatically place them out of the way after rotation or other movements. By default, manually-positioned parameters will be marked with blue dots. To disable this default, enable Disable "Mark Manual Parameters".

The OrCAD pin-to-pin spacing feature currently is not available in Altium Designer. Enter the desired spacing ratio in the Pin-to-Pin Spacing textbox. If you want to also resize the sheet based on the entered spacing, enable Resize Sheet.

Setting Schematic Sheet Options

Use this page of the Wizard to control how OrCAD pages and junctions are imported.

OrCAD title blocks are imported as schematic components. Altium Designer also supports this feature, however, the title blocks in Altium Designer are limited to two types: Standard and ANSI and their graphics are not editable. If this is not desirable for your situation, templates can be used to provide a more flexible solution. Templates allow any graphical data to be placed onto a schematic sheet. Enable Strip OrCAD Title Blocks to strip the OrCAD title blocks. Check Enable Schematic Title Blocks if desired, then use the drop-down to select Standard or ANSI.

There are two types of junctions in Altium Designer: manual and auto. Auto-junctions are automatically calculated depending on the design and they cannot be manually placed or removed by the user. Conversely, users can place and remove manual junctions and the system will not try to remove them even if the design has changed. Use the Import OrCAD Junctions drop-down to select Only Cross Junctions or All.

Setting PCB and PCB Library Default Options

Use this page of the Wizard to set default options that are common to both the PCB and PCB Library import process.

Enable Override Pad Inner Value With Largest Found to specify that imported pads will have their sizes on the mid-layers set to the largest size found.

Setting Options for PCB Import Process

Use this page of the Wizard to set default options that are specific to the PCB import process.

Enable any Design Rules you want to import: Import Clearance Rules, Import Routing Rules, and Import Routing Rules.

Enable any Keep-Out Options you want to import: Import Placement Keep-Outs As Rooms, Import Trace & Copper Keep-Outs As Cut-Out Regions, and Import Copper Pour & Plane Keep-Outs As Cut-Out Regions.

Enable any desired miscellaneous Options:

Add Missing Via On Route Layer Change
Generate Teardrops
Generate Rules For Thermals In Pad Stacks
Change Attributes For Used Layers

Specify the desired Plane Pullback Distance in the textbox. Enable the checkbox to Rebuild All Internal Planes.

PCB and PCB Library Options

This page of the Wizard is used to review and edit options for each PADS PCB and PCB Library. Any unmapped layers are highlighted in pink.

Click Edit Mapping to open the PADS PCB Library ASCII File Import Options dialog.

Setting Output Library Options

Use this page of the Wizard to control how the imported libraries are grouped.

Library Import Options - select one of the following options for how to group output libraries.

Output Libraries as PCB Project - select to minimize the integration between PCB and schematic libraries. The imported libraries will only be grouped as a PCB project. They can be added to the list of libraries in the library panel later. This setup is most advantageous for those who wish to operate in the same environment as they did in OrCAD.
Output Libraries as Library Packages - select to group the libraries into library packages. You can then select to compile the library packages as integrated libraries by enabling Compile as Integrated Libraries. Integrated libraries combine both PCB, schematic and PSpice libraries, enabling better interactions. Errors in the compilation are shown in the Messages panel.

Specifying the Output Directory

Click Menu to access options to edit the project structure:

Create Project - click to open the Create Project dialog to add a project.

Use the Create Project dialog to add a new project.

Rename Project - click to rename the selected project. This option is available only when a *.PrjPcb file is selected.
Remove Selected Projects - click to remove the selected project from the PCB Projects structure.
Reset Structure to Default - click to reset the PCB Projects structure to the defaults.
Add Designs to Project - click to add a design(s) to the project. This option is available only when a *.PrjPcb file is selected.
Remove Selected Designs - click to remove the selected design files.

Right-clicking in the PCB Projects region gives access to the same menus and sub-menus as clicking the Menu button.

Specifying the Output Library Directory

Use this page of the Wizard to review the output library structure and specify the output directory in which to import the library files. Use the Browse Folder icon to search for and choose the Library Output Directory.

Executing Import Process

This page show a green progress bar of the import process.

Closing the Wizard

The OrCAD and PADS Import Wizard has completed. The Messages panel appears with any relevant messages. Click Finish to close the Wizard. If any warnings were generated during the import process, a *.LOG file opens showing the warnings.

PADS and OrCAD files translate as follows:

PADS ASCII PCB Layout (*.ASC) files translate to Altium Designer PCB files (*.PcbDoc).
PADS ASCII PCB Library files translate into Altium Designer PCB library files (*.PcbLib).
OrCAD Capture (*.DSN) files translate to Altium Designer schematic files. Each page within a .DSN file will be imported as a single Altium Designer schematic file (*.SchDoc). Design caches within a .DSN file will be imported as a schematic library (*.SchLib). Design hierarchy is maintained, including complex hierarchy.
OrCAD schematic library (*.OLB) files will be translated into Altium Designer schematic library files (*.SchLib).
The files will be grouped into an Altium Designer PCB project (*.PrjPCB) that is automatically created.
Translated OrCAD libraries are automatically grouped into one PCB project.

P-CAD Designs and Libraries Files

Translating complete P-CAD designs, including schematics, PCB layout, and library files, can all be directly handled by the Import Wizard without first converting to ASCII - thus avoiding the need for having P-CAD installed. The Import Wizard removes many of the problems normally found with design translation by analyzing your files and offering many defaults and suggested settings for project structure, layer mapping, PCB pattern (footprint) naming, and more. Complete flexibility is found in all pages of the Wizard, giving you as little or as much control as you would like over the translation settings before committing to the actual translation process.

In P-CAD, all design work begins on the sheet, the logical working area of the design. There can be multiple schematic sheets within a single P-CAD schematic design file (*.SCH file). In Altium Designer, the logical design area begins with a document and for each document there is a file stored on the hard drive. This means that for each Altium Designer schematic document (sheet) there is a file - an important conceptual difference to remember.

In P-CAD, components form the basic building blocks of design in P-CAD and the symbol is merely a graphical representation of that component in the schematic. In Altium Designer, the symbol is effectively the component for all phases of design and not just the schematic capture portion of it. A little comparison will help show the differences of how the two are modeled between the respective systems for a better understanding.

Select the P-CAD Design Files to Import

Click Add to choose which P-CAD design files to include in the process. You can delete a selected file by clicking Remove.

Select the P-CAD Library Files to Import

Click Add to choose which P-CAD library files (LIB and LIA) to include in the process. You can delete a selected file by clicking Remove.

You can select what type of libraries to create using the Output Libraries As drop-down. Choices include:

Integrated Library
DBLib (Access Backend)
DBLib (CSV Backend)

A progress window will open and close quickly before the next page of the Wizard appears.

PCB Footprint Naming Format

P-CAD data structure is different than that of Altium Designer. On the PCB side, Altium Designer supports the concept of patterns, a pattern cannot be sub-classified into its pattern graphics in P-CAD. Additionally, pads in Altium Designer have only one designator, while in P-CAD where pad designators can come from the component pin designators or the pattern pad numbers.

Due to these differences, PCB footprint names can take many different forms. The PCB Footprint Naming Format page is used to specify the format of the PCB footprints.

Use the drop-downs to select the PCB Footprint Naming Format. The Extracted Sample Footprint Names region dynamically updates according to your selections.

Schematic Component Naming Format

Use this page of the Wizard to review the schematic naming transformations for your P-CAD components. The P-CAD concept of symbol drawings does not exist in Altium Designer. Information such as symbol drawings, attributes, parts, pin names, pin/pad linkages, and gate/pin equivalencies must reside in a schematic component. As a result of this, each P-CAD component will be imported as an Altium Designer schematic component, with the schematic component names set to the P-CAD component names.

Reporting Options

Use the Reporting Options page to set up general log reporting options.

Under General Settings, enable the desired options: Log All Errors, Log All Warnings, Log All Events.

P-CAD PCB component names will be transformed using the settings specified on the PCB Footprint Naming Format page, which may result in some differences. Enable Log warnings for footprint name changes in order to see these differences.

Enable Log warnings for skipped tokens to see warnings regarding P-CAD tokens that were ignored during the import process.

Enable Do not translate hidden net names if desired.

Current Layer Mappings

If desired, you can edit the layer mapping for any or all P-CAD PCBs on this page of the Wizard. Use the drop-downs to the right of each header to select. To group by a column, drag the column header into the area at the top of the table specified.

Menu
- Invert Selection -
- Set Selection To - select to access a sub-menu of layer types (listed below) with their own sub-menus of layers from which you can choose the desired layer:
  - Signal Layers
  - Plane Layers
  - Mechanical Layers
  - Other Layers
- Load Layer Mapping - select to open a dialog to load the desired mapping files.
- Save Layer Mapping - select to open a dialog and choose the path in which to save the layer mapping.

Right-clicking in the grid region gives access to the same menus and sub-menus as clicking the Menu button.

Output PCB Projects

Menu
- Create Project - click to open the Create Project dialog to add a project.

Use the Create Project dialog to add a new project.

Rename Project - click to rename the selected project. This option is available only when a *.PrjPcb file is selected.
Remove Selected Projects - click to remove the selected project from the PCB Projects structure.
Reset Structure to Default - click to reset the PCB Projects structure to the defaults.
Add Designs to Project - click to add a design(s) to the project. This option is available only when a *.PrjPcb file is selected.
Remove Selected Designs - click to remove the selected design files.

Right-clicking in the PCB Projects region gives access to the same menus and sub-menus as clicking the Menu button.

Output Integrated Libraries

The output directory for the imported libraries are shown on this page of the Wizard. Use the Browse Folder icon to search for and choose the desired directory.

Executing Import Process

On this page of the Wizard, a green progress bar shows the progress of the import process while also listing each file at the process continues.

Closing the Wizard

The P-CAD Import Wizard has completed. Click Finish to close the Wizard.

Imported P-CAD files:

P-CAD design files translate as follows:

P-CAD PCB (*.PCB) files translate into Altium Designer PCB files (*.PcbDoc).
P-CAD schematic (*.SCH) files translate into Altium Designer schematic files (*.SchDoc). Each sheet within a P-CAD schematic file is imported as a single Altium Designer schematic file (*.SchDoc). Design hierarchy is maintained including complex hierarchy.
The files will be grouped into an Altium Designer PCB project (*.PrjPCB) that is automatically created.
P-CAD PCB files generate an output job document (*.OutJob) if necessary. This document will contain all the print settings from the P-CAD PCB.

P-CAD library (*.LIB and *.LIA) files translate as follows:

Libraries that contain only pattern information translate into Altium Designer PCB library files (*.PcbLib).
Libraries that contain both pattern and symbol information translate into both Altium Designer PCB library files (*.PcbLib) and schematic library files (*.SchLib).
Libraries that contain both component and symbol information translate into Altium Designer schematic library files (*.SchLib).

Libraries that contain only symbol information do not import as Altium Designer does not have the same concept of a symbol as P-CAD.

Translated P-CAD libraries are automatically grouped in an integrated library package (*.LibPkg).

Zuken CR5000 Design Files

The Zuken CR-5000 Importer requires ASCII files so you will need to convert your Zuken CR-5000 binary files to ASCII before using the Import Wizard.

Converting Zuken binary files to ASCII format requires a special license from Zuken.

Use the following steps to convert your Zuken CR-5000 binary PCB database files to ASCII files:

Convert the binary file <basename>.ftp into an ASCII file: In the cdb directory, extract <basename>.ftf using the DOS (or command script) command: ftout.exe<basename>. For example C:\cr5000\bin\ftout.exe basename.
Convert the binary file <jobname>.pcb into an ASCII file: In the pcb directory, extract <jobname>.pcf using the DOS (or command script) command: pcout.exe<jobname>. For example: C:\cr5000\bin\pcout.exe jobname.

To convert the Zuken CR-5000 schematic binary file (*.sht) to ASCII format (*.eds), run the Zuken editWriter.exe utility. This opens a GUI for creating the ASCII format file.

The Zuken CR-5000 Importer requires two ASCII files to import a Zuken CR-5000 PCB design and an ASCII schematic file to import a schematic:

An ASCII layout file which contains placement and layer symbols, layer count, units, etc. (*.pcf)
An ASCII representation of the footprints used in the design (library) (*.ftf)
An ASCII representation of the schematic (*.eds)

Please note that if you import a PCB (.pcf) file and do not import a footprint library, or the footprint library does not provide any information about a pad, it will be imported as a through-hole with a default size and shape. Similarly, vias will not be imported correctly as well.

Select the Zuken CR-5000 Files to Import

Click Add to choose which Zuken design files to include in the process. You can delete a selected file by clicking Remove.

Select Footprint Libraries to Import

Click Add to choose which Zuken library files (*.FTF) to include in the process. You can delete a selected file by clicking Remove.

Setting the General Options

Use the General Options page to set up general log reporting options.

Under General Settings, enable the desired options: Log All Errors, Log All Warnings, and Log All Events.

Log of Analyzing

The Log of Analyzing page lists any errors/warnings found during the scanning of the Zuken files you are importing.

General Import Options

Use this page of the Wizard to review the output project structure and specify the Output Directory in which to import the files. Use the Browse Folder icon to search for and choose the Output Directory.

Setting the Schematic Import Options

This page of the Wizard is used to set the import options for your schematic. Enable the desired options.

You can edit the Power Ports names and Probes names textboxes, ensuring that each item is separated by a semi-colon.

Setting the PCB Import Options

Use this page of the Wizard to set the import options for your PCB.

You can edit Testpoint names in the textbox, ensuring that each item is separated by a semi-colon. Use the Font drop-down to select the desired font.

Current Board Layer Mapping

This page of the Wizard shows the board layer mapping. Information displayed includes Sort Key, Zuken Layer, and its associated Altium Designer Layer. Pink highlighting in the Altium Designer Layer denotes that the corresponding Zuken Layer will not be imported.

If desired, you can edit the layer mapping for any or all layers. You can rearrange the columns by dragging a column header into the desired position. Click on the header of any column to access

then click to sort that column in ascending or descending order, respectively.

When you hover over the column heading, a filter icon (

) appears. Click to open a drop-down from where you can select your filter choices for that column. Choices include:

(All) - click to display all items in that column.
(Custom) - click to open the Custom AutoFilter dialog in which you can specify a custom filter for that column.

(Blanks) - click to display only items that are blank in that column.
(Non blanks) - click to display only items that are not blank in that column.

Current Footprints Layer Mapping

This page of the Wizard shows the footprints layer mapping. Information displayed includes Sort Key, Zuken Layer, and its associated Altium Designer Layer. Pink highlighting in the Altium Designer Layer denotes that the corresponding Zuken Layer will not be imported.

If desired, you can edit the layer mapping for any or all layers. You can rearrange the columns by dragging a column header into the desired position. Click on the header of any column to access

then click to sort that column in ascending or descending order, respectively.

When you hover over the column heading, a filter icon (

) appears. Click to open a drop-down from where you can select your filter choices for that column. Choices include:

(All) - click to display all items in that column.
(Custom) - click to open the Custom AutoFilter dialog in which you can specify a custom filter for that column.
(Blanks) - click to display only items that are blank in that column.
(Non blanks) - click to display only items that are not blank in that column.

Importing Progress

On this page of the Wizard, a green progress bar shows the progress of the import process while also listing each file at the process continues.

Closing the Wizard

The Zuken CR5000 Import Wizard has completed. The Messages panel appears with any relevant messages. Click Finish to close the Wizard.

The files will be grouped into an Altium Designer PCB project (*.PrjPcb) that is automatically created and available in the Projects panel.

Zuken CR5000 files translate as follows:

Zuken CR5000 ASCII PCB Layout (*.pcf) files translate to Altium Designer PCB files (*.PcbDoc).
Zuken CR5000 ASCII representation of the footprints files (*.ftf) translate into Altium Designer PCB library files (*.PcbLib).
Zuken CR5000 ASCII representation of the schematic files (*.eds) translate to Altium Designer schematic files (*.SchDoc) and schematic library files (*.SchLib).
If any warnings were generated during the import process, a *.LOG file is created showing the warnings.

适合打印版本

If you find an issue, select the text/image and pressCtrl + Enterto send us your feedback.

EDAImporter_Dlg-ImporterManagerFormImport Wizard_AD

Using the Import Wizard

Wizard Navigation

Selecting the Type of Files to Import

99SE DDB Files

Allegro Design Files

CADSTAR Designs and Libraries

CircuitMaker 2000 Schematics and Libraries Files

DxDesigner Designs and Libraries Files

EAGLE Projects and Designs

Mentor Expedition Designs and Libraries

Orcad Designs and Libraries Files

Orcad CIS Configuration Files and Libraries

PADS ASCII Design and Library Files

Orcad and PADS Designs and Libraries Files

P-CAD Designs and Libraries Files

Zuken CR5000 Design Files

Was this page helpful?