Stats

  • Locked Locked
  • Replies 6
  • Subscribers 163
  • Views 18952
  • 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

Templates and CM default values (PCB Designer 16.5)

B Price

Right now, the Constraints Manager (PCB Designer 16.5) populates all the entries with default values (for example, 5 mil spacing minimums for everything).  Is there a way to change these defaults?

On a related note, as I understand it there are several different template files that can be used:

.brd board files

.tcf technology files

.prm parameter files

 

My general understanding is that using a .brd template would include all the .tcf information and some/all of the .xml parameter information.  Can anyone clarify this?

Ideally, by setting up the right template I'll be able to preload all the desired settings for things like minimum trace widths, class colors, thermal relief specs, grid sizes, etc...

  • oldmouldy

    No, you cannot change the defaults. Yes, you can create a board as a "starting point", or Template, and go from there. This template board can contain "anything" that does not relate to a netlist. Start a new board with the defaults, change all the settings you require for the template, save the resulting BRD file.

    Within PCB Editor: 16.5 and on: File>New, there is a template button to browse for a template and a User  Preference to configure as the Template file source. Previous releases: copy the "template" and load the Logic into it.

    Schematic driven: All versions: I think that both the HDL flow, and certainly the Capture (CIS) flow, allow an "input board" to be specified as a starting point to load the Logic into, Export Physical for HDL and Tools>Create Netlist for the Capture CIS flow.

  • B Price

    Thanks once again, oldmouldy.

     

    Just to clarify, is it true that if I set up the .brd file correctly and use that as a template, there should be no reason to use .tcf or .prm files?

    Things like trace widths are netlist specific - but can I preload them with my own 'default' minimums somehow?

     

    Regarding schematics, are you indicating I should load in my input board template at the schematic capture stage?   

  • oldmouldy

    Yes, that's true. You can setup the Constraint Sets for the various routing parameters and then apply then to Nets or Net Classes once the netlist is loaded.

    Well, it's possible to drive this from the Schematic when the Netlist / Logic gets created, this is not a requirement though since you may be "given" the Netlist / Logic data, rather than creating it from the schematic. The process is that the Netlist / Logic and the Template need to be merged, you can do this in PCB Editor or driven from the Create Netlist / Export Logic step.

  • B Price

    I created a .brd board template but when I start a new board and try to load a template, nothing shows up (aside from .brd files in the current directory).  I can't browse to the correct location.  Database is unchecked and Library is checked (both grayed out).

    I assumed I was missing a path in the User Preferences Editor, but I can't find any reference to .brd templates.  It's probably an easy answer, but what do I need to do? 

  • oldmouldy
    Setup>User Preferences, Paths, Config, wizard_template_path will set the paths to the template BRD files. You can remove all the default entries, if required.
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.