Stats

  • Locked Locked
  • Replies 2
  • Subscribers 166
  • Views 16592
  • Members are here 0
More Content
This discussion has been locked.
You can no longer post new replies to this discussion. If you have a question you can start a new discussion

Using Height Property from Orcad Capture

rgmeier3

All,

I would like to use the Height property in Orcad Capture and transfer it to Allegro PCB Editor. I am able to get the height property exported from Orcad and attached as a property in Allegro as a componemt property.But I have not been able to get it to replae the Package_height_max property for DRC checking. If anyone has this working please let me know the steps required.

 

Thanks,

Gerry

 Below is an excerpt fro mthe props ref document. I know it is written for Concept but thisshould work for Orcad too.

 HEIGHT
The HEIGHT property, attached to component definitions in a schematic system and a value
maintained in user units in the database, controls package height and can be sourced from
the Allegro Design Entry HDL Part Table File (PTF). For discrete parts, whose physical
footprints are identical except for height variations due to multiple manufacturers, use the PTF
package height model, which minimizes design disruption as front-end librarians may already
be using this property for IDF support.
When creating the physical footprint, ensure that no PACKAGE_HEIGHT_MAX property is
assigned to place-bound shapes. Only those symbols whose height is driven from the
schematic require this change. (Any existing HEIGHT properties assigned to package
symbols take precedence.)

To allow the DRC system to use the component-definition HEIGHT property driven from the
PTF, choose File – Import– Logic (netin command) to map the component-definition
HEIGHT property currently used by the IDF interface to the PACKAGE_HEIGHT_MAX
property on the component definition.
Because the HEIGHT property is defined as a component property in Allegro, it may be
passed forward to Allegro from an Allegro Design Entry HDL netlist. Its value cannot be
changed in the Allegro database as it is device and netlist driven.
Define the HEIGHT property in one or more of the following locations. When the design is
packaged, Packager XL applies the first HEIGHT value found in the following order of
precedence.
■ as a body property in the symbol definition
■ in the part table as either a key or injected property
■ the chips.prt file as a body property
However, the component may have only one HEIGHT property value. If the component’s
actual height is irregular, the varying heights of its profile cannot be described using a
HEIGHT property, and component-to-component or component-to-package-keepout DRC
audits ignore the HEIGHT property’s value.

 

  • steve

    Give this a try:-

    1.       Set a Capture Property Component_Height.

    2.       Edit the allegro.cfg file to include Component_Height=HEIGHT under ComponentDefinitionProps.

    3.       Import into Allegro as you would normally. Ensure none of your parts have any heights set in the symbol files. (dra). The Height property will then populate the PACKAGE_HEIGHT_MAX and HEIGHT (From a show element on the symbol).4.       When you look at a 3D view of the board the heights should be as per the HEIGHT property.5.       There is a user preference (Setup – user preferences) under the interfaces – IDF folder called idf_ignore_comp_height. Check this property. Then when you create your IDF file the symbol based height property is used.

     

  • fxffxf

    For access this capability, you must be running 16.2 or newer.

     Allegro has a order of precendence in dealing with the PACKAGE_HEIGHT_MAX or MIN properties

    • the (physical) symbol  package bound shapes
    • component definition where HEIGHT is mapped to PACKAGE_HEIGHT_MAX
    • board 

    If you built your symbols (.dra) and assigned the PACKAGE_HEIGHT_MAX property to tjheir place bound shapes, this will always win over any HEIGHT (or PACKAGE_HEIGHT_MAX) properties injected from the schematic. So if you want to drive some or all of your place bound height values from the schematic part libraries, you should inspect your symbol files (.dra) for package height properties.

     

Cadence 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.