Get email delivery of the Cadence blog featured here
The 16.6 Allegro PCB Editor and the Agilent Advanced Design System (ADS) interface have several new enhancements with respect to padstacks and vias.I will cover the Allegro generic via padstack that exports to ADS, and also the enhancements for existing layout IFF interface (import and export) to support the generic via exchange.
Layer-to-layer via structures are almost always used in PCB designs. These common structures are not standardized in ADS -- they are represented in several ways. These include instances of via models such as the microstrip VIA2 and as layout-only footprints that define the catch pads and drill holes with simple polygons.
The disconnection between the capabilities of PCB tool via structures, and the equivalent objects in ADS, makes design transfer difficult. A PCB tool via structure must be flattened to simple polygons for transfer to ADS, losing most of the information contained in the original PCB via. Likewise, those simple polygons can be transferred back to the PCB tool, but are not identified as a via structure and not treated as a layer-to-layer connection. ADS does not have the PCB compatible via library, which means there is no padstack definition for a generic PCB via.
To solve the problem, Cadence and Agilent developed a solution -- you can export Allegro generic via padstacks first from the PCB Editor, and then ADS will build a PCB-style via library with the pcbViaLib utility offered in ADS2011.10. Agilent has provided the pcbViaLib design kit, which provides via import utilities and a new ADS component, the pcbVia. This design kit defines a data file format that holds the definition of a PCB-tool style via structure, which is read by the pcbVia component and used with a layout macro to render exactly the same layout footprint in ADS as in the PCB tool.When you export an Allegro layout design with generic vias to ADS by IFF, you can select export vias as components so all generic vias will be mapped to ADS via components. You can also use the via components in ADS layout and then export the ADS design with the kind of via components by IFF. When importing the design into PCB Editor by IFF, the I/F will automatically map back the ADS via components to Allegro generic via padstacks.Here is the flow for via management between Allegro PCB Editor and ADS: Read on for more details …
Export Allegro Generic Via Padstacks to ADS
There is a utility under the RF-PCB to export generic vias for ADS via component creation. You can click RF-PCB > Export Padstacks to ADS:
All vias used in the design will be listed and then you can select some/all vias to export. Please notice only vias in the layout will be listed on the form, so if you want to export a via padstack, you have to place the via into a design. The via group name is for ADS usage. Once you create the via components on the ADS side, you can place a via component in ADS layout from the specific via group.Note: It’s best to use a unique group name for each design so that ADS will not get confused. The exporting for via padstacks is not based on IFF format but AEL.
Constructing ADS Via Components
You can only get the required utility in ADS2011.10 or later. If you installed the specific design kit (you need to ask for it from Agilent), you will see this menu in ADS layout:
In ADS layout, click PCB Via Utilities > Import Via/Padstack Group… Browse to the proper .ael file exported from Allegro PCB Editor, then you will create the via components:
Export Allegro Design with Generic Vias to ADS by IFF
For a design with generic vias in PCB Editor like the following:
Click RF-PCB > IFF Interface > Export… to get the following dialog:
You can click the More options button, then you can see the Vias tab. Two options are available for via transfer mode. By default, all vias will be considered as components to export. You can still change it to Shape for the exporting as before. You can also RMB click on the header bar to select Change all to components as below:
If you export all vias as components, then all selected generic vias will be written out as via components in IFF file so that ADS can recognize them.
Import Layout IFF with Mapped Via Components into ADS
Make a new workspace in ADS and make sure the PCBVIALIB design kit is in current workspace. To import the design into ADS via IFF, click File > Import… in ADS layout, and then select the Cadence/PCB option, and browse the proper folder for the source files:
You will get the ADS layout will all generic vias converted into ADS via components:
If you double click a via in ADS layout, you will see the details for the via component:
Use Via Components in ADS
Once the via components created in ADS, you can export a layout design with generic vias from Allegro PCB Editor and then import the design into ADS by IFF. The Allegro generic vias can be replaced by ADS via components. Also you may directly use those via components in ADS side. Before you add a via component into the design, you need to know which vias are available. You can click PCB Via Utilities > List Via Groups, all available via names and via groups will be listed:
To add a via component into ADS layout, you can directly enter pcbVia at the following field:
The following dialog will appear:
You may need to change the viaGroupName and viaName and also padTypes. You can get the viaGroupName and viaName by clicking PCB Via Utilities > List Via Groups. For padTypes, you need to manually specify the value.
The meaning of the padTypes is to specify the pad usage on each layer. On each layer there will be a figure (range: 0-7) to indicate the pad usage on the layer. For example, 2 means the pad on this layer is for anti-pad usage. 4 means the pad on this layer is used as regular pad.The details of the definition for the padTypes are as following:
So when you use the via components in ADS, you need to know the layer number of the original via in Allegro design (when you export the padstack from Allegro).
Export Layout IFF with Via Components from ADS
Export a design from ADS layout by click File >Export…, and select the Cadence/PCB option form drop-down list:
Import IFF with Via Components into Allegro
In PCB Editor, click RF-PCB > IFF Interface > Import…, browse to the proper layout.iff file:
All via components in the IFF file will be mapped back to Allegro generic vias:
I look forward to your comments!Jerry "GenPart" Grzenia