News
Home / News /

Generate Gerber File from Cadence Software

0

Published by Pinsheng Electronics Co., Ltd March 11,2020

Gerber file is the standard format for PCB manufacturing, the common extension is .gbr. The designers can output the .gbr files from various software, such as Altium Designer, Allegro SPB, Orcad, Kicad, Eagle, and so on. In which, Allegro and Orcad belong to the same company Cadence, who is one of the leaders in the EDA industry.

The interfaces and operation methods of Allegro and Orcad are almost the same, the difference is that Allegro is to advanced design, while Orcad is to med & low ends design, limited but cheaper. 

Interface of Allegro
Allegro

 

Next, follow me to export Gerber file from Allegro/Orcad step by step.

1. Before exporting the Gerber file, check the parameters of the drawing, the stack-up, the copper traces, and check the DRC report, which will help you to output Gerber file correctly.

1.1 Design Parameters

  • The unit selected in the setup should be consistent with the unit set in Gerber, as well as the accuracy

  • In order to guarantee WYSIWYG in Gerber, check the three boxes as shown

Generate GERBER file from Allegro Figure 1

1.2 Copper Parameters

  • Select "Shap" tab

Generate GERBER file from Allegro Figure 2

  • Click the button in the red rectangle, it will fill in/cut out the copper area automatically
  • In the "Void Controls" tab, select "Gerber RS274X"

Generate GERBER file from Allegro Figure 3

1.3 Stack-up Parameters

  • Click "Setup Cross Section", as shown

Generate GERBER file from Allegro Figure 4

  • Check the stack-up parameters carefully

1.4 DRC Check

  • Select "Display-Status",
  • Click "Update DRC" to run DRC
  • Click "Update to Smooth" to verify the setup errrors, if it is a gray botton, the copper parameters are correct

Generate GERBER file from Allegro Figure 5

1.5 Darebase Check

  • Click "Tools-Database Check"

Generate GERBER file from Allegro Figure 6

  • Check the three boxes as above, click "Check"

 

2. Folder and path of outputting Gerber file

  • Select "Setup-User Preferences Editor"
  • Select "Output_dir" in the red box on the left, then enter the name of the folder for exported Gerber file in the red box on the right

Generate GERBER file from Allegro Figure 7

  • Then select "Temp_file" in the left red box and enter the export path in the right input box

Generate GERBER file from Allegro Figure 8

3. Gerber file output

  • Select "manufacture-NC-NC Parameters",

Generate GERBER file from Allegro Figure 9

  • In the above figure, except for "format" and "output unit" should be adjusted according to the situations, the other parameters are kept as default. NC data (.txt) will be generated after clicking the close button
  • Select "Manufacture-NC-Drill Customization", which will list all the drilling information currently used

Generate GERBER file from Allegro Figure 10

  • Click on the red box 1 in the above picture, allegro will automatically assign symbols to the holes on the current circuit board. Click on the red box 2, check all the drilling pads information. Click on the red box 3, the drilling information will be saved to the output Gerber file
  • Select "Display-Color/Visibility", click the "Global Visibility Off" button in the upper right corner to close all layer displays

Generate GERBER file from Allegro Figure 11

  • Then open the OUTLINE layer alone
  • "Manufacture-NC-Drill Legend", all are kept as default except for the boxes in the red rectangles

Generate GERBER file from Allegro Figure 12

  • Select "File-Viewlog" to check whether there are errors or warnings during generating the drilling data

Generate GERBER file from Allegro Figure 13

  • Execute "Manufacture-NC-NC Drill"

Generate GERBER file from Allegro Figure 14

  • Check the options in the three red boxes in the above figure, then click "Drill"
  • Select "Manufacture-NC-NC Route", just click "Route" to generate the required milling file

Generate GERBER file from Allegro Figure 15

  • Select "Manufacture-Cross Section Chart", leave the setting default, then click "OK", the cross-section data will be hung on the mouse, you can place it on the appropriate location

Generate GERBER file from Allegro Figure 16

  • Select "Manufacture-Artwork", then select "Film Control" tab, check all the options in the red box 1 and click on the button in red box 2, which will generate the artwork file

Generate GERBER file from Allegro Figure 17

  • Come to "General Parameters" tab in the above figure, leave it as default

Generate GERBER file from Allegro Figure 18

  • In the "Film Control" tab, ensure there are 3 layers in each folder

Generate GERBER file from Allegro Figure 19

  • Then keep this window display while select "Display-Color/Visibility", please click "Global Visibility Off" to disappear the other layers and then display the outline layer manually, click "apply"
  • Back to the "Film Control" tab, hover mouse upon any electrical layer, right-click, select "add", enter "outline" in the input line, "OK" then the displayed outline layer has already been added to the available films
  • Similarly, turn off the display of all layers, open the display color manager, as shown, check "Pin" and "Via" in the Pastemask_Top layer, while "Pastemask_Top" box under "Package Geometry", then click "OK" to exit. Go back to the "Film Control" tab and create a new folder named "Past_Top"

Generate GERBER file from Allegro Figure 20

  • Again, create a new folder "Past_Bottom"
  • Note that when creat "Sold_Top" and "Sold_Bottom" folders, one more step is needed, check "Soldermask_Top" and "Soldermask_Bottom" under "Board Geometry" directory in the color display manager

Generate GERBER file from Allegro Figure 21

  • Then create "Silk_Top" and "Silk_Bottom" folders in the same way, please check silkscreen layers in the color manager

Generate GERBER file from Allegro Figure 22

Generate GERBER file from Allegro Figure 23

Generate GERBER file from Allegro Figure 24

  • Add the drilling data in the same way as above
  • Generate the capture range, select "Setup-Areas-Photoplot Outline", and draw a box that contains all the data

Generate GERBER file from Allegro Figure 25

  • Finally, select "Manufacture-Artwork", click "Select All", then "Create Artwork", the required Gerber file will get generated in the output folder

Generate GERBER file from Allegro Figure 26

 

What design software do you use? Can you get the Gerber file easily? Please feel free to contact PS Electronics if you need assistance in your circuit board design or fabrication.

< >