Place all components without schematic

there is automatic placement u may want to try but u need to set many properties up before using it.

Hello,

As you found Quickplace only places components that are in the Parts List and not unassigned Package Symbols , I do have a workaround for you using a shortcut key.

1. On the command line type the following: (Command >)
   
   • funckey q ix 1000
2. Open Placement Dialog (Place > Manually) and under Advanced Settings tab select Library [You got this far before]
3. Select Package Symbols you want to place under Placement List tab and place the first selected symbol on canvas
4. With your cursor on canvas, select q on the keyboard, this will place the next symbol 1000mils to the right of first placed symbol
5. Select q on the keyboard several times until all symbol are placed on canvas
   • For large symbol placements, you can manually place one of the selected symbol than select q on the keyboard to start a new row
6. If the symbols start to overlap you could update shortcut key (Step 1) in middle of this process and select q on the keyboard afterwards, for example:
   • funckey q ix 2000

I am not sure what you are trying to do but if you are looking to place all the Package Symbols in the library on the canvas, this will still be a time consuming process even with the shortcut key.

Alternative: Seeing that you don't have a schematic, you could add the Components to a Part List manually (Logic > Part Logic) and just use Quickplace to placement them all

1. Open the Parts List (Logic > Part Logic)
   
   • Enter Ref Des
   • Enter Device name (if it finds Device name in library it will populate the remaining info, click OK for message dialog)
   • Update Class to indicate component type
   • Select Physical Packages button
   • Optionally, enter Value and Tolerance values
2. Click Add button
3. Repeat steps above for each addition component

Hope this helps,
Mike Catrambone

mcatramb91 said:

I am not sure what you are trying to do but if you are looking to place all the Package Symbols in the library on the canvas, this will still be a time consuming process even with the shortcut key.

The goal is to place all the components in order to have the report that says which pads are used on which components.
Thanks for the answer. Where do I found the Parts List menu on PCB Editor ?

Hi,

Part List dialog is available with Allegro PCB Designer by selecting Part Logic under the Logic Menu.  I just checked and it appears that the command is not available in OrCAD PCB Designer which I got a feeling you are using.

If you have the Productivity Toolbox option, there is a routine that generates PDF File for components in the library.  It places multiple components on each sheet with expanded details on each symbol, including Padstack Names.

This may actual work for you.

• OrCAD PCB Designer = Export > More > PCB Library Plot... (Orcad Productivity Toolbox option)
• Allegro PCB Designer = File > Export > PCB Library Plot...   (Allegro Productivity Toolbox option)

Hope this helps,
Mike Catrambone