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.
Hello ,Can any one explain what exacly is use of command Tools----Setup Advisor .....What parameters are to set using this setup advisor and whether these parameters are to be set every time when we start a new design?We have never used setup advisor before....Regards,Prajakta.
The Setup Advisor is used to configure different elements of the design - it's a gateway to configuring Cross-Section, DC Nets, standard Device values and SI Models. It will also perform an audit on the design.The main function of Setup Advisor is to mainly assist in the design setup for some kind of SI work - the steps in Setup Advisor are recommended but not always needed. For example you could edit the cross section yourself without using the Setup Advisor.The individual steps that make up the Setup Advisor are available seperately in the higher tiers of the tool (XL, GXL), so if you know what you are doing in these tiers the Setup Advisor probably won't be needed. In the lower tiers of Allegro (L, Performance) some of the commands can only be accessed via the Setup Advisor.So, in short, if you are just doing plain PCB design then you probably wouldn't need to run the Setup Advisor - if you are planning on doing some sort of SI work, then it's a good idea to use the Setup Advisor while you find your feet.
Hello Prajakta,The setup advisor command displays the Database Setup Advisor that lets you extract a topology into Signal Explorer:To successfully extract a topology into Signal Explorer, certain information must be setup properly in the layout database so that the electrical circuit topology can be accurately synthesized.The Database Setup Advisor guides you through this setup process. If done correctly, this only needs to be done once with the layout database; then you should be able to extract any signals into Signal Explorer.The Database Setup Advisor is automatically invoked if there is a problem found with the signal that you want to extract. It can also be invoked directly from the Topology Template dialog box in Signal Explorer. You should run the Database Setup Advisor once on each new design before extracting topology data. The Database Setup Advisor walks you through the following modules:1.Stack-Up: Define the type and characteristics of the varied material layers in the layout. Set the layer stackup with copper thickness,prepreg and laminate thickness.It is better to set before routing always.2.DC Nets: Identify which nets in the layout are to be connected to a constant DC voltage. You can identify the DC nets.it is for tool to understand that these are power signals.If you not set ,the tool assumes as a signal. This is must when the design contains high speed signals going between processor to memory devices through terminations.3.Devices: Provide information about the devices in the layout, such as Class and Pinuse properties.4.SI Models: Assign electrical models to components in the layout. You can assign SI models to components like terminations,processors etc... for the SI analysis and constraint settings. This is must when you set length delay constrains going between processor to memory devices through terminations.It is just an example.5.SI Audit: Audit specific nets in the layout to verify that they are set up properly for extraction and simulation.Regards,SATYAAT&S ECAD Tech.
Thanks for your replies . Atleast I got the basic idea ...where and how , exactly the setup advisor can be used...Regards,Prajakta.
The set up advisor is very important if you are using constraint manager. Assigning DC nets and models for passive devices, resistors, caps, Rpacks, allows you to use extended nets to properly use constraints.