Applied Parameters: None
This command is used to export data from the CAMtastic Editor directly to a new PCB document. This enables you to recover old designs that were generated using PCB tools that are perhaps no longer supported, working backwards from the Gerber files.
This command is accessed from the CAMtastic Editor by choosing the File » Export » Export to PCB command from the main menus.
First, ensure that the necessary layers have been loaded into the current CAM document, with respect to the design you wish to export. The Exporter can transfer entire boards into the PCB document, not just Gerber files. For example, if you are exporting a thru-hole board, make sure that the current CAM document contains at least the Top, Bottom and NC Drill layers. Mask, Overlay and other layers are beneficial, but not essential to the export. Also ensure that the netlist for the current document has been extracted.
After launching the command, a new PCB document will be generated (<CAMDocumentName>.PcbDoc) and opened as the active document in the main design window. The actual sequence of events in the transfer of information between the CAM document and the PCB document is as follows:
- The PCB document is created with a board outline based on the current size of the board in the CAM document.
- Net objects are created in the PCB document, using the net information extracted from the CAM document.
- The layer stack-up is generated, based on the physical layers order defined in the CAM document (Create/Update Layers Order dialog, accessed through Tables » Layers Order).
- Nets are assigned to any internal planes.
- Nets are assigned for any split planes that exist.
- Clearance, Width and Power Plane Connect Style design rules are created. Relief connects are created for each plane net.
- Padstacks are built from the CAM data (using pads on the signal/plane layers in the physical order, followed by drill, mask, paste, etc). The padstacks are loaded into the PCB and the required style is defined (simple or full padstack).
- The PCB tracks are created.
- A DRC check is performed for the whole board.
- This command transfers data from the CAM document to the PCB document using the PCB API. In this way, no exported data files (in Gerber or other format) are generated, and so the need to use the PCB Editor's Gerber Importer is bypassed.
- Before extracting the netlist in the CAM document, make sure that the drill layer sets have been defined as required (Create/Update Layers Sets dialog, accessed through Tables » Layers Sets). This is compulsory if you are using blind/buried vias, in order to extract the correct netlist. For blind/buried vias, you must select all layers that are drilled, not just the start and end layers. For thru-holes, start and end layers will suffice.
- If the Gerber files were originally generated from Altium NEXUS's PCB Editor, the Physical Layers order will be defined automatically. For other source PCB tools, you will need to assign this ordering manually.
- If you have the IPC-D-356 netlist for the design, you can load it into the current CAM document and use it to rename the nets to the original (and meaningful) net names that were assigned in the design.
- Although the IPC-D-356 netlist information is not essential to the export, it is desirable. Its presence will aid the CAMtastic Editor in separating the pads from the vias, and hence lead to the correct creation of vias instead of pads, for any blind or buried vias in the design.
- The generated PCB document will be added to the Projects panel as a Free Document, under the PCBs sub-folder. It is generated, but initially unsaved.