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 prior releases, Allegro PCB Editor does not provide the user the ability to place or make placement changes easily. New functionality to provide greater usability for component placement, alignment, replication of circuitry would greatly impact the time to get a design to fabrication.The SPB16.2 Allegro PCB Editor introduces the 4th application mode; General, Etch Edit, IFP and now Placement available to Allegro PCB Editor products. Allegro will continue to support the legacy command driven editing model commonly referred to as ‘verb-noun’ however application modes, based on context sensitive editing (noun-verb) offer a more intuitive approach to common design tasks such as etch edit, placement and querying.
Placement Application Mode"Placement Application Mode" is a tuned, high performance editing environment designed to increase efficiency during component placement sessions. Find filter settings are limited to those elements typically involved in placement such as symbols, pins and rat tees. This reduces unnecessary cycling of unwanted elements that do not contribute towards placement activity. In this mode, it is still possible to perform non-placement functions like add connect or slide however context sensitive and auto executed commands are biased towards component placement functions.
The Placement Application Mode can be enabled a number of ways:
Placement GUIThe list of unplaced components is conveniently located in the Options Panel while in Placement Application Mode. The form is an abbreviated version of the main Place Manual User Interface and supports:
Context Sensitive EditingThe RMB is context sensitive where commands and parameter options associated with component placement are available based on the selection set of elements. A context sensitive environment is designed to reduce the extra steps involved in traveling to the toolbar, menus or option panel while maintaining focus on the area of work in the canvas. Additionally, certain commands can be automatically enabled by a single pick or drag on the element.An example of context sensitive menus is shown in the figures below. The menus are a result of either hovering over or selecting with the LMB a symbol or pin followed by a RMB pick.
As with other application modes, the TAB key can be used to cycle through parent elements. For example, when hovering over a Pin, use the Tab key to change the selection state to Symbol (Symbol is the Parent of a pin).In General Edit Mode, using the TAB key while hovering over a Pin cycles to both Symbol and Net.
Placement Application Mode - Automatic Execution of CommandsCertain commands associated with component placement can be automatically executed using the LMB pick or drag functions. Simply click on a symbol, group, text or rat tee to Move it. Spin or Copy commands require the combination of either the Shift or Control key while in a drag operation with the LMB.
Align ComponentsThe Align Components command is available while in Placement Application mode and only operates on a pre-selected group of symbols.The use model for aligning components is designed to be straight forward and involves:
There are no options available with this command.Row versus column alignment will be decided by checking to see any movement of the components into a row or a column will cause the component placebounds to overlap. If an overlap in one direction occurs, then the opposite direction will be chosen. If this rectangle is "close" to a square, the user will be prompted for row or column alignment. If there is etch routed to the pins of components that are being moved, the first cline segment that is not marked as fanout will be deleted.Placement ReplicationA new suite of commands is introduced in SPB16.2 designed to replicate circuits within the PCB Editor tool. Circuit replication in the Cadence flow has traditionally been accomplished with the Design Re-Use Module application which requires both Front and Back End participation and is limited to Cadence supported schematic systems.A less restrictive, intuitive use model is desired that limits the dependency of front end requirements to just the traditional netlist. The placement of a "seed" circuit followed by a selection of randomly placed components generates the replicated circuits based on common device types, symbols and connectivity. Circuits that often get replicated are memory modules, IO channels and the capacitor scheme associated with BGAs or other active components.The steps involved in placement replication are as follows:
Please reply with how useful you find this new feature.
Jerry "GenPart" Grzenia
Please clarify what you mean by not be able to use the ifp mode.
why can't I use the placementedit mode and ifp mode，other 2 modes is well to use·
As I'm not an Allegro PCB Editor expert, I asked our resident expert (Rik Lee) for advice. Here's what Rik suggests:
There's one way to accomplish this -
Use Place >Replicate in the SPB16.2 release to create the replication of the BGA and associated parts. There MUST(!) be a refdes for the additional BGAs and components.
You then use the subdrawing command to replicate the etch that is attached to the symbol(s)
File >Export >Subdrawing;
Clines, vias available in the find filter;
Select the elements (temp group or window);
Select an origin (pin 1 of the BGA).
You will be prompted to save the data as a name
File> Import >Subdrawing;
Bropwse for the data saved above
Pick a placement location (pin 1 of the new BGA)
The netnames will take on the net name of the existing pin name.
In the upcoming SPB16.3 release, we're planning to enhance the place replicate command and it should replicate both the symbols and(!) the etch.
What I want to do is copy or replicate a circuit which has a BGA on it, and several hundred lines that connect to it. I have discovered that I can copy the etch, and that any etch that is connected to a via, will retain its net. However, the copy command, only copies the symbol. What I am looking for is a command which makes it possible to select a sequence of components, vias and etch, and which produces a copy of them which employs new reference designators and net names, automatically, which I can then back annotate into a schematic. The reason I am interested in this facility, is that it can take close to a man month to fan out a complicated high speed BGA that employs LVDS etch, etc., and once you have a working design, and want to create a board which has many more of these BGAs (and I am thinking about building a board with seven BGAs at this time), it would be nice if you could simply replicate and place the entire circuit. For this to work right now, I need to know how to convert a symbol that has been placed into a component. Another work around might be to do the copy command, carefully locating the BGA, and then delete the symbol and place in its prior location the correct component, and then go through and change the nets on the old etch to match the net names of the new component.
Glad it's working for you Tim. You can explore/ask questions in the PCB User Community Forums at - www.cadence.com/.../pcb, in the Cadence Help documentation (that ships with the products), or you can always contact our Customer Support team.
Jerry, thanks that worked! I thought I would have to re-draw my different groups of parts for each angle, so I am glad you told me about this. Where is the best place to go for other generic schematic editor questions? Thank you. --Tim
Thanks for your question. There sure is. Just construct a group of objects like you would normally. Then, type rotate or spin, and use the middle mouse button to click near the center of the group. The group will rotate. Keep clicking the middle mouse button and the group will rotate another 90 degrees for each click. You then place the group with the left mouse button.
Hope this helps!
Jerry, is there a way to rotate a group of parts in the schematic editor? I am currently working on a Allegro PCB Design HDL XL 16.2 and would like to rotate a group of parts. Thank you for you help. --Tim
This capability to rotate a group of object already exists and has for many releases by using - Edit >Move or Edit > Spin.
If you want to keep the relationship of the symbols to each other you must select "User Pick" in the options tab. The symbols can be a part of the group, but do not have to be. You can select multiple symbols by using Edit >Move; RMB "temp group' and then selecting the symbols you want to move/spin/rotate.
See SourceLink Solution# 1837513 for more details.
Place Replicate is a great addition to Allegro. Just one comment; please add a 'Rotate' function to allow rotation of the group while it's on the end of your cursor.