Stats

  • State Not Answered
  • Replies 2
  • Subscribers 165
  • Views 313
  • Members are here 0
More Content

De assign netname for multiple pins at same time in allegro

Sriranga

We can assign the netname to the multiple pins at a same time by using following option( file- import- logic) in PCB editor.

As like that I need to de-assign the multiple pins from different nets.Is there any default option?

For dense board if need to de assign the netname for multiple pins, currently i am deleting entire nets and then I import the netlist...this process give lot of reworks. If anyone have solution for this please give your guidance.

Parents
  • +1

    Hi Sriranga,

    You can de-assign pins from their existing nets using the steps outlined below:
    1. Choose Logic → Net Logic from the top menu.
    2. In the Options tab, select the Deassign radio button.
    3. (Optional) Enable Ripup Etch/Conductor if you want the connected traces to be removed automatically.
    4. In the Find filter, ensure Pins is selected.
    5. Click individual pins or drag a window to select multiple pins.
    6. The selected pins will be removed from their current nets and assigned to a dummy net.
    7. Right-click and select Done to complete the operation.
    If you later need to assign the pins back to a net, you can follow the same procedure and select the Assign option under Logic → Net Logic, then assign the desired net name to the selected pins.
    I hope this helps. 

Reply
  • +1

    Hi Sriranga,

    You can de-assign pins from their existing nets using the steps outlined below:
    1. Choose Logic → Net Logic from the top menu.
    2. In the Options tab, select the Deassign radio button.
    3. (Optional) Enable Ripup Etch/Conductor if you want the connected traces to be removed automatically.
    4. In the Find filter, ensure Pins is selected.
    5. Click individual pins or drag a window to select multiple pins.
    6. The selected pins will be removed from their current nets and assigned to a dummy net.
    7. Right-click and select Done to complete the operation.
    If you later need to assign the pins back to a net, you can follow the same procedure and select the Assign option under Logic → Net Logic, then assign the desired net name to the selected pins.
    I hope this helps. 

Children
  • 0 in reply to vidhyaparameswari

    Thanks, Vidhya.

    Using the Filter option, I was able to generate the .qfnd file. I then edited the QFND file and specified the pins from which I needed to deassign the net name.

    Based on the pins listed in the QFND file, I removed the net name only from the particular pins without removing the entire property associated with the net.

    I also received a script from my colleague to deassign the net name from the selected pins X & Y location.  The script is as follows:

    setwindow pcb
ifp
net logic
setwindow form.find
FORM find all_off
FORM find pins YES
setwindow form.mini
FORM mini deassign YES
setwindow pcb
pick 11 12
pick 12 13
pick 13 14
pick 14 15
pick 15 16
pick 16 17
pick 17 18
pick 18 19
pick 19 20
pick 20 21
pick 21 22
pop Done

    This approach allows us to deassign the net name from specific pins without affecting the other properties related to the net.

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.