Cadence® system design and verification solutions, integrated under our System Development Suite, provide the simulation, acceleration, emulation, and management capabilities.
System Development Suite Related Products A-Z
Cadence® digital design and signoff solutions provide a fast path to design closure and better predictability, helping you meet your power, performance, and area (PPA) targets.
Full-Flow Digital Solution Related Products A-Z
Cadence® custom, analog, and RF design solutions can help you save time by automating many routine tasks, from block-level and mixed-signal simulation to routing and library characterization.
Overview Related Products A-Z
Driving efficiency and accuracy in advanced packaging, system planning, and multi-fabric interoperability, Cadence® package implementation products deliver the automation and accuracy.
Cadence® PCB design solutions enable shorter, more predictable design cycles with greater integration of component design and system-level simulation for a constraint-driven flow.
An open IP platform for you to customize your app-driven SoC design.
Comprehensive solutions and methodologies.
Helping you meet your broader business goals.
A global customer support infrastructure with around-the-clock help.
24/7 Support - Cadence Online Support
Locate the latest software updates, service request, technical documentation, solutions and more in your personalized environment.
Cadence offers various software services for download. This page describes our offerings, including the Allegro FREE Physical Viewer.
Get the most out of your investment in Cadence technologies through a wide range of training offerings.
This course combines our Allegro PCB Editor Basic Techniques, followed by Allegro PCB Editor Intermediate Techniques.
Virtuoso Analog Design Environment Verifier 16.7
Learn learn to perform requirements-driven analog verification using the Virtuoso ADE Verifier tool.
Exchange ideas, news, technical information, and best practices.
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.
It's not all about the technlogy. Here we exchange ideas on the Cadence Academic Network and other subjects of general interest.
Cadence is a leading provider of system design tools, software, IP, and services.
Coplaner waveguides (CPW) are widely used in packaging, high speed designs and on silicon. These structures are now supported in Allegro PCB SI.
The figure below shows a typical coplaner waveguide. The important distinction for a segment to be a coplaner waveguide is a segment "W" surrounded by two large shapes. In order to detect coplaner waveguide segments while traversing a net, there needs to be a Shape window. The existing Geometry Window is used as the shape window. For a given segment, if two shapes adjacent to the segment exist within the Geometry Window, that segment will be analyzed as a CPW structure.
CPW Detection Flow
Global Setting to enable CPW
The InterconnectModels tab of the Signal Analysis Preferences form has been enhanced to add an option to enable/disable CPW.
One or both of the fields Enable CPW Extraction and EMS2D can be selected at a time. The effects on the field solver are as follows:
Only Enable CPW Extraction enabled:
With only this option enabled, the extraction code goes through a flow different from the regular (old) flow and tries to detect coplanar waveguides. The model generated is then passed to EMS2D to get a solution. Except for CPW, all other models are generated with BEM2D.
Only Field Solver EMS2D enabled:
With EMS2D enabled, the extraction code follows the normal (old) flow. The only difference is that instead of calling BEM2D to get the field solutions, the EMS2D field solver is called.
Both Enable CPW Extraction and EMS2D enabled:
With both options enabled, the extraction code uses the new flow, which tries to detect CPWs. All models are solved with the EMS2D field solver instead of BEM2D.
The Preferences button is only active when the EMS2D solver is selected. By default, EMS2D uses default frequencies (same as BEM2D).
Example of a frequency points file:
0.0001 0.0002 0.001 0.002 1 2 10 20
Coplanar Waveguide Characterization
The following CPW structures are supported:
Single stripline CPW Coupled stripline CPWSingle microstrip CPW Coupled microstrip CPWSingle CPW Coupled CPW
To support CPW structures, two new IML model types have been added to the SI library. These model types are:
The following enhancements have been made to support these new model types:
A CPW model can only be created if running from a product that supports the new EMS field solver. However, if you have an existing IML library that contains CPW models, you will still be able to see these models in the IML model browser regardless of the product that you are running. You must be running a product that supports EMS before one of these existing CPW models will be used for a simulation.
Disabling CPW extraction on individual nets
A new property, CPW_DISABLED, has been added to disable CPW extraction on individual nets. Attach this property to any nets that you want to be handled during analysis as non-CPW nets. If you have selected only the Ems2d Field Solver option (without Enable CPW Extraction), non-CPW nets will be generated with Bem2d.
As always, I'm interested in hearing how you employ these new features.
HI Cindy - yep, your post made it!
I am testing my post, just wanted to make sure it post correctly before I start posting & asking questions. Thanks
The shape under show a classic coplanar waveguide. The main difference for a part to be a coplanar waveguide.
This is my first time i visit here. I found so many entertaining stuff in your blog, especially its discussion. From the tons of comments on your articles, I guess I am not the only one having all the enjoyment here! Keep up the good work.
1. For the meshed ground planes, based on our current 2D field solver, (bem2d or ems2d), we can factor the mesh plane effects into account for the impedance value and reported in the IML model as additional data in the comment section.
2. For the small ground plane, our SPB16.6 version of the EMS3D field solver will be able to solve this type of structures rigorously and provide an S parameter model for it. For our current SPB16.5 release, the solver can handle it as a shape. The difficulty is how our GUI side and the geometry extraction part can get the information. So, could you please provide us either an example or a design (with the interested net specified). We can take a look and see how it's supported in our SI flow. I would suggest you contact our Customer Support team (file a new Service Request at - http://support.cadence.com) and a PCB SI AE expert will be able to work with you on this.
Are meshed ground planes (e.g. used for flex circuits) with track width, hole width and orientation taken into account in the solver ?
Same question for a 'small' ground plane which is not infinite regarding the Cline, i.e. edge of ground plane is closed to edge of line
CoPlanar waveguide information
Here's a reply from our PCB SI AE expert -
If you use a ground trace (which is a cline, or connect line), you will not see any difference in the impedance, regardless of whether or not you have enabled CPW extraction. Our tools do not support CPW extraction for ground traces surrounding a signal trace.
The only time you will see a change in the impedance is if you use a shape to surround the signal trace. The width of the ground shape that is surrounding the signal trace does not matter. The tool just looks for the existence of a shape associated with a DC voltage (within the geometry window) to determine if the trace will be analyzed as a CPW structure.
To see the change in the impedance, extract the net into SigXp from PCB SI (Analyze > SI/EMI Sim > Probe > View Topology) and note the impedance on the trace in SigXp. Change the spacing from the shape to the trace and extract again. You will see a change in the impedance in the CPW trace in SigXp.
Thanks Jerry.Again,For example if i use 10 mil wide ground trace and then 10 mil wide signal trace and then 10 mil wide ground trace,( the airgap among these traces will be 10 mil),then assume the simulated impedance is 50 ohm .If i change the airgap between signal trace and ground trace(from 10mil to 20mil),what will be impact on impedance.Can i check it out in PCB SI.?
I checked with our PCB SI expert AE, and she says -
"Ground traces are not taken into consideration, so the impedance will not change. It is only shapes that will affect the impedance when next to a trace."
What will be impact on impedance if we use ground trace instead of big shape.How we can check it out?Will the width of the ground trace play any role?
Hi redwire - Yep, typo in the first line of my post. The stackup in the board is used to determine the structure. If there is a soldermask defined, then this will be taken into consideration. Anything outside the stackup is not used.
What assumptions above the CPW are made? Soldermask? Metal height (for example, a grounded metal case)?
Oh, it's "coplanar" not "coplaner" :)