8
\$\begingroup\$

Question
I would like to import Gerber files into an Altium Designer PCB document for re-using an in-PCB spiral inductor but the importer fails to interpret the Gerber files in a correct way. Has anyone here knowledge on how to import Gerber files into an Altium Designer layout?

Background/What I have tried
The design containing this PCB spiral is a reference design from Linear Technologies and there are design files available for download here (clicking link will download a .zip-file). The design files contains a Mentor Pads PCB file but also Gerber files.

The ECAD system I'm using is Altium Designer 15.1. Since the Mentor PADS PCB file is of binary type I can't import it into an Altium Designer layout document. Altium designer can only import ASCII type Mentor PADS PCB files and I don't have access to conversion tools for converting from PADS binary format to PADS ASCII format. Therefore I tried to import the Gerber files into an Altium layout document. The result is not right at all, there is just a mess of top layer copper.

I have opened the Mentor PADS PCB file into the free Mentor PADS viewer and the design looks like it is supposed to. I have also imported the Gerber files into CAMtastic (the built in Gerber viewer in Altium Designer) and the design looks like it is supposed to. I also tried to export new Gerber files from CAMtastic and then import them into an Altium Designer PCB document but I had no luck with that.

Added to original post (1)
The way I've been trying to do the import of Gerber files into an Altium Designer PCB document is that I open a new PCB document and then I import one Gerber file at a time by choosing File->Import->Gerber File. I stop after the first import since I just get a mess of tracks and pads.

Added to original post (2)
Just opening the Gerber file using the Built in Altium CAMtastic viewer is not the complete answer for me. I would like to transfer some design elements from these Gerber files into a design for reuse.

\$\endgroup\$
  • 1
    \$\begingroup\$ Maybe this can help you designcontent.live.altium.com/PluginDetail/Importer_Gerber \$\endgroup\$ – Lazar Jun 3 '15 at 10:17
  • \$\begingroup\$ @LazaR, Thank you for your suggestion. Using the Gerber importer plugin from the File->Import menu is the way I've been trying to do it. I get something imported but it is not translated correct at all. The import becomes a mess of tracks and pads. \$\endgroup\$ – Mattias Johansson Jun 3 '15 at 11:16
  • 1
    \$\begingroup\$ Would it be good if you could open the gerber files one by one (layer by layer) in Altium? \$\endgroup\$ – Bence Kaulics Jun 3 '15 at 12:04
  • \$\begingroup\$ @BattleHamster, thnak you for your suggestion. That is what I've been trying to do. I open a new PCB document in Altium and then I choose File->Import->Gerber File. No matter which copper layer I choose I just get a mess of tracks and pads. \$\endgroup\$ – Mattias Johansson Jun 3 '15 at 12:07
  • 1
    \$\begingroup\$ @Mattias Johansson You needed the PCB coil design from this other PCBdoc. With TI's WEBENCH a wide selection of PCB coil designs are available in Altium Designer, Cadence Allegro 16.0-16.5, CadSoft EAGLE PCB (v6.4 or newer), DesignSpark PCB, Mentor Graphics PADS PCB. I have just discovered it a couple of days ago, thought it could be useful next time. \$\endgroup\$ – Bence Kaulics Jun 8 '15 at 15:04
14
\$\begingroup\$

I have downloaded the design you are dealing with. The gerber files, all layer files have .PHO extension.

enter image description here


Import gerbers into Altium

If you rename the files as follows you will be able to open them in Altium:

  • Layer4.pho \$ \longrightarrow \$ Layer4.GBL, this is the bottom layer
  • Layer1.pho \$ \longrightarrow \$ Layer1.GTL, this is the top layer
  • Layer2.pho \$ \longrightarrow \$ Layer2.GP1, GND plane 1
  • Layer3.pho \$ \longrightarrow \$ Layer3.GP2, GND plane 2
  • SoldermaskBottom.pho \$ \longrightarrow \$ SoldermaskBottom.GBS
  • SoldermaskTop.pho \$ \longrightarrow \$ SoldermaskTop.GTS

I have identified the layers by the PDF appendix. For Pastemask (GBP, GBT) and Silkscreen layers you should search for their Altium extensions.

These modified files can be dragged and dropped into Altium, example for Top layer:

enter image description here

This way all layer files are easily openable in Altium.


Export TopLayer gerber into PCB document file

  1. Select Layer1.GTL tab in Altium
  2. Select the Menu → Tables → Layers Order option. Following dialog will be shown: Fill the cells as below.

    enter image description here

  3. Enable the Export to PCB option as follows: Menu → Tools → Netlist → Extract.

    "After a netlist has been extracted from your CAM data, the File » Export » Export to PCB command becomes enabled" source

  4. Now, select Menu → File → Export → Export to PCB and a new PCB document will be opened with the Top Layer.

    Result:

    enter image description here

\$\endgroup\$
  • \$\begingroup\$ Thank you. I have come this far as well but what I would like to do next is to transfer the spiral from the .GTL file into a .pcbdoc file to use in a new design? How do I do that? \$\endgroup\$ – Mattias Johansson Jun 3 '15 at 12:53
  • \$\begingroup\$ The gerber importer plugin still does not work? \$\endgroup\$ – Bence Kaulics Jun 3 '15 at 13:25
  • \$\begingroup\$ Unfortunately not. It seems like the Gerber importer can't interpret the Gerber files correctly. I just get a mess of tracks and pads. \$\endgroup\$ – Mattias Johansson Jun 3 '15 at 13:29
  • 1
    \$\begingroup\$ @Mattias Johansson I have edited the answer, it seems OK to me. I have all the traces as it supposed to be. I hope it will work for you too. \$\endgroup\$ – Bence Kaulics Jun 3 '15 at 14:25
  • \$\begingroup\$ I really appreciate your help @BattleHamster, thank you. I'm sad to see that even though I've followed your instructions step by step the "Export to PCB" option is greyed out for me. \$\endgroup\$ – Mattias Johansson Jun 3 '15 at 14:43
1
\$\begingroup\$

The only way round I found was getting old PADs Logic/PowerPCB files into Altium Designer were to first find a local company, that uses Pads, to go through my files on a USB stick and export in ASCII format. Each file, for schematic (.txt) or layout (.asc), were exported as version 9.5 ASCII file (NOT PADS VX ASCII) which seemed to be the latest that Altium designer would support.

For Pads library files, Altium Designer will import from Pads library files version 5 onwards. I have tried previous versions, by opening and editing the Pads library file (.c, .d, .p type files) and editing the top line and then importing into Altium. This method does not always work and it is trial and error.

I do not think you can import Gerber file and convert into a native format like .Pcbdoc or a Pads file since Gerber is an instruction file for print/manufacture.

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.