Home > Community > Blogs > PCB Design > what s good about allegro s placement application mode look to spb16 2 and see
 
Login with a Cadence account.
Not a member yet?
Create a permanent login account to make interactions with Cadence more convenient.

Register | Membership benefits
Get email delivery of the PCB Design blog (individual posts).
 

Email

* Required Fields

Recipients email * (separate multiple addresses with commas)

Your name *

Your email *

Message *

Contact Us

* Required Fields
First Name *

Last Name *

Email *

Company / Institution *

Comments: *

What's Good About Allegro's Placement Application Mode? - Look to SPB16.2 and See!

Comments(10)Filed under: PCB design, PCB Editor, Allegro 16.2

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:

  • Setup — Application Mode — Placement Edit
  • RMB click in Canvas area followed by Application Mode — Placement Edit
  • ToolBar Icon

 

Placement GUI

The 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:

  • Selection of one or more components from the tree view form.
  • Refresh of form as components are placed.
  • "Place by refdes" function to place specific components by reference designator names; wildcards (* and ?) are supported.
  • Mirror" option automatically changes component selection set from Top to Bottom side."More Options", when selected launches the main Place Manual form providing access to filtering functions.

 

Context Sensitive Editing

The 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 Commands

Certain 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.

 

Element Type Drag Shift-Drag Control-Drag Single Click
         
Group Move Spin Copy Move
Symbol Move Spin Copy Place Manual
Text Move Spin Copy Move
Rat T Move     Move

 

Align Components

The 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:

  • Set Application Mode to Placement Edit
  • Select with the LMB all components that are to be aligned. The selection set is limited to the same side of board.
  • Hover over the reference component which should be part of the original selection set and pick Align Components from the RMB popup menu.
  • Components in the selection set will be aligned to the reference component by body center.


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 Replication

A 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:

  • Set Application Mode to Placement Edit; Place Replication is only available in this mode.
  • Layout initial (seed) circuit.


     

  • Create .CRF (Circuit Replicate File).
    • With the LMB, select all components associated with the seed circuit then use RMB — Place Replicate Create command.

       

       

    • Enter a name for the replication file. There is an option to save the file to disk for use on other boards

    •  

  • Apply .CRF (Circuit Replicate File)
    • Window select components of the targeted replication groups. Selection can include components that do not factor into the replicated circuits however limiting the selection to relevant members reduces processing time.
    • Once selected, use RMB — Place Replicate Apply command then select the .CRF file in the RMB menu or browse to the file on disk.

       

       

       

    • If a solution is found, the resultant circuits appear on your cursor, one instance at a time.

       

       

       

    • Each circuit is stored in the database as a group object. The naming convention used is _PR_CRF#. In the above example, the group names would be _PR_DIMM_1, _PR_DIMM_2, etc.
    • Routes are not captured as part of the .CRF file. Use the copy command to copy routes from the seed circuit to each replicated one.
    • Currently if changes are made, for example the need to add components to each circuit, a new .CRF must be generated and re-applied. This will result in the re-placing of each circuit.

 

Please reply with how useful you find this new feature.

Jerry "GenPart" Grzenia

Comments(10)

By annoonan on August 14, 2009
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.

By Jerry GenPart on August 17, 2009
Hi,
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.
Jerry

By Tim Severance on September 2, 2009
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

By Jerry GenPart on September 3, 2009
Hi 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

By Tim Severance on September 3, 2009
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

By Jerry GenPart on September 3, 2009
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

By Stephen Fried on October 16, 2009
Jerry,
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.
Any ideas?
Steve

By Jerry GenPart on October 19, 2009
Hi Steve,
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.
Jerry

By sate.xu on November 16, 2010
why can't I use the placementedit mode and ifp modeļ¼Œother 2 modes is well to use·


By Jerry GenPart on November 17, 2010
Hi "sate.xu",
Please clarify what you mean by not be able to use the ifp mode.
Jerry

Leave a Comment


Name
E-mail (will not be published)
Comment
 I have read and agree to the Terms of use and Community Guidelines.
Community Guidelines
The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. 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. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.