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.
In the Allegro PCB SI 16.6 release, vias in SigXp have been enhanced to make it more efficient for design use. In addition, Allegro PCB Editor padstacks will be used to build the models.
Read on for more details …Adding Vias
Adding a via is easier and faster than before. You no longer have to go through the Via Model Generator to create a model nor are you required to search the list of existing models that fit the need. The difference is that you are now adding a via rather than a via model. The via may not be pre-solved to a specific model.The current way of adding a via in SigXp is still supported and unchanged. You can still add a via model on the canvas.In order to add these “dynamic” vias in SigXp, a layerstack will have to be present in the topology. In a new topology this can be accomplished by using the Manage LayerStacks function to create or import a layerstack. When a topology is extracted from Allegro, the layerstack of that board is automatically imported in the topology.A new via is added with two nodes (two connection points) on the canvas. When newly added, the two nodes are not tied to any specific layer as they will take on the properties of the connected node, so the label of those nodes will be Layer1 and Layer2:
If a trace is connected and is on a particular layer then the via node is assumed to be on that layer and will take its properties. In the case of a "floating trace" (a trace not on a layer stack layer), the via node will take its properties and still say LayerX (unchanged). Since we do not know what layer that is, we will assume the top or bottom most layer of the via structure: The prior release (16.5) via toolbar button is a two-part button which lists all available via models on the right hand side pulldown: Clicking on the left side of the button (the one with the via image) brings up the Add Element Browser. In 16.6, the left part of the Add Via button will add the new “dynamic” via with only two nodes. The pulldown remains unchanged to list the pre-solved via models.
Reuse of Via Models
You will want to reuse already solved via models in SigXp. To do that, the same technique used today is available. You can either select the right button of the Add Via toolbar button, which will list all existing via models available sorted by types, or RMB > Add Element can still be used to choose the desired via model.
When these via models are added to the canvas, the model is “locked” to the via and cannot be changed - this is the via model that will be used to simulate.
The new (dynamic) via has the following parameters which are listed in the standard parameters spreadsheet. These parameters can be modified: model The via model associated with the via. A via which has no model yet will have UNMODELED as a model. Once solved, the name of the model will be used.viaOutputFormat The format with which the model was solved. If no model exists yet, the format is blank.viaPadstack The name of an available padstack. This parameter is a pulldown which lists the available padstack files on disk and in the library.viaTopLayer The top most layer of the via drill.viaBottomLayer The bottom most layer of the via drill.
For coupled vias the parameters will be a little different. It will show the via name with which it is coupled as well as the distance between them. Aside from that, it will look just like a single via.Padstack Consumption
SigXp can now consume and optionally modify the same padstacks as Allegro PCB Editor. You can to import *.pad files and keep them as file if they are different than the library.You can access the Via Padstack Manager through the menus using Setup > Manage Via Padstacks, or by right clicking in the SigXp canvas and selecting Manage Via Padstacks. Editing or creating a new padstack will use the same padstack editor available in Allegro. The padstack can be saved as an external file. If shapes are associated with the padstack, they will be stored in the same location. All information in the padstack relevant to the via is used to generate the model: Via Modeling
When a new “dynamic” via is added to the topology, no model is associated with it. Only when you perform a simulation or manually solve the via will the field solver be called. In batch mode, the field solver uses the standard via modeling preferences that are currently found in PCB SI. These settings are available in SigXp and can be accessed through the menus using Analyze > Via Setup Preferences or by right clicking in the SigXp canvas and selecting Via Setup Preferences: The via subckt section is built using the padstack information, the layerstack and the connected traces, as is done in Allegro PCB SI. The via model is stored in the working IML file.
With this feature, you can couple 2 single vias to form one single model. You can select 2 vias in the SigXp canvas and select Couple from the right mouse button menu: When the Couple function is used, you will be required to specify a spacing between the vias: This spacing is added to the parameters in the spreadsheet: When you select a coupled via, all vias in the set will be selected: You can decouple the vias by selecting Decouple from the right mouse button when one of the vias is selected:Please share your experiences using these 16.6 features.
Jerry "GenPart" Grzenia
Here's a very good landing page for the Sigrity products: www.cadence.com/.../default.aspx
I need the simple datasheet (manual) for signal integrity in allegro(cadence). please help me?