Importing and Using Allegro DFI Files into ADS

This chapter discusses how to import and use the files created with Allegro Design Flow Integration in ADS.

Importing Allegro DFI files in ADS Using the Import_Allegro Design Kit

Importing exported files from Allegro Design Flow Integration in ADS has been simplified through the introduction of the Import_Allegro Design Kit version 1.5 .

This Design Kit can be downloaded from the Agilent Knowledge Center, select EEsof Knowledge Center > Examples > Support Examples > ADS > Layout

Import_Allegro Design Kit for the Allegro Design Flow Integration
To install the design kit, or for more information about ADS design kits, refer to the Design Kit Installation and Setup] manual.

Using the Import_Allegro Design Kit

To import the exported Allegro files using Import_Allegro Design Kit do the follwing:

1. Open a new ADS layout window, select Allegro Tools > Import Allegro Layout .
   
2. This opens a file browser window. Go to the export directory and select the < boardfile >. ads, click OK .
   !allegrolink-3-1-02.gif!

This opens an Allegro importstatus window, as shown in Status Window. Click OK to dismiss the dialog and load the board.

Status Window

This loads the exported EGS layout, the Momentum substrate definition and the exported ports and associated pins, as shown in Importing and Using Allegro DFI Files into ADS#1115899.

All pins are Momentum internal or ground reference pins. The internal pins have the port number of the port on the Allegro side. The pin/port numbers above the highest exported port number are the Negative Reference pins (these are ground reference pins in ADS).
Two properties are attached to each imported ADS pin:

• allegro_pin : This provides the component instance.package pin number.
• allegro_net : The provides the name of the Allegro net.

Importing Allegro DFI Files Using ADS Import

This section discusses how to import the files created with Allegro DFI into ADS.

1. Start ADS and create a new project.
2. Open a new Layout window.
   
3. From the Layout windows main menu select File > Import . This opens the Import dialog.
   
   Select EGS Archive Format from the File Type dropdown list on the Import dialog and use the Browse button to select the layout file created in Allegro.

   Note The filename will be the same as the board name with the extention _a, and no suffix (e.g., cds_routed1_a).

4. Click OK to import the file into ADS.
   A Status window will open indicating a successful translation has occurred.
   
5. Click OK to dismiss this dialog. The imported design is now available in the ADS Layout window.
   
6. From the ADS Layout window's main menu select Momentum > Substrate > Open...
7. This opens the Open Substrate dialog. Select No to "Open a supplied substrate?"
   
   A dialog will open enabling you to choose a substrate file as seen in Open Substrate Dialog.

Open Substrate Dialog

1. Select the substrate file and click OK .

   Note The filename will be the same as the board name with the extension .slm (e.g., cds_routed1.slm).

2. If the substrate opens successfully, an Information Message dialog will open. Click OK to dismiss this dialog.
   

Verification

The following steps can be used to verify that the file information exported from the Allegro Design Flow Integration tool was successfully imported into ADS.
For this example, the substrate file contains the following board layers:

• ETCH_TOP
• ETCH_BOTTOM
• ETCH_GND
• DRILL_THROUGH

  Note For more information on selecting layers in Allegro, refer to Using the Layer Select Tab.

1. For this example, to view the Etch/Top layer select ETCH_TOP in the Layers dialog and de-select the other layers associated with the imported design.
   
   The ETCH_TOP layer should now be visible in the Layout window.
   
2. To view the Etch/Bottom layer, select ETCH_BOTTOM in the Layers dialog and de-select the other layers associated with the imported design.
   
   The ETCH_Bottom layer should now be visible in the Layout window.
   
3. To view the Etch/Gnd with Drill_Through layers, select the ETCH_GND and DRILL_THROUGH in the Layers dialog and de-select the other layers associated with the imported design.
   
   The ETCH_GND with Drill_Through layers should now be visible in the Layout window.
   
4. To check the layers information imported from Allegro, select Momentum > Substrate > Create/Modify... from the ADS Layout windows main menu.
   
   This brings up the Create/Modify Substrate dialog with the imported information. The Substrate Layers information is shown below.
   
5. To view the layer mapping information imported from Allegro, select the Layout Layers tab in the Create/Modify... Substrate dialog window.
   
   Before a physical simulaiton can be run, you still need to define the ports and the frequency plan from within the ADS framework. For more information on defining ports and setting up a frequency plan, refer to the ADS "Momentum" ] manual.