To generate Gerber & NC Drill files from OrCAD (Cadence Allegro) PCB Editor, Open the native file (.BRD) in OrCAD PCB Editor;

Gerber Files: From the Editors window, go to Manufacture > Artwork; on the Artwork Control Form, click on the General Parameters tab to make active and then confirm the following settings:

Device Type ~ Gerber RS274X
Film Size Limits ~ 14 x 16

Leave remaining default settings to keep outputs consistent. 

Global Visibility OFF apply

Board Geometry Outline ON

Go to Display -> Visibility on the PCB Editor Main Window. Select Global Visibility to All Invisible, an option on the top-right of the pop-up window that opens. Then select Group -> Geometry on the top-left, and turn on Board Geometry -> Outline. Click OK.

Go to Manufacture -> Artwork. Artwork Control Form opens. On the bottom, click on Apertures, then Edit, then Auto -> Without Rotation. Click on OK and go back to the Artwork Control Form.

Right-click on a film in the Available Films Window and select Add (don't use the Add... button). Name the new film as BoardOutline. Click on OK.

Go to Display -> Visibility and turn off all layers except SoldermaskTop (Stack-Up -- Non-Conductor). Go to Manufacture -> Artwork and create a film layer with that name, similar to what you did for BoardOutline. 

Repeat the steps for:
  SoldermaskBottom
  SilkscreenTop (Board_Geometry, Components_RefDes, Package_Geometry)
  SilkscreenBottom (Board_Geometry, Components_RefDes, Package_Geometry)
  DrawingFormat (Drawing_Format all ON, Board_Geometry--Assembly_Notes--Outline, Manufacturing--Nclegend1-4)

*********** !!! *********
On the right side of the Artwork Control Form, set undefined line width to 10 mils for all film layers.
*********** !!! *********


Now, click on the Film Control tab and choose Select all from the bottom of the Available Films section and then Create Artwork. Choose OK to close this window. The artwork (Gerber files) should now reside in the MANUFACTURING folder ( beneath the " allegro " folder ).

Click on Viewlog to see if there are any errors or warnings; correct them if there are any.

Fire up GC-Prevue, import *.art. ( Alternative method: create a new board in PCB Editor window and import all artwork layers from File -> Import -> Artwork and check if they look good. )

---0---

NC Drill File : From the Editors window, go to Manufacture > NC > NC Drill. The NC Drill dialog box will open. Confirm that the root file name is present (board name.drl) and choose 'Auto Tool Select'. Leave remaining default selections. Click on the Drill button to generate the NC Drill file. 

---0---

Route Path Files:

Create text file " ncroutebits.txt "; save in Gerbs folder  eg: 0.100  T01.
Cut Marks, create shape from board outline lines.  Manufacture > Cut Marks.
Draw Cut Path on Board Geometry, Ncroute_Path subclass, add line, width same as tool size.
Generate " NC route file " Manufacture > NC > NC Route ...

---0---

File >Export >IPC_356; set the IPC Version (IPC-D-356 or IPC-D-356A) and other options such as output name and then select 'Export"

---0---

Placed Components Report for Pick and Place
Tools---Reports---
 Top text list; double-click "Placed Component Report"
 Check Boxes: Write Report and Display Report
 Click the "Report" button
 Look in the allegro directory of the project for file "pcp_rep.rpt"
 Fire up Microsoft Excel
 Import the file as comma separated values
 Edit the columns as appropriate
   Editing ... Find and select ... Change NO to TOP ... Change YES to BOTTOM
 Save the Excel file for the assembly house

---0---

For 1:1 paper plot check
  Make gerber file of top/bottom cu 
  Import into GC-Prevue
    Print Setup -- Page Setup -- Page Layout: 1 on 1
     CheckBox: Manual Scaling
       Scaling: 100%
    OK -- OK
  File Print
    Print Setup dialog box opens
    Layers to print: Visible
    Format: Board 1:1
    Print separate page(s) for each:
      Physical Layer
    Print all data in black
    Center data in print area
  OK -- OK