Home > Community > Blogs > PCB Design > what s good about rf pcb and ads via exchange 16 6 has many new enhancements
Login with a Cadence account.
Not a member yet?
Create a permanent login account to make interactions with Cadence more conveniennt.

Register | Membership benefits
Get email delivery of the PCB Design blog (individual posts).


* Required Fields

Recipients email * (separate multiple addresses with commas)

Your name *

Your email *

Message *

Contact Us

* Required Fields
First Name *

Last Name *

Email *

Company / Institution *

Comments: *

What's Good About RF PCB and Agilent ADS Via Exchange? 16.6 Has Many New Enhancements!

Comments(7)Filed under: PCB Layout and routing, PCB design, SPB, Allegro PCB Editor, Allegro, via, RF, PCB Editor, PCB, layer stacks, layout, design, vias, via patterns, Allegro GUI, Grzenia, Allegro 16.6, 16.6, RF PCB, 16.6 routing, via exchange, Agilent, ADS, Agilent ADS

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


By Simon Mejia on January 29, 2014
hi Jerry,  i am looking into importing IFF files from ADS rf designer into Allegro pcb editor.  Reading your document "What's Good About RF PCB and Agilent ADS via Exchange?...  i noticed that i am missing the RF PCB feature in my tool.  Is this an additional feature which it made not be included into my current version?  this is what i currently have for Allgero PCB Designer XL (Legacy) 16.6  thank you for yout time, i am currently trying to undersand this interactiong between ADS and Allegro (a new process for me).  Your feedback is greatly appreciated.  thank you

By Jerry GenPart on January 29, 2014
Hi Simon,
Yes - I do believe that the RF PCB options are available through a separate license feature. You can contact you Cadence Sales team to discuss this.
Jerry G.

By Simon Mejia on January 31, 2014
Hi Jeff, thank you much.   Just to confirm, Allegro has the IFF import feature and just wondering that in order to import the ADS IFF file into Allegro, do i need to have the RF PCB option available in allegro?  

By Jerry GenPart on February 3, 2014
Hi Simon,
I stand corrected. I confirmed with one of our Allegro PCB Editor Support AE experts that - you can import IFF files without the RF PCB Option - use:
File - Import - IFF
Jerry G.

By Simon Mejia on February 3, 2014
Thank you Jeff,  I have tried importing the IFF file that was generated by ADS tool that the RF engineer designed.  As I tried importing it into PCB Allegro, i am not able to see it when i place it.  This is one resaon I was asking the questions about the need to have RF PCB option.  I will look into it more, maybe my settings in allegro are no properly set (?).  Thank you for you answers, now I need to go and try it again.  If I am successful, I will add additional comments just for information.  Thank you.

By Simon Mejia on February 4, 2014
Hi Jerry,  FYI, i was able to import an IFF file generated by ADS RF Designer.  This time, the designer generated an export file and the setting he used was cadence/pcb instead of just exporting IFF file of the design.  So this worked out well for me.  Again, thank you for looking into my comments. :)

By Jerry GenPart on February 4, 2014
Glad it worked out Simon!

Leave a Comment

E-mail (will not be published)
 I have read and agree to the Terms of use and Community Guidelines.
Community Guidelines
The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.