On 05:32 AM 24/06/2003, palaniraja said:
Thanks Ian Wilson, Graham Brown & Thomas for your valuable comments
on PCB Duplication Methods.


The version of Camtastic that is included with DXP apparently has some aids to export a PCB from Gerber and drill data.

I quote an Altium employees comments on reverse engineering PCB from gerber below in full. His reply was on the public Altium DXP forum so I don't think Altium would mind me posting here - I could have linked to the post on the DXP forum I guess (I have removed his name but you can easily find it out by looking at the relevant msg on the forum archive). Camtastic in DXP offers an Export to PCB command. A question was asked about why it was greyed out. Following is the reply.


<..snip some stuff about editing gerbers..>

About Export 2 PCB command there are a few restrictions you must be aware
of. This command should be used for reverse engineering a board from Gerber,
NC Drill & IPC 356-D data. I emphasis that you need at least the Gerber & NC
Drill data (if you want to get the designed net names then you need the IPC
356-D netlist as well), this is because before going to Export 2 PCB you
need to do the following:
1. Set-up the layers types if they are not already correct - Tables /
Layers... command
2. Set-up the layers order - Tables / Layers Order... command
3. Set-up the layers sets - Tables / Layers Sets... command  - this is
needed of you have blind / burried vias only.
4. If you have split-planes then you need to verify that the boundaries used
to draw the splits are closed polylines (use Q for Query command & query
each split plane, if the properties of the queried object tells you that the
Type = Closed Polyline then you don't have to do anything, if the Type =
Open Polyline or Line then you need to join the lines in order to create a
closed boundary for each split. To do this you can use CAMtastic Edit /
Objects / Join command, or if this doesn't give you the best result you
might want to try Analisys / Clean Boundaries command). Keep in mind that
CAMtastic's nelist extraction process doesn't support nested split-planes
right now.
5. Extract the netlist from connected copper - use Tools / Netlist / Extract
6. Rename the nets to their design name - if you loaded an IPC 356-D net
then you can run the Tools / Netlist / Rename Nets command in order to
rename CAMtastic extracted nets to some more useful names than $Netnnn.
Once you completed these steps you are ready for running Export 2 PCB
command (the command should no-longer be greyed out).
If you encounter any problem you can read more from

This article contains a more detailed description of the above 6 points.

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
* Contact the list manager:
* Forum Guidelines Rules:
* http://www.techservinc.com/protelusers/forumrules.html
* Browse or Search previous postings:
* http://www.mail-archive.com/[EMAIL PROTECTED]
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to