Home > Community > Blogs > PCB Design > what s good about allegro pcb editor idx support look to spb16 5 and see
 
Login with a Cadence account.
Not a member yet?
Create a permanent login account to make interactions with Cadence more conveniennt.

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 PCB Editor IDX Support? Look to SPB16.5 and See!

Comments(0)Filed under: PCB Layout and routing, PCB design, Allegro, PCB Editor, PCB, layout, "PCB design", routing, SPB16.5, Allegro 16.5, MCAD, IDX, EDMD, IDF

The Allegro 16.5 release was made available on May 17, 2011!

This release adds additional improvements and efficiencies to your design process.

New technologies in Allegro 16.5 include advanced miniaturization capabilities, integrated power delivery network analysis, DDR3 design-in kit, bolstered co-design featured and flexible team-design enablement to address global designer productivity.

Today, I’ll discuss the enhancements to the Allegro PCB Editor for a new standard EDMD schema. The EDMD schema is a new XML based data exchange format.

Historically, design data has been passed between ECAD and MCAD domains using interim file formats such as IDF and DXF. These formats have numerous limitations that prevent accurate and/or complete representation of data from the source design (whether ECAD or MCAD) in the target domain. Additionally, there has been no effective way to communicate proposed changes from one domain to the other without sending the design in its entirety. As a result, collaboration between these domains has been cumbersome, and it gets worse as the design progresses. Designers are forced to either extend the time it takes to do the designs or risk going to manufacturing with design errors, resulting in rework and delayed time to market.

This new approach allows ECAD and MCAD designers to pass changes they made to their designs in an incremental fashion. Additionally, the new standard provides a way for designers from both sides to accept/reject the changes proposed on an object by object basis. This provides a level of control, traceability and collaboration that has never been possible before.  With only incremental design data being passed between ECAD and MCAD domains, designers spend very short time reviewing, accepting/rejecting the changes and ensuring that the two domains are in sync. This avoids any miscommunication that can result in rework and improving chances of first time success significantly.

Allegro PCB Editor 16.5 supports this new standard v2.0.

What is EDMD? EDMD Schema (file extension) is a file format for the Incremental Data Exchange (IDX) of data between Electrical and Mechanical data systems referred to as EDMD (Electrical Design Mechanical Design). Version 2.0 of the format contains the same data as IDF 3.0 without panelization data. IDX is Managed by ProStep iVip, a European based consortium

IDX formats give you the ability to preview changes graphically before accepting or rejecting the data. The main benefit of the IDX interface is it provides support of collaboration by using incremental changes with accept/reject and comments defining intent.


IDX Import


New in Allegro 16.5 is the IDX Import command idx in (File— Import — IDX).


 


Selecting "Import" will open the file browser to select the IDX file you want to import. Selecting "Import" again will open the "Select Items to Import" dialog to select the objects to import. All the items will be dimmed except for the changed objects.



 

  • The field's Object Type, Object Name, Comment, and Status are from the IDX file and are read-only.
  • The reject comment can be edited and will be added as history to the IDX file.
  • The transaction history for the current object will be displayed in the bottom form field.
  • Click any cell instead of "check box" to preview the object changes graphically for board outline, keepin, and keepout. For components and holes, the change information will be displayed in the Allegro command window.
  • Properties changed will be displayed in the Allegro command window.
  • Enable the check box to import and highlight the object, uncheck the box to rollback the change.
  • The next button ( --> ) will move to the next changed object.
  • The previous button ( <-- ) will move to the previous changed object.
  • Right clicking the mouse button pops up the Accept/Reject/Next menu. Accept will check the import box, Reject will rollback the change and uncheck the import box if it was checked, and Next will process the next object.
  • Reset - rollback all the imported objects and start over again.
  • Cancel - rollback all the imported objects and exit the dialog.
  • Select All - import all the objects.
  • Roam and Zoom - if checked, it will roam and zoom to a size for displaying the old and new location of the item being changed.
  • OK - updates the baseline and creates a new IDX file with the updated transaction states and reject comments, and then exits the dialog. A log file is generated to review the history.

Allegro will reject any Via changes.

There is no batch interface for importing IDX data. The new import process allows you to accept or reject individual changes; this is the heart of the IDX’s support for incremental change management and ECAD-MCAD co-design.


IDX Export


The idx out command (File — Export — IDX) allows the export of IDX data.




 

The baseline will be created for the first export and the baseline will be attached to the database. If you want this new configuration to be the baseline, select the "Re-Baseline" button.

The base filter configuration can be changed at this point using the button “Filter Options” button:





Just as in IDF import, the base filter configuration is used to exclude objects from the IDX file.

  • Vias and unplaced components are filtered by default.
  • The file extension for filter configuration file will be “.config”.
  • The new environment variable IDXFILTERPATH will be used to search for base filter configuration file for the first time setup.
  • The filter file settings are attached to database if the OK button is clicked.

Selecting "Export" will open the "Select Items to Export" dialog:



 

  • The fields Object Type, Object Name, Status are from IDX file and are read-only.
  • The export comments can be edited here and will be recorded as history in incremental data file.
  • Select All – Select or Deselect all the objects.
  • Reset – Change back to the original selections.
  • Cancel – Exit export.
  • OK will export the selected items to an incremental data file. The current selection and comments will be saved in a configuration file, which will be used as default value for the next export.

One single IDX file will be maintained, and the new IDX data will be added to the existing processed IDX data.


Batch interface for IDX Export


The idx_out executable can be used to write an IDX file out of Allegro. The file extension is the same as the GUI output - “.idx”.
Command syntax:
idx_out <design_name > [-obsh] [-c <base_config>] [-f <increment_config>] [-i <baseline>] [-xp]

-o Output file base name. Name of the resultant IDX files. Default: <design_name>.idx

-c Base configuration File. Name of the file to use to filter the specified parameters from the resultant IDX file.

-f Incremental configuration File. Name of the file to use to filter the specified objects from the resultant IDX file.

-b Board Version.

Valid Arguments: user specified integer. Default: 1
-s System ID.

Valid Arguments: user specified string. Default: ""
-i Baseline used to create incremental data file.

-h Default height. Applies this value to all package symbols without a specified package height.

Valid Arguments: a floating point value consistent with the original design units. Default: 0.0
-xp Export Plane_shapes, Clines, Pins, Vias, Test_points only

Example 1: Baseline File:
idx_out test.brd -o test_base -c idxFilterOut.config -h 150.00


Example 2: Incremental Data File:
idx_out test.brd -o test_delta -c idxFilterOut.config -h 150.00 -i test_base


Example 3: Export Plane_shapes, Clines, Pins, Vias, Test_points only
idx_out test.brd -o test_copper -c idxFilterOut.config -xp


Note: The format of the filter file is:
(filter Vias Pins Plane_shapes Clines Test_points)



IDX versus IDF


When importing IDX data into a design that has IDF data/properties in it, the following prompt will appear:




Click No to exit. Click Yes to proceed and display “IDX In” dialog.

When importing IDF data into a design that has IDX data/properties in it the following prompt will appear:




Click No to exit. Click Yes to proceed and display IDF In dialog.

As always, I welcome your comments about how you’re using this new 16.5 capability.

Jerry “GenPart” Grzenia

Comments(0)

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.