Cadence® system design and verification solutions, integrated under our Verification 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.
More Support Log In
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 technology. 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.
Get email delivery of the Cadence blog featured here
Placement replication was introduced in Allegro PCB Editor SPB16.2. At that time, the application was limited to replication of component placement. The SPB16.3 release introduces the support of etch circuits (shapes, clines, vias) as well as ease of use improvements associated with basic move, mirror and rotate functions. Once replicated circuits are placed, physical changes such as moving components or modifying etch circuits are easily instantiated across all instances with a new update command.The methodology for creating and applying replicated circuits is similar to that of SPB16.2 however the stored file format is different due to the support of etch and the refresh capability. The file format leverages the legacy module (.mdd) database structure and replaces the circuit replicate file (.crf) format. SPB tools continue to support the front end driven re-use flow and the backend driven placement replication which is schematic neutral. Placement replication files can be leveraged across different designs containing common circuitry blocks such as decoupling schemes for high pin count devices, memory arrays, and IO channelsPlacement replication is only available within the "Placement Edit" application mode environment. The use model requires the pre-selection of symbols followed by a RMB action command.
Aligning modules and replicated circuitsThe alignment of re-use modules and place replicate circuits is now supported in Placement Edit Application mode. The use model is similar to the Align Components command that was introduced in 16.2. The three step process begins with a window selection of the module circuits; hover over a symbol within the circuit you wish all others to be aligned to and then using the right mouse button command "Align Modules" to perform the alignment.
Using the commands1. Enter the placement application mode.
2. With the seed circuit placed, window select all of the components followed by a right mouse button "Place Replicate Create." When accessing the right mouse "Place Replicate Create." menu item be sure to hover over a component element, such as a pin, in order to get the right mouse button menu. Hovering over black space will not produce the commands related to the selected elements.
All intra connected circuitry will be highlighted.
3. You will be given the opportunity to select or unselect additional etch from that which was auto-generated for the seed circuit. A typical application may be to extend the circuit to include I/O.At the Allegro command window you will be prompted "Select/unselect additional etch as needed, then click Done." Select or unselect additional etch elements using the combination of the left mouse button and the control key. In the image below the 5 clines off of U120 were selected.
4. You will be prompted to "Pick origin or use RMB for Snap to" functionality. Use the Snap to functionality to snap to a pin or via or other element.5. You will be prompted, with a GUI to save the seed circuit. It will be stored in .mdd format.6. Window select the remaining components that you want to replicate followed by a right mouse button "Place Replicate Apply". You can either continue in the right mouse button selection to select the replication module or select "Browse" to use a GUI to select the module.. Minimize the selection to relevant components to minimize any performance impact.
7. The following interface appears which lets you swap components. The first column lists the contents of the next circuit to be placed, the second column lists the swappable components in that circuit. When a component is selected in the "Swappable" column, a list of components to swap with appears in the "Swap With" column.
8. Selecting "OK" will place the replicated circuit on your cursor.
9. Place all of the circuits. Care doesn't need to be taken to place them in proper alignment.
10. Window around all of the replicated circuits, including the seed circuit, and select right mouse button "Align Modules" while hovering of a component that you wish the other circuits to be aligned to.
11. If a change needs to be made to the circuitry you can make those changes and then update those changes to the other replicated modules. IN the image below some delay has been added to etch.
12. Set the super filter (right mouse button) to "Module". Hover over the circuit that the changes were made to and select, using the right mouse button, Place replicate apply. You will be prompted to select/unselect additional elements and then select "Done".
13. A file save GUI will be presented to you where you can save the circuit. At that time the updates will be applied to the circuits in the design.
-14. While you are in the placement application mode and the super filter is set to "Module" you can move the replicated circuit as a group by hovering over the module and selecting "Move". You can also take advantage of single pick functionality by enabling the right mouse button functionality "Customize -- Enable Single Click Execution." Using this you only select the module to move rather than hovering over the module and selecting "move" from either the right mouse button or the Allegro menu.14. While you are in the placement application mode and the super filter is set to "Module" you can move the replicated circuit as a group by hovering over the module and selecting "Move". You can also take advantage of single pick functionality by enabling the right mouse button functionality "Customize -- Enable Single Click Execution." Using this you only select the module to move rather than hovering over the module and selecting "move" from either the right mouse button or the Allegro menu.
As always - I welcome your feedback and suggestions on using the new SPB16.3 features.
Jerry "GenPart" Grzenia
I'm not too sure of the exact nature of the issue you're having based on your description. It "may" be a older release problem, or a database problem, or just a use model issue. The best method to getting this resolved would be if you contact our Customer Support team at http://support.cadence.com so that an Allegro PCB Editor expert AE can work with you to resolve this specific issue.
i am using cadence16.3. my old project is orcad9 i am translate this pcb to cadence 16.3. after converting one ic(U1) is hide.that U1 manually place there.i try to place that component but that component not placed.please tell me any another way of this project translation
PCB Design L would be the lowest level product supporting these SPB16.3 features.
Is this option available in Orcad PCB Editor 16.3?
What I suspect you're trying to do, is if you move the Ref Des position(s) for footprints on the original circuitry that you made the copies (replications), you want all the Ref Des positions in the replicated circuits to also move accordingly. You need to move each of the replicated circuit Ref Des positions individually. Let me know if this answers your question.
How to "replicate update" the silcscreen drawings, e.g. Ref Des positions and orientation?
Hi Ashok -
This functionality is part of the Allegro PCB Editor SPB16.3 release - you don't need to purchase anything separately. Also, while you're replicating the modules, the part ref des/pin # values are being driven from the schematic netlist - this is why you see the values automatically being updated as you replicate a circuit. So, the synchronization is maintained.
while using this repeat placement how to sync the repeated placement with the schematics. also please let me know is this function a model which needs to be purchased seperately?
The Allegro Free viewer for the SPB16.3 release is now available!
You can flip & rotate, but the stack needs to be the same. If you try to place it on a board with a different stackup the application will issue a message that the stackup are not the same and not place it.
Good write up Jerry.
You mentioned a mirror function - will this support flipping the circuit to the other side of the board? So, in a 4 layer board, layer 1 is mapped to layer 4, layer 2 to 3 and so on?
Also, if I wanted to use a circuit from one design in another, do the layer stackups have to be the same?
The SPB16.3 free viewer is not available for download just yet. When it is, you can use the Cadence Online Support Solution# 11250908 to locate it (www.cadence.com/.../Downloads.aspx)
If you have installed Allegro you can use the executable in Cadence_installation_directory/tools/pcb/bin/allegro_free_viewer.exe
When will 16.3 viewer be available?