Cadence® system design and verification solutions, integrated under our System Development Suite, provide the simulation, acceleration, emulation, and management capabilities.
Verification 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.
The Cadence Academic Network helps build strong relationships between academia and industry, and promotes the proliferation of leading-edge technologies and methodologies at universities renowned for their engineering and design excellence.
Participate in CDNLive
A huge knowledge exchange platform for academia to network with industry. We are looking for academic speakers to talk about their research to the industry attendees at the Academic Track at CDNLive EMEA and Silicon Valley.
Come & Meet Us @ Events
A huge knowledge exchange platform for academia. We are looking for academic speakers to talk about their research to industry attendees.
Americas University Software Program
Join the 250+ qualified Americas member universities who have already incorporated Cadence EDA software into their classrooms and academic research projects.
EMEA University Software Program
In EMEA, Cadence works with EUROPRACTICE to ensure cost-effective availability of our extensive electronic design automation (EDA) tools for non-commercial activities.
Apply Now For Jobs
If you are a recent college graduate or a student looking for internship. Visit our exclusive job search page for interns and recent college graduate jobs.
Cadence is a Great Place to do great work
Learn more about our internship program and visit our careers page to do meaningful work and make a great impact.
Get the most out of your investment in Cadence technologies through a wide range of training offerings.
Overview All Courses Asia Pacific EMEANorth America
Instructor-led training [ILT] are live classes that are offered in our state-of-the-art classrooms at our worldwide training centers, at your site, or as a Virtual classroom.
Online Training is delivered over the web to let you proceed at your own pace, anytime and anywhere.
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.
I'm using Allegro PCB Editor 16.3, kind of new to it but I have plenty of experience using OrCAD Layout. I.e., I know what I want to do, but not how to do it in PCB Editor.
I'd like some help with the following problems, one or (preferably) more of them:
In case 1, I have a 3-pin symbol in the schematic, that is to be connected to a 4-pin, through-hole footprint (the physical component, a TO-220, have pin #2 and the heatsink connected internally). I have placed a static solid (non-dynamic) shape on the TOP layer, that includes both the electrical pin #2 and the mechanical pin. This works but produces DRC errors ("Thru Pin to Shape Spacing", which I waive in the board editor). However, there must be a better way to do this. (I don't want to introduce a fourth pin in the schematic symbol.)
In case 2, I want to place a copper area on the BOTTOM layer beneath the TO-220 mentioned above, and connect the two with thermal vias. Of course I want the bottom copper to remain beneath the actual component, even if it is moved.
In case 3, I tried including a "anti-etch ALL" shape, in both the symbol editor and the board editor, but the dynamic copper fills still came to within the global clearance limit. I solved the problem by creating voids in, or modifying edge contours of, the dynamic ground plane shapes, but this will of course cause problems if the components are moved (and if I forget to update the planes). Must I somehow give the anti-etch shape a higher priority than the dynamic fills?
In case 4, I have a 6-pin DPDT switch that I use as a SP3T switch (by shorting two of the leads). The symbol have relatively gigantic holes in the PCB, since the actual component is supposed to be panel mounted, not TH mounted. So I included smaller-diameter holes near each electrical pin, defined as mechanical pins, to make it easier to solder cables to the board. All four electrical pins are connected to the corresponding mechanical pin with a solid copper shape on an etch layer. The four remaining mechanical pins are connected by a similar shape (and are automatically attached to "Dummy net"). However, when this symbol is placed on a ground plane, the ground plane shorts all four mechanical pins. (The electrical pins and the corresponding mechanical pins have the global shape clearance distance.)
[Edit: The schematic SP3T symbol is a 4-pin component, so I could solve this by making the schematic symbol a six-pin component, to match the actual footprint. But this forces the schematic designer to manually connect the two remaining pins. It would also clutter the schematic. My non-ideal solution so far is to make voids in the ground plane around each SP3T switch.]
1. DRC errors are always produced in the symbol (DRA file). The DRC's are cleared when you place the symbol into a board file and import the netlist. The shape will take on the netname of the net connected to the pin. So If pin 2 is connected to VCC that would be the netame of the shape.
2. You can window select the items you want (check find filter for more control) then use RMB (right mosue button) Add to Group, enter a name and OK. Then make sure only group are checked in the find filter (or RMB super filter) and move the group.
3. Add a shape to the layer Route Keepout / All or layer specific.
4. If they are mechanical pins then they WILL ALWAYS be voided from a net. Check that the shapes are dynamic and that the shape to clearances are set. If they are electrical pins and they do connect (but you don;t want them to) then add a property to the PIN (RMB - Property Edit) called DYN_THERM_CON_TYPE and set this to NONE.
In reply to steve:
In reply to Johnny Nguyen:
I don't remember if it is available in 16.3, but in 16.6 you c an add the property "Via allowed" to the route keep out shape to get the results you are looking for I believe.