Gerber Translator

The Gerber Artwork Translator can translate artwork directly from circuit layouts created with Advanced Design System into Gerber format. It exports ADS layouts into ASCII files that control Gerber photoplotting equipment.

The Gerber Viewer is a companion program included with the ACS Gerber translator. The Viewer is used for viewing artwork on a computer monitor and for printing it to a graphics printer before creating artwork on the Gerber photoplotter. It is also used for generating drill data and tooling reports.

The Gerber Union tool is also available within the Gerber Viewer. This tool requires a separate license from the Gerber export license. The Gerber Union tool provides the ability to import Gerber files into ADS. It can create EGS Archive files from a set of Gerber files which can then be imported into ADS.

Gerber Command Format

The Gerber format is a numerical control language developed to generate photo artwork. The output of this translator is an ASCII file that contains the following Gerber commands:

G01E = linear interpolation
G54 = aperture select
D01 = shutter open
D02 = shutter close
D03 = flash
M02 = end of program
X and Y = coordinates
* = end of block

Coordinates are absolute, with implied decimal point and optional leading zero suppression. However, the literal string values may be modified in the message file. For example, G01 may be changed to AB. A sample listing of the Gerber file commands, with interpretation to the right, might look like this:

This example would produce the following figure.

The output files are:

The photoplotter vendor receives both output files.

Importing Gerber Files

Gerber files can be imported into ADS layout by following a two step process. First, one or more Gerber files are converted into a single EGS Archive file using the Gerber Union tool. This EGS file is then imported into ADS layout.

Note
Only Gerber RS274X files can be processed by the Gerber Union tool.

A layer will be created for each Gerber file that is imported. The names of the layers created will be "1", "_2", "_3", ..., "_n". The layer table (_File > Layer) in the Gerber Viewer will show how the Gerber files are mapped to each layer number. This is the default behavior when using the option Multi-Layer Output. Changing this option to Single-Layer Output places all elements on the layer "_1".

To import Gerber Files into ADS layout:

  1. In the Layout window, select File > Import.
  2. Set the File Type to Gerber Viewer and click OK, this invokes the Gerber Viewer tool.
  3. When the Gerber Viewer (GBRVU) opens, a browser window entitled Open GRB File appears. This window enables you to browse to the folder containing the Gerber files. Select the Gerber file(s) you wish to use and click Open. This dismisses the Open GRB File window and moves the Gerber Viewer tool to the foreground, enabling you to view the contents of the file(s).
  4. Select Tools > Gerber Union from the GBRUV window. A dialog appears with the following options.
  5. Setting the Gerber Union options:
    Settings Use Multi-Layer Output to generate a layer for each Gerber file imported. Use Single-Layer Output to place all elements on the layer "_1".
    Window Specifies an area of the Gerber files to import by defining its region here.
    Output Defines the units and scale of the output EGS Archive file.
    Output File Name Destination path and filename of the EGS Archive file.
    Note
    Details on all options can be seen by clicking the Help button in the Gerber Union options dialog.
  6. Set the options as desired, then select OK to create the EGS Archive file.
  7. Close the Gerber Viewer tool.
  8. In the layout window, select File > Import.
  9. Set the File Type to EGS Archive.
  10. Select the file to import and click OK.

Exporting Gerber Files

ADS Release 2008 contains a simplified Gerber export tool. This tool can generate Gerber files in RS274X and MDA format for raster photo plotters. For instructions on using MTools to export Gerber files, see Exporting Gerber Files Using MTools.

The Gerber export tool creates one output file for each different layer used in the layout design. For example, if the design contains two layers, cond and cond2, two Gerber files will be generated:

To export Gerber files:

  1. In the layout window containing your design, choose File > Export.
    The Export dialog box appears.
  2. In the File type field, select Gerber.
  3. To define export options, click More Options.
  4. Set the options that apply.
    For available options, see Gerber File Options.
  5. Click OK to save your settings or Cancel to retain the default settings.
  6. In the Destination Directory field, accept the default directory, or click Browse to locate a new destination directory.
    The destination directory will be the <Project Dir>/mfg/<Design Name>/gerber/
    where:
    <Project Dir> is the project directory
    <Design Name> is directory named with the design name
    The checkbox option View file after export is not applicable for the Gerber file type.
  7. Click OK to export the ADS layout design to a Gerber file.
    A Status window appears detailing the export information.
  8. Examine the log, searching for any warnings or errors that may have occurred during translation.
    To save the log message in a file: select the text, copy, and then paste into any text editor.

Gerber File Options

You can view or edit the translator settings, by clicking More Options in the Export dialog box.

The Export Gerber Options dialog appears, providing access to these options.

Gerber file choices can be edited in the Options tab.

File format

Hole format

In ADS, when a hole is created in a geometrical figure (like polygon), a cutline is introduced. This is a false edge connecting the outer boundary of the polygon with the inner boundary. This polygon is actually a single re-entrant polygon. When you select Holes as cutlines this re-entrant polygon is translated to Gerber as-is. The default is Holes as cutlines.

Holes as Cutlines

Select Holes as polygons or Preserve holes to remove the false edge from the polygon.

Holes as polygons

When Holes as polygons is selected, holes are exported as filled elements. Therefore the polygon will appear to have no holes.

Preserve holes


When Preserve holes is selected, the resultant polygon in Gerber contains a dark area and empty area. This option is not available for exporting Gerber files in RS274X format.

Unit

Available units are inch or mm. Inch is the default.

Number format

The number of integers placed before and after the decimal point. If chosen incorrectly, Gerber data resolution can be poor. The default is 2.4. If the unit is set to mm then you can set the number format to 3.3.

A warning message is displayed in the Status window to notify the user that to preserve the precision in the Gerber data, number format has to be selected carefully. If the Gerber data is not generated correctly for the selected number format then a suitable error message is displayed in the Status window.

Zero suppression

Available settings are Leading and None. Select Leading (the default) to remove all leading zeros in the coordinate data, making the Gerber file smaller.

Line width for polylines

Polylines in ADS have zero width, but you can use this option to provide a width to be used for drawing this polyline in the Gerber file.

If the polylines and arcs (both zero width entities) are not required to be exported, then set the width to zero.

Generate single file

When this checkbox is selected, a single file is generated for all the selected layers in the Layer tab. Specify the file name with extension .gbr. This file will be created in the destination directory selected in the Export dialog box.

Gerber Layer Options

All the layers used in the design are displayed in a table in the Layers tab of the Export Gerber Options dialog. By default, all the layers will be displayed with positive polarity and all layers will be exported. You can avoid exporting a specific layer by deselecting the checkbox in the Export column for that layer.

Limitations and Considerations

Exporting Drill Files

In ADS 2008, drill file export is accomplished simultaneously as part of the Gerber export. The procedure for generating the drill file is similar to generating the Gerber file.

Drill files are configured from the Drill tab in the Export Gerber Options dialog.

Select the checkbox to designate the layer for which you want to generate the drill file. When a layer is selected, all the tools on that layer are automatically selected. By default, no drill file will be generated during Gerber export.

The drill file options Number format, Output unit, and Zero suppression are same as options set for Gerber export in Options tab of Export Gerber Options dialog. However, note that the zero suppression in Drill is actually a zero inclusion.

Tool Dia. (Diameter) is an editable field. By default the Tool Diameter value equals the Drawing Diameter value.

Considerations:

Exporting Gerber Files Using MTools

The ADS-to-Gerber translator creates one output file for each different layer used in the layout design. For example, if the design contains two layers, cond and cond2, two Gerber files will be generated:

cond.gbr
cond2.gbr

In ADS 2002C and earlier versions of ADS it was not possible to perform multiple Gerber translations in a project, as these filenames would be overwritten. However, starting with the ADS 2003A release it is possible to specify a destination folder for each Gerber file, allowing for multiple translations in a single project.

To export Gerber files:

  1. In the layout window containing your design, choose File > Export.
  2. The Export dialog box appears. In the File Type field, click the arrow in the right-hand corner to display the available formats. Select Gerber.
  3. To define export options, select More Options. Set the options that apply. For available options, see Export Gerber Options. Click OK to save your settings or Cancel to retain the default settings.
  4. In the Destination Directory field, accept the default directory, or use the Browse button to locate a new destination directory.
    Note
    If you generate Gerber files for more than one design in the same project, you need to specify different destination folders to avoid overwriting common files (i.e., layers common to most projects like cond and cond2).
  5. Click OK to accept the settings. The status window appears:

    The entry Mask to Gerber displays under the heading Activated Modules. The Gerber translator converts your design into a mask file before outputting it in Gerber format.
    The option Keep History is selected as the default. When this option is selected, the preferences you specify are saved and used as the default for future translations. If you do not want your settings saved, deselect this option.
    Click OK to proceed. The Mtools Log and Gerber Translator Interface window appear.
  6. Verify that the Mtools Log contains the correct information. If necessary, edit the information. To dismiss the Mtools Log window, click OK.
    Note
    You may view the Mtools Log at any time by clicking the GERBER tab in the translator interface window.
  7. In the Gerber Translator Interface window, set the Mask Files and Aperture File paths. The Mask Files field displays the mask file created in the Export dialog box. This is the file that the Gerber translator converts into Gerber format.
    The Aperture File field displays the configuration file used to hold all of the translation parameters and Gerber apertures. When performing a translation, you can create a new configuration file or reuse the same file. To modify this file, see Gerber File Options.
    To view the Mask Files and Aperture File paths, click the adjacent Browse button.
  8. Select Gerber File Options , Translation Settings , and Edit Apertures to specify settings. Select View Mask to invoke the Gerber Viewer for DXF and Gerber translations and View Gerber for Gerber translations only. For details on Gerber translator interface options, see the appropriate section: Gerber File Options, Translation Settings, Edit Apertures, and Using the Gerber Viewer.
  9. Click Translate to select the layers you want to include in the translated file (see Translate). After selecting the layers, click OK to complete the translation. A window appears briefly, indicating that the file is being converted to Gerber format.
  10. When the translation is complete, the Mtools Log appears, detailing the export information. Examine the log file, searching for any warnings or errors that may have occurred during translation.

When you are finished viewing the log file, click OK to dismiss the MTools Log and exit the Gerber translator.

Gerber File Options

You can view or edit the translator settings, by selecting Gerber File Options in the Gerber Translator Interface window.

A dialog appears, providing access to these options:

Gerber Unit. Available units are INCH or MM. MM is the default.

Format. The number of integers placed before and after the decimal point. If chosen incorrectly, Gerber data resolution can be poor. The default is 3.3.

Zero Suppress. Available settings are Leading and None. Leading (the default) removes all leading zeros in the coordinate data, making the Gerber file smaller.

If the setting is inappropriate, the Gerber data display is nonsensical.

Data Mode. The program always writes out absolute coordinates.

Circular. Available settings are 360 or Off. When Off is selected, arcs are fractured. When 360 is selected, arcs are written by means of GO2/GO3 with 360 interpolation. The default is 360.

EOB Character. Sets the character that denotes the end of a Gerber data block. Currently set as an asterisk (*).

EOJ String. This string, inserted at the end of the Gerber file, indicates that the plot is complete. Currently set as MO2.

CR/LF. Available settings are Include or Suppress. Some Gerber files include a carriage return/line feed (CR/LF) at the end of each command. When the CR/LF is suppressed, the file size is reduced by twenty percent and the translation is completed more quickly. Suppressing the CR/LF does not effect your ability to view the Gerber data in the Gerber Viewer. Suppress is selected as the default.

Note
After you have set these options, you do not need to do so again unless you deselect the Keep History option in the initial Mtools dialog (see Exporting Gerber Files).

Translation Settings

You can control how the program converts the mask data into Gerber format by selecting Translation Settings in the Gerber Translator Interface window. These settings, crucial to correct output, are described in this section.

Global Parameters

Line DCode. Open figures output to this D-code.

Scale Factor. Output data is scaled up or down according to this factor.

ArcRes. Value, in degrees, by which arcs are broken up.

APT Out. Drop-down list for selecting aperture output from popular CAM software.

Outline/Fill

Outline or Fill. Each closed area is either outlined or filled, depending upon selection.

Note
Maximum vertex count for polygons is 50k.
Note
When Fill mode is selected, large shapes will be chopped into blocks of 1000 pt Gerber polygons. When Outline mode is selected, large shapes will be chopped into blocks of 5000 pt Gerber polygons.


Compensation

Compensate for etch factor by the given inch amount, shrink or swell , as needed.

Output Offset

The Gerber data coordinates are moved by the amount defined in the X and Y fields.

Gerber Output Format

The flavor of Gerber output: standard RS274D, extended RS274X or MDA with the Autoplot header. Barco DPF is planned for the future.

Considerations

When setting the translation options, consider the following:

Edit Apertures

When you click Edit Apertures , a table listing the aperture settings appears.

Gerber files use apertures much like plotters use pens. Defining available photoplotter apertures is very similar to installing pens into a pen plotter carousel.

To insert a standard set of apertures into the list, click Add Default Set in the Aperture dialog box.

To add a setting, change a coordinate, or change an aperture type, click in the section you wish to change and enter the desired value. You can also change the aperture type via the Dcode dialog:

  1. Click the D-code number under the heading DCode. A dialog box appears, listing the available aperture types.
  2. Select the desired type and click OK. The dialog box disappears.

Among the available aperture types are POEX and POIN. These are special apertures for the FIRE 9000 laser plotter. This plotter can take outline data and fill the inside of each polygon. If you are using such a plotter, the D-codes should be defined for POEX and POIN and the translator should be run in outline mode (see Translation Settings). For more information about this plotter, see FIRE 9000 Photoplotter Configuration.

Cir/Rect/Poly allows you to flash specific shapes with fixed dimensions, and will bring up the Map Circles/Rectangles/Polygons dialog. When a shape is flashed it will only be defined once in the Gerber file. Every instance of the shape can be referenced in the Gerber file with only the x,y coordinates of its location. Flashing shapes in Gerber files reduces the file size and simplifies the output file.

Show Circles, Rectangles, Polygons check boxes can be used to filter the list of shapes. Unchecking a box will remove those elements from the list of shapes that can be flashed. The default postion is checked.
When the Min. Count On checkbox is selected, only shapes that have a minimum count specified in the field will be shown in the list of shapes that can be flashed. The default position is unchecked.
Polygons can be prevented from being processed by the boolean engine if it has the property DB_NO_BOOL and its value is 1.

To add this property to a shape:

  1. Select the shape.
  2. Select Edit > Properties.
  3. Type DB_NO_BOOL in the name field, with a value of 1 in the value field.
  4. click Add > OK.
    Note
    Selecting the Auto Flash button in the Aperture dialog will automatically add all elements that can be flashed to the aperture table, bypassing the Map Circles/Rectangles/Polygons dialog.
    When you are satisfied with the aperture settings, click Save or Save As , or click Cancel to return to the default settings. The Aperture settings window disappears.

Translate


The Translate button invokes the Select Translation Layers dialog. This dialog enables you to select the layers to be included in the translated file. (The Gerber translator creates a Gerber file for each layer in the mask file.) All layers are selected as the default.

Note
Layers are selected when they are highlighted.

To select or deselect a layer, click it. You may also choose Select All or Clear All.

To complete the translation, click OK. A dialog briefly appears, informing you that the mask file is being converted into Gerber format. When the translation is complete, the Mtools Log appears. Inspect the log to verify that the file was translated as expected. (To dismiss the log window, click OK.)

View Mask


The View Mask button invokes the Gerber Viewer to display the mask file. For information on the Gerber Viewer, see Using the Gerber Viewer.

View Gerber

Once the translation is complete, click View Gerber to launch the Gerber Viewer and load the Gerber file(s). The

Gerber Viewer enables you to view your file(s) and generate drill data.

Check the bottom of the Viewer window for messages or instructions.

For more information on the Gerber Viewer, see Using the Gerber Viewer.

Export Gerber Options

Units

These are the units that the Gerber file will be written in. You may select from the following options: same , mil , inch , um , mm , cm. The default is same. When same is selected, the design is written in the same units that are stored in the design file. For information on choosing layout units, refer to Setting Units/Scale Factors in the Customization and Configuration manual.

Scale X, Scale Y

These are the fields for inputting the scale factors for shapes in the direction of X and Y. The default settings are 1.0, 1.0.

Define Layers

Clicking the Define Layers button invokes the Layer Editor. For Layer Editor Options, see Defining Layers.

Layers Include, Layers Exclude

The Include and Exclude buttons enable you to specify layers to either include or exclude.

Layer Number(s)

The numbers of the layers to be included or excluded in the export process. Entries are separated by commas. For example:
1,6,20

Layer File Name(s)

The numbers and names of the layers to be included in the export process. The information must be presented in pairs, as follows:
<layer_number> <layer_name> <layer_number> <layer_name>...
where all are separated by spaces. For example:
1 msk1 3 msk3

Auto Merge

When Auto Merge is selected, all shapes for every mask layer that intersect or overlap are merged. This option is deselected as the default.

Arcs As Polygons

When Arcs As Polygons is selected, the design arcs are exported as line segments (or polygons). This option is deselected as the default.

Rectangles As Polylines

When Rectangles As Polylines is selected, all rectangles are translated as open plane figures bounded by straight lines. When this option is deselected, all rectangles are translated as closed plane figures bounded by straight lines. This option is deselected as the default.

Holes As Polygons

When Holes As Polygons is selected, holes are exported as a filled element, which is also how polygons are exported in the gerber format. When Holes As Polygons is not selected, polygons with holes are translated as single-segment polygons, the false edge segment becoming part of the polygon. Some systems may not be able to tolerate this type of complex polygon. For these systems, make certain that Holes As Polygons is selected. This option is deselected as the default.

Holes As Cutlines

When Holes As Cutlines is selected, holes are converted into cutlines. This option is selected as the default.

Preserve Holes

When Preserve Holes is selected, holes are exported as an empty element. This option is not available for exporting gerber files.

Etch Factor

The etch factor applies a global over/undersize amount to each shape translated. This is meant to compensate for etch effect during processing. However, using this option can be problematic. Thus, we recommend that you retain the default setting of 0.

If you use Etch Factor, carefully verify the correctness of the compensation to minimize problems. Limitations include the following: When a figure has a side smaller than the etch factor, this function may fail. If two boundaries butt up against one another before compensation, because each boundary is handled independently, such boundaries will either overlap or show a gap when compensation is specified. When Etch Factor is applied, re-entrant polygons may be transformed into illegal polygons.

Miter Angle

This is the angle cutoff used with the etch factor. The miter angle controls acute angle edge over-extension. Any angle below the miter angle amount is mitered. The default value is 90.0.

Limitations and Considerations

How you want to use the Gerber output-including layer numbering, use of holes, and polygon shapes-should be extensively considered before beginning your layout design. Setting up the proper layout rules can save a lot of time in generating acceptable Gerber output. For specific considerations or limitations, particularly in relation to apertures and film wheels, consult with your photoplotter vendor.

Using the Gerber Viewer

The Gerber Viewer enables you to view mask (.msk) and Gerber (.gbr) files. The Gerber viewer can be invoked from the layout window File menu, or during export from the Mtools DXF or Gerber translator window.

Criteria for Viewing Gerber Files

In order to be viewed, the files must meet the following criteria:

Launching the Viewer from a Layout Window

  1. From an Advanced Design System layout window, choose File > Export. The Export dialog box appears.
  2. Select Gerber Viewer as the file type.
  3. In the New File Name (Destination) field, enter the name of the file you wish to view. Alternatively, you can click Browse and the Export File Selection dialog box appears, enabling you to browse your directories for the desired file.
  4. Click OK and the following window appears:
  5. In this window, click OK. The Mtools translator and log windows appear.
  6. To dismiss the Mtools Log window, click OK in the window. You may review it at any time by clicking the GERBER tab in the translator window.
  7. In the Mtools translator window, enter the name of the file to view in the Mask Files field. This file must carry the extension .msk.
  8. To invoke the Gerber Viewer, click either View Mask (for DXF and Gerber translations) or View Gerber (for Gerber translations only). The Gerber Viewer appears.
    For information about Gerber Viewer options, see Gerber Viewer Menu Options. For information on the buttons available from the Gerber translator interface, see Exporting Gerber Files.
  9. To exit the Viewer, select File > Exit Xgbrvu.

Launching the Viewer During File Export

You can launch the Gerber Viewer from the Mtools translator window when exporting DXF or Gerber files.

  1. From the Mtools translator window, click View Mask (for DXF and Gerber translations) or View Gerber (for Gerber translations only). The Gerber Viewer appears.

    For information about Gerber Viewer options, see Gerber_Viewer_Menu_Options.._For_information_on_Gerber_translation_options,_see_Exporting_Gerber_Files._For_information_on_the_options_available_from_the_Mtools_DXF_translator_interface,_see_DXF Translator.
  2. To exit the Viewer, select File > Exit Xgbrvu.

Loading a File to View

  1. Choose File > Open/Import
    If there is a file in current memory (that is, you have initiated the Viewer during a file export) and it is not yet loaded, that file is automatically loaded at this time. There is no need to proceed with the following steps.
    Otherwise, the Open Job/Import Gerber dialog appears.

    This dialog enables you to load an existing file, or to create a new job file. (The job file is used for purposes internal to the Viewer and is not required by the vendor.)
  2. Select the desired file type and click OK. A browser dialog that is specific to the file type you selected appears. For example, if you chose ACS Job/Standard RS274D , the Select/Create Job dialog appears.
  3. Select the file you want to load or create and click OK.
    If you cannot remember the name of the file you want to load, you can use a wildcard (*). The browser will display all files that match the wildcard specification.
    If the file you choose does not exist, a dialog appears asking if you want to create it. Click Yes to create the file, or No to cancel.
  4. The Select/Create Aperture dialog appears. Select the file you want to load or create and click OK.
    If the file you choose does not exist, a dialog appears asking if you want to create it. Click Yes to create the file, or No to cancel.
  5. The Gerber Settings dialog appears. Set options as desired and click OK. (For more information, see Gerber Settings.)
  6. The Layer dialog appears. Select layers as desired and click OK. (For more information, see Layer.)
  7. The Aperture dialog appears. Set apertures as desired (see Aperture) and click Save.
  8. Set options, view, and plot as desired. See Gerber Viewer Menu Options.

Gerber Viewer Menu Options

This section describes the Gerber Viewer menu options. A message area at the bottom of the Viewer window provides information specific to your situation.
The two file display options are: Outline or Fill. Click the appropriate button to change the window display. The button title changes to reflect the display.

File

Click File and a drop-down menu containing the following options appears:

View

The following display options are available:

Tools

The Tools menu contains the following options:

Info

The Info menu provides the following options:

When you select (click) an option, information and instructions appear in the message area at the bottom of the Gerber Viewer window. To quit a task, press the ESC key.

Note
Actions prompted for in the Viewer message area (such as pressing ESC to abort) are effective only when the mouse is pointed in the Viewer display area.

Plot

The following options are available from the plot menu:

Outline/Fill

The Outline/Fill button reads as either Outline or Fill , depending upon the display type activated. That is, if Outline appears, the file is displayed in outline form, and if Fill appears, it is displayed as filled.

To change the display from outlined to filled, or vice-versa, click this button.

Layer

The Layer button invokes the Gerber Viewer Layer menu. (You can also choose the menu command File > Layer to open the Layer menu.)

The Layer menu enables you to select which layer files are loaded for display; whether these are displayed as paint, scratch, or negative; and the color they are displayed in. Up to 48 layers may be simultaneously displayed. For information, see Layer Menu.

Note
Changes to the Layer dialog options do not affect the raw Gerber data. They change the display only.

Gerber Settings

File > Preferences > Gerber Settings

Gerber Unit. The units the Gerber data adopts when it is loaded. You may select either INCH or MM. MM is the default.

Format. Gerber data does not contain the decimal point. For coordinate data, you must tell the program the number of digits to insert before and after the decimal point. The default Format value is 3.3. Other common formats are 2.3 and 4.4.

Data formats from 0.1 to 6.3 are acceptable. However, arithmetic problems may arise when very large data values are rendered precisely. For example, if you have a circuit board that extends out 20 inches from the origin and you require 4-place accuracy across the board, you may find that some data points out at the 20,20 coordinate have only 3-place accuracy. This may cause the program to incorrectly fill polygons in this region.

Zero Suppress. Gerber files are normally compressed by suppressing either the leading or trailing zeros of the Gerber data. You may specify Leading , Trailing , or None. Leading is the default. If you choose the wrong setting, the Viewer displays nonsensical data.

Data Mode. The data coordinates can represent either absolute or incremental values relative to 0,0. Absolute is the default. When Incremental is selected, each coordinate represents the distance from the previous coordinate. Selecting an incorrect data mode results in an incoherent display of the data.

Circular. You may select either 90 or 360. Older photoplotters used 90 degree arc interpolation. Newer machines support 360 degree interpolation. The default setting is 360.
If your arcs display incorrectly, try changing this setting.

Arc Resolution. To display Gerber circular commands (G01/G02), the Gerber Viewer uses small, straight segments to approximate the data. How fine the approximation is depends upon the Arc Resolution value. The default value of 9 degrees is appropriate in most cases. This value offers a good compromise between speed and resolution. Valid values are between 0.5 and 30 degrees.

Snap Settings

File > Preferences > Grid/Snap Settings

Grid Spacing. Use Grid Spacing field to set the grid spacing as desired.

Snap On. Click the selection box to turn this option on or off. This option is selected as the default.

Grid On. Click the Grid On selection box to turn this option on or off. This option is deselected as the default.

Gerber Merge

To invoke the Gerber Merge dialog, select Tools > Film Merge

Films. The current filename is displayed in this field. To enter a filename, click in the entry box and type the desired file path. You can also click the ellipses box (...) in the right-hand side of the Film field to select a file from the Working Directory browse dialog.

Negative Image. Click the selection box to turn this option on or off. This option is deselected as the default.

Gerber Files. Your Gerber files are listed in this field. You may delete or undelete these by clicking the Delete/Undelete button below this field.

Output Type. You may select RS274D, RS274X, or MDA Autoplot as the output format. RS274D is selected as the default.

Gerber File. List the Gerber files that you wish to merge in this column.

Delete. This field is disabled.

Paint/Scratch. This field is disabled.

View Film. Click the selection box to select or deselect this option. View Film is selected as the default.

Layer Options

To load your Gerber files, click on a Layer number button. A file selection dialog box appears, enabling you to select the file(s) you want loaded. You may select display options as desired.

The Layer dialog and its options are shown in the figure.

Paint displays the layer data normally.

Scratch performs an XOR operation on all data previously loaded. The resulting display mimics the effect of scratch behavior available on many photoplotters.

Negative reverses the polarity of the layer and is useful for displaying ground planes.

Aperture

File > Aperture
The aperture button in the Gerber Viewer Options window invokes the Aperture menu, enabling you to define apertures from D10 through D999 and assign drill tools to create Excellon drill codes.

To accurately display your data, you must set the correct apertures.

DCode. You may define D-codes from D10 through D999. Click in this field and the Dcode dialog appears, enabling you to select one of 12 standard types (see below).

Type. Twelve types are available: round, donut, square, rectangle, thermal, target, octagon, oblong, poex, poin, thmsq, and custom.

To specify a type, click in the Type field and enter the desired type. Alternatively, click the DCode number and the Dcode dialog appears, presenting the available types for selection.

X , Y. These are the aperture dimensions in units of inches or millimeters (mm), depending on the Gerber unit selected (see Gerber Settings). Some apertures, such as round pads, have only an X value; others require X and Y values.

Tool #. This field is for specifying an Excellon drill data tool. This field is optional and need only be specified when converting Gerber flashes to Excellon drill commands. Valid ranges are T01 through T99.

Drill Dia. Enter the drill tool diameter in this field. This field is optional. Valid ranges are 0.001 inch to 0.99 inch.

Add Default Set. When you click this button, a standard set of apertures is inserted into the list.

Plot Screen

You may select this option by clicking the Plot Screen button on the Gerber Viewer menu bar or by selecting the menu command Plot > Plot Screen. The screen is plotted, and the plot information appears in the message area at the bottom of the Viewer.

Plot Window

You may select this option by clicking the Plot Window button on the Gerber Viewer menu bar or by selecting the menu command Plot > Plot Window. This option enables you to plot a portion of the screen by using the mouse to draw a box around the area you wish to plot. This is done by clicking the mouse on the first and second corners, diagonally, of the plot window. Instructions and plot information appear in the message area at the bottom of the Viewer.

Highlight Apt.

The Highlight Apt. button opens the Highlight Aperture dialog. This dialog enables you to select apertures to be highlighted on the display.
!trans-08-1-33.gif!

Note
Double click an aperture to select and display it. All traces associated with a highlighted aperture appear in light gray rather than in the assigned layer color. Click OK to dismiss the dialog box.

Page/Plotter Setup

This dialog box contains four tabs: Page Setup, Plot Format, Output, and Setup Strings. The options available from each tab are as follows. To access this dialog box, select Plot > Plot/Page Setup

Page Setup. This tab provides access to page size, margin values, and orientation options.

Plot Format. This tab provides access to the plotter driver type, print type, scaling factor, raster memory size (in MBytes), and dpi (dots per inch).

Output. This tab enables you to select the output file name and designate a printer path.

Setup Strings. This tab enables you to set up headers and trailers.

Gerber Viewer Keyboard Commands

You can access many Gerber Viewer commands either through the mouse or the keyboard. In fact, a few commands are available only through the keyboard.

Key Action
Esc Cancels command or moves up one level in the menu structure.
. Toggles the grid on and off.
+ Zooms in 2x.
- Zooms out 2x.
Ins Same as Pan command.
Home Zooms to extents. Same as All command.

Configuring the Gerber Translator for Photoplotters

Types of Photoplotters

There are two types of photoplotters: vector and raster.

Vector Photoplotters

Vector photoplotters process each draw and flash command directly from the Gerber database. These are normally mechanical plotters with an X-Y table, a light head, and an aperture wheel. Examples of vector plotters include the Gerber 3200 and 4000 series flatbed plotters.

Raster Photoplotters

Raster photoplotters rasterize the input Gerber data using a computer, and then use the resulting bitmap to modulate a laser that is scanned across the film. What is interesting about raster plotters is that many of them can accept polygons in addition to draws and flashes. The ability of a photoplotter to fill a polygon is extremely useful to the microwave and RF designer. Examples of powerful raster plotters that support polygons include the Gerber Crescent family of plotters and the Cymbolic Sciences family of FIRE 9000 plotters.

Vector Plotter Configuration

The mask file input to the Gerber translator is essentially a collection of polygons that need to be filled. Therefore, when you run the translator you should:

Typical D-code diameters range from 0.001 inch up to 0.200 inch. Most mechanical photoplotters support up to 24 D-codes.
The Gerber translator uses an advanced multi-aperture fill instead of what we call a pen plotter fill. The multi-aperture fill generates Gerber files with the same resolution as a pen plotter fill, but creates data files 5-10 times smaller.

Polygon Filling Rules

Each polygon is filled independently of any other polygon in the mask file.

Any arcs that are part of a polygon boundary are broken into segments using the ArcRes parameter. This parameter is the number of degrees per segment. The default of ArcRes is 9 degrees. If you need smoother arcs in your film, reduce the number to 6 or even 4 degrees.

The routines start filling at the inner edge of the polygon with the smallest aperture (the one you specify as the Start Aperture in the translation configuration menu). This aperture is normally used twice and is offset from the edge of the polygon by 1/2 diameter (see A below). The first two strokes overlap by 1/2 diameter (see B below).

The routines then select a larger aperture (but normally no larger than 2 times the starting aperture) and repeat this process.

The interior of most large polygons is scan-filled with a fat aperture. There is no overlap between strokes once the routines jump into scan-fill mode.

Empty Polygons

Because the Gerber translator fills each polygon as it encounters it in the data stream, when it encounters an empty polygon it cannot clear away areas already filled. Therefore, for vector photoplotters, avoid using empty polygons in your layout. (This limitation is not in effect for some raster plotters.)

The translator issues a warning in the log file when it does encounter an empty polygon so that you do not accidentally plot over it.

If you have used empty polygons in your design, you may select the Advanced Design System Gerber export option Auto Merge , enabling you to merge filled and empty polygons to form a single filled polygon. This creates what we call a re-entrant polygon and is supported by the Gerber translator. However, while we recommend this function for relatively simple structures, we do not recommend you use such a function where hundreds of drill holes must appear in a power plane.

Compensation

Compensation works by swelling or shrinking each polygon prior to filling it. Again, because the translator views polygons independently, it cannot take into account spatial relationships between polygons. If you attempt to use a shrink compensation with butting polygons, a narrow gap will form between them.

FIRE 9000 Photoplotter Configuration

The Cymbolic Sciences FIRE 9000 photoplotter is a raster laser plotter that is ideal for creating microwave and RF artwork. Not only does this photoplotter have a very high resolution (typically 1/8 mil), but its RIP front end supports two very important extensions to standard Gerber (RS274D) data:

Because of these high level commands, the Gerber translator can translate a mask file with empty polygons directly into a stream of POEX and POIN commands. Configuring the translator for MDA output is the only mode that supports empty figures in the mask file.

Not only does configuring the translator for MDA output eliminate the need to stroke out the interior of each polygon, but the resulting artwork is limited only by the precision of the photoplotter. The FIRE 9000 autoplot format also embeds all Gerber format, unit, and data mode information into its header so that a separate aperture and information list is not needed.

We highly recommend (if possible) that you send your data to a photoplot or board shop equipped with a raster photoplotter such as the FIRE 9000.

The Gerber Viewer can properly view both POEX and POIN data so that you can verify the correctness of the output.

Recommended Settings for FIRE 9000 Output


The proper settings for FIRE 9000 output are summarized in the table below. When Outline/Fill is set to OUTLINE , each mask polygon is outlined. If a polygon is filled, then it is sent to either D20 or D21; these are both assigned as POEX. If it is an empty polygon or a hole, it is assigned to D22 or D23 which correspond to a POIN. Any open mask entities are sent to D10, which is a standard round aperture.


Gerber Translator Settings for FIRE 9000 Output
Gerber File Options Translation Settings Apertures (inches)
Option Setting Option Setting D-Code Type Inch (X,Y)
Unit INCH or MM Line DCode d10 10 Round 0.005
Format 4.4 or 4.3 Scale Factor 1 20 Poex 0.000
Zero Suppression Leading Outline/Fill Outline 21 Poex 0.000
Circular 360 Filled D-codes (POEX) d20, d21 22 Poin 0.000
CR/LF Suppress Empty D-codes (POIN) d22, d23 23 Poin 0.000




Compensation None









Output Offset 0,0









Gerber Output Format MDA Autoplot





RS274X Output Configuration

Gerber Scientific's laser photoplotters read the extended RS274X specification. These photoplotters also support a polygon definition. Unfortunately, however, "empty" polygons are not supported. If you use empty figures in the mask file they will be covered up.
Other photoplotters may also support the RS274X specification, but before using them you should verify that they properly support the G36/G37 command used to switch into polygon mode.


Recommended Gerber Translator Settings for RS274X Output
Gerber File Options Translation Settings Apertures (inches)
Option Setting Option Setting D-Code Type Inch (X,Y)
Unit INCH or MM Line DCode d10 10 Round 0.005
Format 4.4 or 4.3 Scale Factor 1 20 Poex 0.000
Zero Suppression Leading Outline/Fill Outline 21 Poex 0.000
Circular 360 Filled D-codes (POEX) d20, d21





CR/LF Suppress Compensation None









Output Offset 0,0









Gerber Output Format RS274X





Creating an Excellon Drill File from an ADS Layout Using MTools

This section describes the procedure for creating an Excellon drill file from an ADS Layout. Excellon drill files define x and y coordinates for hole location and drill size. These files are used to automate the drilling process in manufacturing environments.

To create a drill file:

  1. In the layout window containing your design, choose File > Export. The Export dialog box appears.
  2. Select Gerber from the File Type drop down list then specify the file name in the New File Name (Destination) field. Click OK. The Mtools status window appears.
  3. Click OK in the Mtools status window to accept the settings. The Mtools Log and Gerber Translator Interface windows appear.
    Gerber Translator Interface Window
  4. From the Gerber Translator Interface window, click Edit Apertures. A table listing the aperture settings appears.
  5. In the Aperture dialog box, click Flash Circles. A Map Circles/Holes dialog box appears.
  6. In the Map Circles/Holes dialog box, verify that the circle Count and Diameter for each Block are correct. Ensure that the Update Aperture box is checked. Note the Block name of each of the circles in the Map Circles/Holes dialog box. Click OK in the Map Circles/Holes dialog box.
    In the Aperture dialog box, using the information from step 6, note which D-codes have the Block names that were mapped to circles and then click Save. A small dialog box asking if you want to save the changes appears. Click OK.
  7. From the Gerber Translator Interface window, click Translate to select the layers you want to include in the translated file (see Translate). After selecting the layers, click OK to complete the translation. A window appears briefly, indicating that the file is being converted to Gerber format.
  8. When the translation is complete, the Mtools Log appears, detailing the export information. Examine the log file, searching for any warnings or errors that may have occurred during translation.
  9. When you are finished viewing the log file, click OK to dismiss the MTools Log and exit the Gerber translator. You can also save the MTools Log before exiting using the File > Save As menu pick.
  10. From the Gerber Translator Interface window, click View Gerber. The GBRVU dialog appears with a Gerber view of your layout.
  11. From the GBRVU dialog, click Aperture. The Aperture dialog box appears.
  12. In the Aperture dialog box, enter the Tool # (integer only) and Drill Dia. for each of the D-codes that were noted in step 7. Click Save. A small dialog box asking if you want to save the changes appears. Click OK.
  13. From GBRVU, choose Tools > Drill > Excellon. Choose whether or not to suppress the leading zero's. The Drill Output dialog box appears.
  14. Click the appropriate Drill Output and then click Report. The GERBER VIEWER - DRILL REPORT file is displayed. This file contains a DRILL TOOLS TABLE that lists tool numbers, tool size, quantity and remarks.
    Example Drill Report:
  15. Use any ASCII text editor to open and view the drill file (file extension .drl) stored in the current ADS project directory.

Example Drill File:
M48
INCH,TZ
VER,1
FMAT,2
DETECT,ON
%
M72
G05
T01C.025
X-03000Y001000
X-03050Y-00500
X-01500
X002000
X001500Y000000
T02C.125
X-01500Y001000
Y000500
X-01000
Y001000
M30

Note
Both the drill report and drill file are created in the ADS project directory with the layer name as a prefix and .rpt and .drl as suffixes.
Example: layer_name.rpt is the drill report and layer_name.drl is the drill file.


 

Privacy Statement  | Terms of Use  | Legal | Contact Us  | © Agilent 2000-2008 

Contents
Additional Resources