changing footprint on PCB editor

 No schematic means no netlist so you won't be able to drive logic into the design to change that part, but you could do it manually. Unplace the bad foot print and manually drop the new one, but then your flying blind without rats to guide your trace routing. place>manually>placement list>drop package symbol.

 You can derive a netlist from the design and then edit the exported netlist and change the pcb symbol. As noted above your schematic and netlist woudl be ouot of sync.

To do this follow these steps

1. File >Export Netlist w/properties. This will create a text file which you will edit.
2. File >Export > Libraries. Select all and then 'Export'. This is to ensure you have all needed files when importing the new netlist.

Edit the netlist text file with an editor of your choice. Ensure that the editor you are using doesn't inset formatting characters. I typically use Textpad. Change the PCB symbol in the packages section. If I wanted to change a DIP14 for an SOIC package for the refdes U96 an example snipit would be

$PACKAGES
CAP300 ! 'FCAP-1' ; C1 C2 C3
DIP14_3 ! '74LS00-2' ; U96
DIP14_3 ! '74LS74-2' ; U69
DIP20_3 ! '74HC541-1' ; U1

to:

$PACKAGES
CAP300 ! 'FCAP-1' ; C1 C2 C3
SOIC_14 ! '74LS00-2' ; U96
DIP14_3 ! '74LS74-2' ; U69
DIP20_3 ! '74HC541-1' ; U1

You will also need to edit the device file for the package. In this example the device file for U96/DIP14_3 is "74ls00-2.txt" and inside that file you will see the package symbol DIP14_3 called out. If this is the only package using this device file you can chage just the PACKAGE line and then inport the netlist

 (DEVICE FILE: 74LS74-2)

PACKAGE DIP14_3

 An alternative to changing the PACKAGE in the device file is to add an ALTERNATE_SYMBOLS line in the text file for the device. The "ALT_SYMBOLS" line allows you to place an alternate symbol when the symbol is selected from the Place Manually form using the right mouse button.

You would need to include a similar line in your device file as:

 PACKAGEPROP ALT_SYMBOLS '(B:SOIC_14)'

Once you have the netlist and device file editied and saved you import the netlist using File >Import >Logic.
Select the "Other" tab and check 'Supersede alllogical data' to overwrite the netlist in the design.
Select "Import Other".

You should now be able to place the other package

#########

Example device text file:

(DEVICE FILE: 74LS74-2)

PACKAGE DIP14_3
CLASS IC
PINCOUNT 14

PINORDER '74LS74-2' '-CL' '-PR' '-Q<0>' CLOCK 'D<0>' 'Q<0>'
PINUSE '74LS74-2' IN IN OUT IN IN OUT
FUNCTION G1 '74LS74-2' 13 10 8 11 12 9
FUNCTION G2 '74LS74-2' 1 4 6 3 2 5

GROUND GND ; 7
POWER A5NEW_VCC ; 14

PACKAGEPROP ALT_SYMBOLS '(B:SOIC14)'
PACKAGEPROP INSERTION_CODE D
PACKAGEPROP MAX_POWER_DISS '0.2'
PACKAGEPROP PART_NUMBER 1234

END

 If you have a performance license you can change the footprint within Allegro under logic->part logic.

I tried Rik Lee's method and my problem is solved now. Thank you Rik and all!!!

Even If the question was answered some time ago, I reply with another method that is really simple and does not involve modifications to netlist. Do the following:

1) Create your alternative footprint and place it into a new folder, located somewhere. Say, for example, C:\My_Design_path\My_Library

2) Rename it with the same name of the "old" footprint you want to replace.

3) Add the new folder to your User Preferences->Paths->Library->psmpath and place it to the top of the list. This will allow PCB Editor to search for symbols in the new folder for first.

4) Do Place->Update symbols and select the symbol you want to replace. When PCB Editor will search for symbols, it will find the new footprint for first and stop the searching. Now You have updated your symbol without changing netlist.