Importing a Design from xDX Designer or DxDesigner into Altium Designer

xDX Designer Schematic and Library Import Support

Support for the transfer of binary format designs captured using Siemens EDA^® Xpedition^® xDX Designer^® (formerly DxDesigner^®), to Altium Designer, is available courtesy of the latter's Import Wizard. Essentially formed from the separation of the binary importer from the existing ASCII importer (which remains unchanged), not only has the binary importer interface been upgraded to support data transfer from the latest version of xDX Designer, a wider range of object types are also now supported.

The xDX Designer design and library file importer is available through Altium Designer's Import Wizard (File » Import Wizard) by selecting the Mentor xDxDesigner Designs and Libraries option on the Wizard's Select Type of Files to Import page.

Select Mentor xDxDesigner Designs and Libraries in the Import Wizard to import xDX Designer files.

Version Support

The Importer has been updated for, and tested against, version 7.9.4 of xDX Designer (Expedition Enterprise 7.9.4, or simply EE7.9.4).

Supported Object Types

The following xDX Designer object types are supported when importing a design into Altium Designer:

• Arc
• Bus
• Circle
• Component Custom Parameter
• Component Geometry
• Component Pin
• Line
• Multi-Part Component (package)
• Multi-Sheet Document
• Offsheet Symbol
• Polygon
• Port and Power Port (existing as components)
• Rectangle
• Sheet Custom Parameter
• Sheet Symbol
• Sheet Template (stamp)
• Text Label
• Wire (with caption)

Notes for xDX Designer Import

DxDesigner Schematic and Library Import Support

Translating complete Siemens EDA DxDesigner designs, including schematics and library files can all be directly imported by having Altium Designer's Import Wizard without having to convert to an intermediary format - thus avoiding the need for having DxDesigner installed. Such files will be converted into Altium Designer schematic documents (*.SchDoc) - one schematic document per sheet defined within the Logic file - and added to a PCB project (*.PrjPcb).

The Import Wizard (File » Import Wizard) removes much of the headache normally found with design translation by analyzing your files and offering many defaults and suggested settings such as project folders, project links to other libraries, drawing styles, and output project structure. 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. Select the DxDesigner Designs and Libraries Files option on the Wizard's Select Type of Files to Import page.

Select DxDesigner Designs and Libraries Files in the Import Wizard to import DxDesigner files.

Using the Import Wizard for DxDesigner Designs

You can drag and drop your designs directly from Windows Explorer project folders into the designs and libraries page of the Import Wizard.

You can use the Import Wizard whether using DxDesigner schematic files by themselves or in combination with a PADS Layout PCB. Because there is a difference in the way that project files and schematic files are named and organized between DxDesigner and Altium Designer, it's worth briefly reviewing this so that you understand exactly how your schematic design and libraries files will be translated after the import process.

DxDesigner manages the design project based on a user-defined directory path, and everything in the system uses this project path as the initial point of reference. For example, instead of using file extensions for a file's type, a folder called sch in the project path indicates that files under this folder are schematic files. The individual schematic files follow the naming convention of Name.N where N is a numeric number. An example of this would be schematic_design.1. DxDesigner identifies this as a schematic file only because it is in the specified project path and under the folder called sch. Likewise, a folder called sym in this project path indicates it is a symbol folder, and that all files under it are assumed to be the equivalent library files (also following the same naming convention as schematic files).

Altium Designer uses specific file extensions for certain file types such as schematic design files, library files and project files. As you begin to import your DxDesigner files using the Import Wizard, you will be asked for your project directory name. The Import Wizard knows to look for the sch and sym folders inside the specified project path. If that directory does not exist, you will be given a warning message.

Schematic Design File Translation

DxDesigner project paths and schematic files in the Import Wizard 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. Once the schematics have been opened, the schematic hierarchy will be shown.

Translated design files are displayed immediately after translation in the Projects panel.

Schematic Design Object Translation

Most component attributes are translated into parameters with a few exceptions:

• Power Objects - DxDesigner symbols that contain a NETNAME attribute are identified as and translated into power objects in Altium Designer.
• Ports - similar to power objects, a symbol with an attached attribute represents it as a port. DxDesigner symbols that contain an IN, OUT, or BI attribute are identified and translated into Input, Output, or Bidirectional ports respectively.
• Signal - symbols that contain a SIGNAL attribute are identified as and translated into hidden power pins.
• Reference Designator - the REFDES attribute attached in the DxDesigner symbol usually has the format of: REFDES = R? When it is placed into a sheet, the user will specify the REFDES of the component in the sheet i.e. REFDES = R21.

Other common design objects translate as follows:

• DxDesigner wire segments and busses translate to wires and busses respectively.
• A wire or bus segment in DxDesigner can have a label attached to it. This is translated into a net label. Net label strings in DxDesigner with the following format D[0:8] are replaced with the following format D[0..8].
• Composite symbol types are identified and translated as Altium Designer sheet symbols. The symbol pin is translated as sheet entries and the sheet symbol file name will point to the list of schematic sheets that matches the symbol file prefix.

Schematic Library File Translation

DxDesigner symbol library files translate as follows: symbol files (Name.N) translate to Altium Designer library files (*.SchLib). Each symbol file will be imported into a single Altium Designer library file. Once translated, files are grouped into the Altium Designer PCB project (*.PrjPCB) that is automatically created.

Schematic Symbol Translation

Component Name - the following table describes how the DxDesigner symbol translates to the Altium Designer component:

Pin Type - the following table maps the PINTYPE attribute from DxDesigner to Altium Designer:

• Graphical Objects - most objects have a direct translation from DXDesigner to Altium Designer. Boxes (as defined as lower left and upper right corners) translate to four-point polygons.

• Multiple-part symbols - the PARTS attribute attached to the symbol indicates the number of parts this symbol represents and translates to the number sub-parts in Altium Designer.

• Annotate Symbol Type - DxDesigner categorizes the symbol into four types: composite, pin, annotate, and module. The most common use of symbols in DxDesigner is for sheet borders and graphical annotation. Because of this reason, such symbols are translated in Altium Designer components with a TYPE = Graphical.

• Heterogeneous Symbols - heterogeneous symbols in DxDesigner are any group of symbols that have the same HETERO attribute. When symbols are grouped under one HETERO type, they represent one device. Altium Designer translates these symbols to multiple parts or display modes under one component depending on the heterogeneous type. There are three distinct types:

  • HETERO TYPE 1- different components within the same device. The Altium Designer attribute assigned to this type follows the format: HETERO = sym1, sym2, [sym3].

  • HETERO TYPE 2 - different gates within the same device. The Altium Designer attribute assigned to this type follows the format: HETERO = sym, (symP) where P = PARTS number.

  • HETERO TYPE 3 - this is a split IC. The Altium Designer attribute assigned to this type follows the format: HETERO = (icsymname), (icsymname). The main difference between this type and HETERO TYPE 1 is only the context used by DxDesigner related to ICs.

Working with Documents in Altium Designer

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 sheet (page) there is a file. There can also be multiple design documents of varying types, depending on the nature of the design you are working on. Getting started, most DxDesigner users will be interested in the schematic and PCB document types as these are the files that their designs will be translated to.

Basic file operations: new PCB and schematic document types can be easily created via File » New, or by right-clicking on the project in the Projects panel.

The Schematic Symbol is the Part

In DxDesigner, a symbol block type is the logical entity that is described graphically by attributes, pins and various properties. As block types are placed in a schematic design, DxDesigner maintains the identity of the part for back annotation, net listing, bills of materials, and so forth. At the very minimum, a part requires a part name, a part reference prefix, and a name of a PCB footprint.

In Altium Designer, the logical symbol is assumed to be the essential starting point of a component. It can be initially defined at minimum as a name in a schematic library to which pins and any graphical symbols or alternative display options needed for implementation may be added. This flexibility allows a component to be represented in different ways during the design and capture process. This may not only be as a logical symbol on the schematic, but also be a footprint on the PCB or even as a SPICE definition for simulation.