"Gerber rs 274 d"
"Gerber rs 274 x"
See also:

Gerber Special
Drill Output
Problems with the import of X-Gerber
Sample Gerber files of a sample project


Creating Gerber data in TARGET 3001! is a matter of seconds. The specialty of this Gerber driver is that Extended Gerber (RS-274-X) is generated but nevertheless those data can be read by "standard" Gerber machines too because only the old Gerber commands (RS-274-D) are used. Gerber aperture data are generated, superfluous for CAM factories working with Extended Gerber but necessary for CAM factories working with standard Gerber( RS-274-D). An additional info text file is generated plain talking what is wanted from the manufacturer.

Creation of Gerber data from TARGET 3001!

After you had finished your layout/routing work, please use the Menu File / Input/Output Formats / Production / "(X-)Gerber and drill output PCBout" The following dialog opens:

The Create TARGET 3001! CAM-Data dialog
Image: The Create TARGET 3001! CAM-Data dialog

If you are a PCB manufacturer, please find a set of sample Gerbers to check their matching with your production processes. These Gerbers are based on this project: sample project

The list shows the Gerber files going to be created (see extensions in brackets) which will be sufficient to manufacture your board. The number and kind of Gerber data depend on the complexity of your project. TARGET recognizes it and puts the expected files to this list. Choose a directory for saving the files (in the dialog bottom left). With button Special>> set further specifications if necessary. What's behind this button please see in detail here: Gerber Special. An option to set Gerber X2 please find there as well.

Now press the Start button.

Special settings can be done
Image: The Create TARGET 3001! CAM-Data dialog opened for Special settings

Now the XGerber data are generated to the desired directory. That's what they look like for this example:

These Gerbers are created from the Pic_3D.T3001 example file
Image: These Gerbers are created from the Pic_3D.T3001 example file

Hand out those files to your PCB manufacturer. The *.info file can be opened by any text editor and informs your PCB manufacturer in clear words which Gerber files are given regarding this special project. So he can check whether all files had arrived at him. For the project file in our example, the *.info file looks like this:

Contents of the Gerber-Info file
Image: Contents of the Gerber-Info file based on the project shown

Important technical note for PCB manufacturers:

from version the order of the copper layers is numbered from top to bottom:

double sided:
L1 = Top
L2 = Bottom


n-times multilayer:
L1 = Top
L2, L3, L4, L5... = inner layers, counted from top to bottom
Ln = Bottom

In earlier versions copper layers were counted from bottom to top.


If your pcb house should ask Gerber files with different extensions from you please press the Special>> button. This will extend the Gerber dialog and at the bottom to the right give opportunity to choose different extensions (button "Standard").

Selection of Gerber data

Selection of data when creating Gerbers
Image: Data selection when creating Gerbers

The "Selection" option refers to the ability to design multiple sub layouts within one project. You can give this name and output its Gerber data separately. At this point, select the name of the sub-layout whose Gerber data you want to create. Read more about it here: Multiple PCBs within one project

Read in of Gerber data to TARGET 3001! (Gerber viewer?)

Please note: TARGET 3001! is not a Gerber viewer! The Gerber import is able to read files containing XGerber (RS-274-X) and Excellon data from various other CAD packages with the aim of importing them layer by layer into a TARGET project. If you want to check your Gerbers by a Gerber viewer, have a look at the free tool GerberLogix


As an alternative Gerbv might be welcome. You can download this viewer at sourceforge for free. There is no installation neccessary, the exe file runs instantly.


The Gerber viewer GC-Prevue is not free anymore.

Read XGerber and Excellon files

An X-Gerber file is a textfile which may have the following syntax:


An Excellon File (for the drills) also is a text file and for example looks like this:


In case your data look completely different, it's likely that you don't have XGerber or EXCELLON-data.

The opening dialog for Xgerber-import please find in TARGET 3001! Menu File / Input/Output Formats / Data exchange/Documentation / Read XGerber and Excellon files.

An XGerber file-name is overtaken to a line of the dialog and "noted" for conversion...

XgerberImp e.jpg
Image: This is the XGerber import dialog!

Button (1.) opens your Windows browser for the selection of one of your given Gerber files which you select from your folder. Now enter which kind of data (2.) the file contains. Afterwards define by (3.), to which layer in TARGET 3001! the data shall be transferred (e. g. layer "2, copper bottom", "24, drillholes"... ). Now see the file already listed in the first dialog line (4.). Now click on "New line". TARGET 3001! now is ready for reception of a new file to a new line (=layer) and you start with 1. again to pick the next data file.

EXCELLON data (most often used to define drill holes) you import the same way.

If you click button: "File contains Excellon" in the box "File format", you'll get the option "Excellon Factor". So you can take influence on the drill data. How big the factor needs to be set is a question of trial and error. The same with "Gerber factor" if you had ticked the XGerber file format. Press "Start" to convert the selected files.

E ExcellonFactor.jpg

If your Excellon-File doesn't give Information on the diameters of the drilling tools, but you know the diameters, you can simply precede the Excellon syntax with a simple text:


M71 switches over to "mm". A "T" is followed by the number of the tool e.g. 1...17. After the "C" please find the tool diameter in mm. The dot separates the decimals. The initial file started with "G90" . M72 switches back to imperial unit (inch), which is the standard setting in EXCELLON.

Read Gerber (RS274D) and Excellon files using the TARGET 3001! "XGerber import" dialog (recommended)

XGerber (RS274X) carries all aperture information in its genuine layout file. In case you are using the older standard Gerber files (RS274D) for reading in, you must have (identify) the aperture file delivered and need to have it interpreted by TARGET 3001!. Those aperture files do not have a standardized structure at all. Neither the file extensions nor the information within the file itself. Fortunately at least all files (Gerber-, aperture, drill- and drill tool files) are bare text files easily to be read by normal text editors. First open the import dialog in Menu File/Input-/Output formats/Data exchange/documentation/Read XGerber and Excellon files...

Gerber e 1.jpg
Image: Importing Gerber data using the XGerber import

Now you read in each of your images line by line to a separate layer. Define which file you want to read in first and say to which layer in TARGET you want to import it. The answer to the question which of your file contains which information needs some experience and some testing. Sometimes there is a descriptive info-file. Copper top often is denoted by TOP or T within the file name, copper bottom often is denoted by BOT or B.

XgerberImp e.jpg
Image: Same dialog as above.

Search for your Gerber data within your directories ("Read file", top right). In this example we choose/destinate layer 2, copper bottom.

Gerber e 3.jpg

We do the same with the next file...

Gerber e 4.jpg

...which contains data for copper top. Import it to layer 16, Copper top.

Gerber e 5.jpg

If you press the START button, you get asked whether you want to search for an aperture file which defines the so called "D codes" because at this time D codes are not sufficiently defined yet. D codes care for size and shape of the apertures which get moved in front of exposure to light. Gerber data control those moves. The aperture file is a kind of description of the exposure tools while Gerber files say what is to be done with them.

Gerber e 6.jpg

Press button "Yes" and search and select from your file set the one which keeps the aperture information.

Gerber e 7.jpg

Aperture files often can be identified by an A or APR (aperture) or WHL (Wheel=aperture wheel) in the file name.

Gerber e 8.jpg

After you have selected an appropriate file a dialog opens allowing the interpretation of the aperture data. Aperture data often consist of a header and eventually of an appendix. Both can be deleted. Only those lines are of interest which contain D codes D10,D11,D12...

Gerber e 9.jpg

The structure of D codes is not defined. The image only shows an example. Look at a D code line and now interpret it column by column. The button Automatic helps finding a preselection. In our example the first parameter defines the d code, the second the shape of the aperture (ROUND or SQUARE), the third parameter defines width and diameter of an aperture. Because we don't have a fourth parameter "Height"we set it "3. Parameter" too. In which scale your your gerbers come across please set in the last box. If the sequence of your parameters match, please press button "Use apertures". Now see your copper bottom and copper top layout in TARGET 3001!.

Gerber e 10.jpg

Read Gerber (RS274D) and Excellon files using the "Gerber import" dialog (outdated but still working)

Using this tool (File/Input/Output Formats/File transfer/Documentations/Read Gerber and Excellon files) you can view the Gerber (RS274D) data of your project before producing a PCB. The Gerber data are directly read into a TARGET project. By selecting the PCB layers set visible, the corresponding views can be seen and checked with the TARGET project in separated windows besides each other. Additionally you can import Gerber data from other layout CAD packages and edit those within TARGET.

E Gerber Einlesen.jpg

REMARK: Gerber data concerning the layer "solder stop" should be read in from another layer than "Solder Stop Bottom", because TARGET recognizes the pads of the Solder Stop Layer automatically by activating them in the normal layer dialog. Gerber data of the solder stop layer with topping of the vias are ignored then or dominated by those "recognized".

If the external CAD format you need concerning the aperture and drilling list not is offered by TARGET, please describe it to us (evtl. using an example - file). We add all formats you drop to us into the list as we estimate it reasonable.

What's the difference between Gerber and G-Code?

G-Code and Gerber are similar but describe different things: Gerber describes the drawing of a PCB layer. A command in Gerber mostly results in a piece of a track or in a pad. G-Code mostly is used for controlling milling machines. A command in G-Code normally results in a movement of the milling bit.

Regarding isolation milling, moving the milling tool inside tracks and pads would destroy them. The movement has to be outside along the tracks and pads to create isolation channels all around. TARGET 3001! is able to compute the G-Code for PCBs, regarding the milling bit diameter and the track widths. Because TARGET 3001! can also import Gerber files, it can be used as a universal Gerber-to-G-Code converter.

G-Code can be created in TARGET 3001! by the menu option:

Gcode e 1.jpg

This menu entry opens the following dialog where you can opt for G-code as output format.

Gcode e 2.jpg