copy/paste of wiring from refernce design > Forums

Forums

Subject: copy/paste of wiring from refernce design

Posting to forums is available to community members only.
Login or Register

Rate this topic:

Author

Messages

purikku
Posts: 20
Online: User is Offline

6/30/2008 8:20 PM
another question, is there a way that i could copy/paste a portion of wiring from a reference data (eg LVDS patterns) to the current design? (the reference and current design has the same placement and parts list for the LVDS part but differs in DDR, its like a revision project).What to do? thanks. regards, eric

Trykon
Posts: 58
Online: User is Offline

7/01/2008 4:05 AM
o In the reference design select File > Export > Subdrawing. o Enable the elements you would like to copy in the Find Filter e.g. clines and vias. o Using your left mouse button select, using window or by selecting elements, the items you want to copy. o Select a point, such as a pin or XY location (You can type it at the Allegro command line) to use as a reference or origin for the elements in the reference design. Allegro's command line will state "Pick clipboard origin point" o Save the drawing (.clp) file. o In the current design select File > Import > Subdrawing. o Browse to the saved drawing and select it. It will be attached to the cursor. o Place the clip file at the correct location.

LM_Roger
Posts: 2
Online: User is Offline

7/01/2008 8:22 AM
When you do this action, is connectivity still established? I ask because I have done this; however, when I update the netlist (import), it looks like the components in the subdrawing are not being included in the connected nets statistics and the placed components statistics. What about reference designations as well? Do they need to be the same in the new source schematic? I appreciate the help very much! I am adding a reference design to an existing board and this very topic is absoutely current with my existing task. Thanks very much!

Trykon
Posts: 58
Online: User is Offline

7/01/2008 8:28 AM
When you are in the export command you have the options of preserving: Refdes Nets of shapes Vias Testpoints on vias That being said the connectivity, including the refdes has to be in the logic imported. The connectivity, provided the logic is in the design, should establish. I would import the logic prior to importing the subdrawing.

LM_Roger
Posts: 2
Online: User is Offline

7/01/2008 8:33 AM
Just so I am clear...I think this is the order I should follow: 1. Import the Reference Design Logic (schematic net list) into the board file. 2. Import the subdrawing into the board file. 3. As long as REF DES; connectivity is the same, then the connectivity should be established? I plan on copy/pasting the schematic from the reference design into my new schematic, so preserving REFDES, etc. will be no issue. I will try this and let you know if there are any issue. Thanks VERY much for the tip. That will save a lot of time/effort.

Trykon
Posts: 58
Online: User is Offline

7/01/2008 8:53 AM
If the refdes and the connectivity is the same in both designs then yes, your list of the order would be what I would do. Good luck.

cadpro2k
Posts: 45
Online: User is Offline

7/01/2008 9:43 AM
One thing to try: Once you've pasted the "copied" connect lines into your design (provided you have the exact placement as the 'copy from' database); go to Tool/Derive Connectivity. This should reconnect all the clines you've copied into the new placement. Give it a try. Good day. Mitch

purikku
Posts: 20
Online: User is Offline

7/01/2008 5:55 PM
minnasan, arigatou gozaimasu! thanks a lot... Good day, eric

Posting to forums is available to community members only.
Login or Register

Forums > Silicon-package-board > PCB Design > copy/paste of wiring from refernce design