Converting "CadStar gerber files" to "Protel

Do anybody know how is most easy to build a "Protel2004DXP PCB" from "CadStar gerber set files"? I have tried with the Protel CAMtastic, but I have two major problems - aligning the layer is too difficult for me and finally I don't see the command "Export to PCB" active when I'm ready to export from CAMtastic to PCB. Is there anything more I have to do?
Thanks!

Re: Converting "CadStar gerber files" to "Pro

Try Cam350 – you can convert Gerber in native .cam format and then export to tango, power pcb or some other cad programs readable from protel dxp. But result is not editable file like normal design file

Re: Converting "CadStar gerber files" to "Pro

I'm not sure why aligning layers is too difficult for you in CAMTASTIC. All you do is select matching items (such as a multilayer pad) and hit 'CTRL L'.

In order to reverse engineer a board, you also have to load the drill file in addition to the Gerbers. This is true no matter what CAM editor you use.

Once the Gerbers and drill file are loaded and aligned, you have to tell the Gerber editor to extract a netlist. This is the ONLY way the editor has of knowing what is connected to what. When the netlist has been extracted, the export to PCB button will no longer be greyed out.

If you also have the IPC-D350 file for your Gerbers, you can load that into the CAM editor. CAMTASTIC will identify the componets from that file, and assign the nets their original names. Then, when you export to the PCB editor you have a fairly complete representation of the original board.

You should read the following document for a step-by-step description of how to reverse engineer: https://www.altium.com/files/learningguides/AR0121 CAMtastic Reverse Engineering PCBs.pdf

Re: Converting "CadStar gerber files" to "Pro

Thank you very much! It works perfect!
I havn't wanted to lose a time reading the *.pdf's and wanted to start the work quickly. I have read all the concerned *.pdf's now and all aspects are much more clear.
Thanks again!