Exporting Gerber Files from NI Ultiboard

Publish Date: Dec 08, 2008 | 7 Ratings | 3.43 out of 5 | Print | 1 Customer Review | Submit your review

Overview

When the design of a printed circuit board (PCB) is complete, the design needs to be sent to a PCB manufacturer to be physically fabricated. Rather than send the entire design file, manufacturers require an industry standard file format to be used in their fabrication process. The standard format is called a Gerber file.

NI Ultiboard exports to the Gerber format. Gerber files effectively break down a board into its various layers providing computer controlled fabrication machines the exact design patterns to be drawn upon the fabricated board.

The Gerber file contains information (on a layer-by-layer basis) of the board outline, land patterns (footprints), drilled holes, vias, copper routes, and any other information that is required by the board manufacturer to create a board.

This article dicusses how to export a Gerber file from NI Ultiboard, and investigate the various options in the export dialog box.

Table of Contents

  1. Introduction
  2. Gerber Files
  3. The Export Dialog
  4. Exporting a Gerber File
  5. Viewing the Gerber File

1. Introduction

Exporting a file refers to taking a CAD representation of a PCB (as can be seen in your Ultiboard file) and producing an output in a format that can be understood by the fabrication equipment at the board manufacturer. There are many different manufacturing techniques used to produce PCBs and Ultiboard can produce a wide variety of outputs to meet these needs.

 

Export and Manufacturing

It is important to talk to your production house and identify all the files and formatting information they need to support their manufacturing process.

You can export a file in the following formats:

  • Gerber photoplotter 274X or 274D
  • DXF
  • 3D DXF
  • 3D IGES
  • IPC-D-356A Netlist
  • NC drill
  • SVG (Scalable Vector Graphics)

You can also export text files that contain:

  • Board Statistics
  • Part Centroids
  • Bill of Materials

You can also create reports on:

  • Copper Amounts
  • Test Points
  • Layer Stackup

 

Back to Top

2. Gerber Files

A Gerber file is a standard file format that contains information necessary for the computer controlled machines used by PCB manufacturers to exactly replicate CAD-based design patterns. The patterns usually contains features such as the board outline, land patterns (footprints),  drilled holes, vias, copper routes, and any other information that is required by the board manufacturer to create a board.

PCB manufacturers currently use two Gerber formats, the RS274D and RS274X. The current industry standard is the RS274X format, because these files provide a complete set of manufacturing instructions including the routing patterns and land patterns as well as the aperture settings.

NI Ultiboard has a standard Export dialog box to export a set of Gerber files.

 

Back to Top

3. The Export Dialog

The Export dialog box is a simplified dialog box that you can use to establish the different parameters required by different manufacturers for the final file export.

This tutorial uses a shipping example to showcase the export process.

  1. Select File >> Open Samples.
  2. Select Intl4lRouted.ewprj.
  3. Click on the Open button.

You are now ready to view the export dialog box.

  1. Choose File»Export. The Export dialog box appears as seen in Figure 1 below.

You can see in the dialog box the various types of formats and reports that can be exported from NI Ultiboard for manufacturing purposes. This tutorial focuses primarily on the Gerber RS274X options, as this is one of the most common outputs for manufacturing purposes.

Figure 1. Export Dialog Box

 

Back to Top

4. Exporting a Gerber File

With the Gerber properties (RS274X or RS274D) dialog box, you can select the layers to be exported, the number of digits in numerals, and the kind of measurements.

  1. In the Export dialog box select Gerber RS274X and click the Properties button.

In Figure 2 below, you can see the various parameters that can be set to configure your Gerber file export.

Figure 2. Gerber File Export

 

As can be seen in the figure above, there are a number of different parameters that must be set to properly export your design to the Gerber format. In Table 1 below you can see a description for each export option.

 

Table 1. Gerber File Parameters

Option What Is This Setting For?
 Available Layers  Set the layers of the design that are to be exported.
 Units  Set or change the measurement unit. There are two options,
either metric (mm) or imperial (mil).
 Digits  Set the number of digits of precision for board measurements.
 Oversize  Top Soldermask  Add incremental size to the soldermask on the top layer to  
increase the real-estate available to solder SMD parts.
 Bottom 
Soldermask
 Add incremental size to the soldermask on the bottom layer to  
increase the real-estate available to solder SMD parts.
 Solderpaste  Add incremental size to the solderpaste layer.
 Options  Open Pad Holes  Open up the pad holes on the design (a requirement by some
manufacturers)
 Reflection  Set a mirror image of the board design.
 Board Outline  Include the board outline on each exported Gerber file layer.
 Negative Image  Invert all the colors on the board.
 Allow
Nonconvex
Polygon
 Check this box if the design contains complex polygons.
 Merge Polygons  Merging of the polygons is a requirement by some manufacturers.

 

Selecting Layers to Export

  1. To select the layers to export to Gerber format, you can left-click on the name of each layer in the Available Layers selection box. To select multiple layers at once, hold down the <CTRL> key while selecting.

The following are typical Gerber files needed to produce the board:

  • All copper layers
  • Soldermask Top/Bottom
  • Silkscreen Top/Bottom
  • Board Outline

Once you have selected all of the necessary layers, click the right arrow (highlighted in red in Figure 3 below), to add the selection to the Export Layers list.

Figure 3. Selected Layers

With the layers selected (and any other option set, such as units, digits, options, oversize, and so on) you are ready to export the Gerber files.

Click on the OK button to save the settings and exit the properties dialog box.

 

The Export Process

  1. To finally export the various layers of your design, click on the Export button in the export dialog box (as seen in Figure 1).

Ultiboard directs you to the Create aperture mapping dialog box (Figure 4). For Gerber RS274X files, there is no need to edit the aperture settings as they are automatically set by the export process.

Figure 4. Aperture Mappings

  1. Click on the OK button to finalize the export.
  2. Ultiboard directs you to save the exported gerber file. Select a destination folder and click on the Save button to finalize the location of the export.

Ultiboard now cycles through all the layers, and allows you to set the aperture settings and file locations for each layer of the design. This means repeating Steps 8 and 9 for each layer.

 

Back to Top

5. Viewing the Gerber File

Ultiboard includes a built-in Gerber Viewer that you can use to verify the production files created. 

  1. Simply go to File»Open and select a generated Gerber files.
  2. Click on the Open button.

You can now view the exact file that the manufacturer views, as can be seen in Figure 5 below.

Figure 5. Gerber Viewer

 

Back to Top

Customer Reviews
1 Review | Submit your review

Export options for NI Ultiboard  - Jul 25, 2012

Export options for NI Ultiboard. What are the formates in which we can export /save the layout database? Is ODB++ supported?Or any other ascii format supported?

Bookmark & Share


Ratings

Rate this document

Answered Your Question?
Yes No

Submit