What's Good About Allegro PCB Editor Dual-Side Contact Components…
PCB Design Blogs
15 Jul 2014
Get email delivery of the Cadence blog featured here
All Blog Categories
Cadence Academic Network
Cadence on the Beat
Custom IC Design
IC Packaging and SiP Design
The India Circuit
Insights on Culture
Signal and Power Integrity (PCB/IC Packaging)
System Design and Verification
Tensilica, Design, and Verification IP
The Design Chronicles
What's Good About Allegro PCB Editor Dual-Side Contact Components? It’s in the 16.6 Release!
The use of dual-sided contact components when placed on internal layers of the PCB allows connections to be made from either side of the device. One of the benefits of using this emerging technology is the reduction of core vias that may have been used to make connections from the component to either side of the PCB. Symbols targeted for dual-side applications must have the property ‘dual_sided_component’ applied in the
Allegro Symbol Editor
. The associated padstacks of the symbol must have a ‘begin’ and ‘end’ layer pad defined.
When the symbol with the dual-sided property is placed, the ‘begin’ pad defined in the padstack definition is mapped to the inner layer upon which the component is placed. The alternate pad, defined as the ‘end’ pad at the definition level, is mapped to the layer closest to the top of the component based on the component height.
Existing Allegro embedded setup methodologies are fully supported; direct or indirect attach as well as body up/down. Since the stackup is unlikely to be constructed with material thickness that aligns with the component height, it’s likely the indirect attach method is used for this technology.
Read on for more details …
There are two prerequisites required at the symbol definition level -
1. Add the property ‘dual_sided_component’ to the symbol definition
2. The associative padstack must have a ‘BEGIN’ and ‘END’ pad defined
The property assignment must be made in the ‘Symbol Editor’, not the ‘PCB Editor’. When in the ‘Symbol Editor’, the property is applied to the ‘drawing’ as shown below:
As an example, consider changing the embedded layer setup (using the Setup > Embedded layer setup form) for SIGNAL_4 to the values specified below for “Embedded Status” and “Attach Method”:
In the “Placement Application mode” Options Panel you should see components in the placement list. The letter ‘E’ indicates the component has been assigned the ‘Embedded_Placement’ property and the green background indicates the property value is set to ‘Required’:
When you place the components, you’ll note the following -
You will not be allowed to place these components on the outer layers as a result of the components having the ‘dual_sided_component’ property applied
When initially moving any of the resistors from the placement list, they will automatically drop to the embedded layer (SIGNAL_4). There is no RMB action necessary when the component has a ‘required’ property value and there is only one embedded layer identified in the stackup.
The component pads are suppressed when using ‘Indirect Attach’ method
You should see 2 indirect symbol vias on SIGNAL_4
Disable the visibility of layer Signal_4, The alternate side of the component is based on its symbol height value. Based on the height of the symbol and thickness of the dielectric, via pads in this case will appear on SIGNAL 3:
Invoke ‘Add Connect’ then adjust option in panel to ‘WL’ (Working Layer):
Use the ‘3-D viewer’ to display your routed design. Enable the visibility of the place-bound shapes for all subclasses (top, bottom, embedded):
Please share your experiences using this capability.
PCB Layout and routing
Allegro PCB Editor
Share Your Comment
Post (Login required)