Creating RS274X Gerber Files for PCBs Designed using "Tango PCB for DOS"

Version 1.01 (9-Nov-21) Copyright 1994-2021
Sam Goldwasser
--- All Rights Reserved ---

For contact info, please see the Sci.Electronics.Repair FAQ Email Links Page.

Reproduction of this document in whole or in part is permitted if both of the following conditions are satisfied:
  1. This notice is included in its entirety at the beginning.
  2. There is no charge except to cover the costs of copying.

Table of Contents


This document outlines ways to generate RS274X Gerber files PCBs created with the pre-Jurassic but fabulously wonderful layout program: "Tango PCB for DOS". (Much of this information also applies to other ancient PCB layout programs that generate Gerber files in the RS274D format.) This is the original version of Tango PCB and has sufficient capabilities for doing quite complex PCB layout as long there something fancy is required like parts at funny angles or controlled-impedance traces. And it has a user interface that results in an experience has been likened to "playing a musical instrument". I have created 11 x 13 inch 12 layer PCBs using Tango PCB for DOS in the early 1990s on a 100 MHz Pentium PC running Window 98 in a DOS shell. They had hundreds of mixed through-hole and SMT components and over 5,000 holes. (No, I didn't route every trace by hand. Tango sold a separate autorouter which also ran under DOS that did much of the work, though subsequent cleanup of jiggly and errant traces was needed.) Subsequent releases of Tango (after the company were acquired by OrCad) converted to run under Windows 2000 and beyond have suffered from the limitations of the Windows GUI as well as creeping featurism on a grand scale. If you are familiar with Tango PCB for DOS, you know what I'm describing. If you're not, unfortunately, the program requires a parallel port security dongle and cannot be installed from the Web or anywhere else. Or at least, I haven't figured out a way. I could also not get Tango PCB for DOS to run under DOSBOX (Note 6) even with its dongle plugged into a valid parallel port. And copies of Tango PCB for DOS with the dongle are now scarcer than raw dragon's eggs and probably being hoarded as I've yet to find one anywhere. If anyone has more info on any of this (or one to sell as I'd like a spare), please contact me via the Sci.Electronics.Repair FAQ Email Links Page.

The problem with Tango PCB for DOS is that it is only capable of generating Gerber files in the equally ancient RS274D format which is not accepted by most PCB houses nowadays including Seeed Studio and JLCPCB (Note 5). Thus conversion to RS274X is required. While how to do such a conversion is probably intuitively obvious to someone who designs PCBs on a daily basis, if just dusting off Tango PCB for DOS every other blue moon, the following could prove useful. It was written specifically with JLCPCB in mind but should apply to most others.

The first two procedures depend on the type of PCB but they all use the same Tango settings for CAM output. (The third does not use Tango to generate the Gerbers, so these settings are irrelevant.)

Some other settings work but not all.

Multilayer PCBs with or without Internal Planes using Gerbview

This procedure requires Gerbview (Note 1) or another program that can do RS274D to RS274X conversion. Gerbview is not freeware but offers a 30 day free evaluation license. And the purchase cost for a single seat license is relatively modest and justifiable if you want to stick with Tango PCB for DOS and do a steady stream of PCBs. ;-)

The example below is for a 4 layer PCB named 4LAYER.PCB in Tango. With obvious modifications, it should also apply to PCBs with 2 signal layers and no plane layers or more than 4 signal layers with or without plane layers.

  1. Make sure the apertures are set and then generate the Gerbers for 4LAYER.PCB in Tango PCB. Use the extensions: gto, gts, gtl, g1, g2, gbl, gbs, gbo, and gko for the keepout/board layer. Note: Tango PCB may capitalize them and not maintain the 2-letter g1 and g2 extensions and will rename them to g10 and g20. Rename them back to g1 and g2 manually.

  2. Generate the Excellon drill file for 4LAYER.PCB using the settings shown above - ASCII: None and Zero Suppression: None. The typical extension is .NCD or .XLN. This is NOT the DRL file that Tango normally produces, which is just a map of drill symbols and useless to machines.

  3. Generate the Report (REP) file with the Aperture List enabled. It is needed to convert to RS274X.

  4. Load all Gerbers generated by Tango for the 4LAYER.PCB, the drill layer (4LAYER.NCD or 4LAYER.XLN), and 4LAYER.REP file) into Gerbview (Note 1).

  5. Confirm that all layers including the drill layer show up and are correct.

  6. Convert to RS274X as separate files without extensions so they will have the original extensions. (Clear the extension field in the Conversion dialog box.)

  7. Zip all layers (gto, gts, gtl, g1, g2, gbl, gbs, gbo, drl) along with a README if desired.

Two Layer PCBs with Signal (top) and Ground Plane (bottom)

This procedure is the same as for four layer PCBs but do NOT include the g2 and gbl Gerbers. Rename g1 to gbl and specify it to be NEGATIVE in a note to JLCPCB and in the artwork.

Two Layer PCBs with Top and Bottom Signal Layers Using TangoKiCAD Converter and KiCAD PCB Editor

Two layer PCBs can also be done using the procedure, above. But this one does not require RS274D to RS274X conversion using Gerbview as KiCad (Note 3) generates RS274X Gerbers directly. However, it can ONLY be used for PCBs with 1 or 2 signal layers TangoKiCAD chokes on anything more complex including more layers and/or plane layers.

  1. All that is needed is the Tango PCB file, 2LAYER.PCB saved as ASCII. Tango is not used to generate the Gerbers.

  2. Use TangoKiCad (Note 2) to convert 2LAYER.PCB to 2LAYER..BRD. Only the source (Tango PCB file) and destination (KiCAD BRD file) fields need to be filled in. Run "Convert PCB" and exit - TangoKiCad screws up and generates anomalous traces (or worse) if run more than once even if the Tango PCB file is unchanged. (TangoKiCAD may turn off "Show window contents while dragging" for no justifiable reason. To re-enable it, go to "Control Panel, System and Security, System, Advanced System Settings, Performance Settings.)

  3. Open 2LAYER.BRD with the KiCad Pcbnew editor. No editing needs to be done except possibly to move the PCB inside the KiCad template (though this probably doesn't matter). Generate the Gerbers for the top and bottom layers (gtl, gbl), top and bottom soldermasks (gts, gbs), top and bottom overlay/silkscreen (gto, gbo), keepout (eco2, BRD layer in Tango), and the drill layer (drl, which is NOT derived from the DRL layer normally generated by Tango, but from the pads definitions in the PCB file itself). Rename 2LAYER.eco2 to 2LAYER.gko.

  4. Zip all layers (gto, gts, gtl, gbl, gbs, gbo, drl) along with a README if desired.

Final Check

Use Gerbview or Gerbv (Note 4) to display the final Gerber files to confirm that there are no screwups. Once uploaded to JLCPCB, view the Gerbers in the "Production File" (under the folder "ok") and confirm again. For PCBs with plane layers (negative), they should appear as mostly copper (negative of what Tango displays). Access to the Production Files may require that the board be paid for and, uh, in production. But perhaps there's a way to have JLCPCB give you a sneak peak before approval.

The examples below show the typical appearance of a Gerber signal layer, a Gerber plane layer as generated in Tango PCB, and a Gerber plane layer as displayed using Gerbv from the JLCPCB production file for the board.


Typical Gerbers: Signal Layer (left, copper is red); Plane Layer Generated by Tango (Center, copper is black); Plane Layer from Production File (right, copper is green)


  1. Gerbview is not freeware but does offer a 30 day free evaluation.

  2. TangoKiCad seems to have disappeared from the Web. I can provide a copy but note that Zonealarm has sometimes believed it was Malware and deleted or quarantined it, but that hasn't happened for several years and I have never had problems using TangoKiCad for even more years, except for how brain-dead it is. :( ;-)

  3. KiCad is freeware which includes a suite of CAD tools, though only the PCB editor is used here.

  4. Gerbv is freeware and works well for displaying Gerber files.

  5. Seeed Studio Fusion PCB and JLC PCB are two companies that will fab PCBs in small quantities at excellent prices.

  6. DOSBOX is a DOS emulator that runs under Windows. While Tanog PCB for DOS will attempt to startup in DOSBOX, it aborts since its security dongle is not recognized.