CAM Editor Feature Highlights

This article looks at some of the feature highlights of Altium Designer's CAM Editor (CAMtastic®), including ODB++ import and export, advanced panelization and direct export to Altium Designer's PCB Editor.

One of the essential steps in the development and manufacture of an electronic product is the fabrication of the PCB. Time to market pressures demand that the PCB design is transferred from PCB layout through to fabrication rapidly and error free.
To achieve this the fabrication company needs a sophisticated CAD/CAM tool that can load data generated from any PCB layout program, verify the data, panelize and prepare drilling and routing details, and output in the correct film and machine formats. Altium Designer's CAM Editor provides just such an environment and feature set to meet these requirements.

ODB++ Import and Export

The primary task of the CAD/CAM engineer is to accurately translate PCB design data into film and NC machine files, ready to fabricate the PCB. While Gerber and NC drill files continue to satisfy the needs of many companies, the increased complexity of PCBs, combined with the need for faster design turn-around has resulted in the emergence of new CAD/CAM data formats. The most popular of these, ODB++, captures all PCB fabrication and assembly data in a single, unified database.
You can take advantage of ODB++ functionality even if you have assembled your CAM data from other image/drill data, such as Gerber, NC Drill, IPC netlists, or HPGL files. In fact, the CAM Editor will gently nudge you in this direction by massaging imported layer names into an ODB-compliant format, just in case you want to use this technology. This door swings both ways - you may also export any of these traditional formats from data you imported from an ODB++ source.
The benefits of ODB++ go far beyond packaging relevant CAM files together; as far as imaging goes, it adds a whole new dimension to your CAM descriptions. Whereas Gerber files contain flash and draw instructions in a single list, layer by layer, ODB++ adds the concept of steps, which are like columns alongside each layer row. Once steps are defined, they may be nested within other steps, either as single instances or in arrays.

Apertures to Match

The CAM Editor supports an extensive set of aperture shapes/types - including all of those supported by ODB++. A single aperture list can hold up to 1000 separate aperture definitions (using D codes D00 to D9999). This range is typically broken down as follows:

• D0 - D9: reserved
• D10 - D9499: available for aperture definition
• D9500 - D9999: typically used for any defined tools.
  The aperture list also assists you during aperture definition/ modification, showing a preview of the aperture. This lets you see exactly how your aperture will change as you alter X:Y size, rotation or other parameter values. Interactive tool tips in this table will let you see how current values map to each shape's distinct dimensions.
    Whenever you import Gerber files into the CAM Editor without embedded aperture definitions, the import wizards will be consulted until a perfect match is found. The CAM Editor provides dozens of these wizards, matching aperture descriptions from both major and minor EDA programs, including both current and legacy formats. These wizards are also fully accessible for editing, should tweaking be required to achieve a perfect transfer of aperture list data. Existing wizards may also be used as templates for new wizards of your own.

Precise Data Verification

Many board designers use CAM tools for viewing only, visually examining the flashes and draws on each individual layer, cross-referencing their original design all the while. Such tests are valuable, but lack precision.

The CAM Editor can extract a virtual netlist from the connected copper areas in your image files, using drill data to follow nets between signal and internal plane layers. This process can also handle blind and buried via connections. To make this possible, the CAM Editor supports definition of physical layer stackup and drill layer pairing, but for the most part, these calculations are made automatically.
Extracting the netlist opens the door for other sophisticated verification tests. The CAM Editor can compare an extracted netlist to an IPC netlist generated from the original design, thus locating shorts or broken connections in complicated boards.

Design Rule Checking also becomes available once a netlist is extracted, isolating potential problems such as silkscreen over mask, solder bridging, net antennas or starved thermals. Eighteen design checks are available, covering a full range of possible fabrication problems. Half of these checks include an Auto Fix option, which automatically resolves the violation as it is found.
  Design rule violations can also be examined using the CAM panel. After running a design rule check ( Analysis » PCB Design Check/Fix ) the panel's DRC tab will automatically be made active. Any errors are listed by checking category. Click on an individual error within a category to highlight the offending object in the main design window. If the error can be automatically fixed, the command to do so will be available from the right-click menu for the error entry.

Advanced Panelization

A straightforward process allows a single board to fill a panel according to border and spacing information you provide. By using inherent ODB++ functionality, this is only the beginning of panelization in the CAM Editor. Additional data, such as drill coupons, tooling holes, or anything else you want to place may be defined in separate steps, then inserted on the panel alongside the array of board data. CAM files from different boards may be mapped to the same physical layer on the panel, meaning that you can fill your panel with any boards you want - assuming they all share the same stackup.

This freedom in panelization can benefit both fabrication and assembly houses. Fabrication houses will appreciate the ability to maximize the usage of panel real-estate, allowing them to combine jobs from different sources. Assembly houses, on the other hand, might take advantage of the Swap Layers Data command ( Edit » Layers » Swap Layers Data ) that lets you flip half of the boards on your panel. When this is done in a symmetrical way, the panel will be identical no matter which side is up. An assembly house receiving such panels will not require two separately configured pick-and-place machines, just one. After the components are placed and affixed on one side, the panel may be turned over and passed through the same machine again - cutting assembly costs considerably.
  A venting pattern may be applied to the unused sections of your copper layers, helping to even out the distribution of chemicals during etching. This pattern may be raster or vector, solid or shape-based. You may choose from generic shape options with user defined sizes, or even a pre-defined aperture.

Extensive NC Drill/Rout Features

Core to any effective CAD/CAM software is the ability to create both regular (drilled) and irregular (routed) holes in the PCB panel. The CAM Editor offers an array of automatic and manual tools to fulfill these needs. The flashes on a layer may be converted to drills, or used as the basis for the creation of a separate PTH drill layer. When either of these processes is run, any new drill bits will be automatically added to the Tool Table.
Irregular holes, such as rectangular slots or circular cut-outs in a board, can be defined with routing paths. These paths may be generated automatically wherever closed polylines exist - simply indicate the corner where the path should start and the direction the routing tool should move. You will maintain full control over tool parameters, plunge/retraction points and the path offset.
Instead of routing around a slot, you may want to mill a path that will shave away entire sections of a panel. The CAM Editor lets you do this automatically, showing you the back-and-forth pattern that the milling tool will follow. This tool is particularly valuable where you have assigned a Z-axis parameter to a tool that is less than the panel thickness - therefore creating an indentation on the board where you might want to mount a special component.
Once routing paths are defined, the CAM Editor allows tabs to be placed at intervals along the way, interrupting the continuous path with an instruction to extract the routing tool, then re-plunge a little further along the way. This allows boards to remain attached to the panel until they are intentionally broken off, perhaps after assembly is complete.

Direct Export to PCB

You can enjoy the ability to reverse-engineer boards from CAM data using a direct export facility between Altium Designer's CAM and PCB Editors. This process is not an export to the hard drive, but rather a direct load of layer primitives onto a PCB document within the application. This improves the quality of data that will be loaded into the PCB when only the image and drill information is available.
  The quality of the exported PCB will be increased when an IPC netlist is provided with the image and drill data. This file carries blind and buried via information, as well as the ability to differentiate between through-hole vias and free pads. Finally, this netlist will allow you to recover the original net names in your exported file, making the PCB easier to understand and manage.

Keeping CAM and PCB Data Synchronized

When generating fabrication output (ODB++ or Gerber, NC Drill, IPC Netlist) using an Output Job Configuration file (.OutJob), options are provided to automatically import the generated data into a new CAM document. These options are available from the Output Job Options dialog, accessed from the *Tools menu when the Output Job file is active.
After checking the data in the CAM document, you may find that changes are required to the source PCB design. Upon generating new fabrication files you will typically (and naturally) wish to have the new data imported into the same CAM document - essentially keeping the two synchronized. To prevent subsequently generated data being imported into a new CAM document each time, enable the Reset auto-load options after generation option in the same dialog.

Rescan and Reload-based commands will only become available if the Reset auto-load options after generation option is enabled prior to initial generation of fabrication output.

Note that enabling this option does not mean that the newly generated data will be automatically imported into the existing CAM document, rather these changes must be manually imported. Select the layer(s) to be modified in the Layers region of the CAM panel, then right-click and use the following two commands to load the new data from the PCB:

• Rescan/Rescan Selected
  - using this command performs a date comparison for all selected layers between data (Gerber/ODB ++ feature) existing in the active CAM document and that last generated from the same source PCB document. If the last generated data is newer than the existing data, the Reload command will be enabled
• Reload/ Reload Selected
  - use this command to regenerate the data for all selected layers that have been detected by the Rescan process to have been changed. All changes to the layers will be taken into the active CAM document in order to resynchronize with the source PCB document.

  Additional Features

The following is a list of additional features related to the CAM Editor. The list is by no means exhaustive, but rather an indication of just a few more of the features that make the CAM Editor a powerful CAM tool.

Macros

Macro functionality allows you to automate common or complicated tasks. Recording a macro generates a script using Altium Designer's EnableBasic scripting language. When you stop recording a macro, the generated script file (*.bas) will be opened automatically as the active document in the main design window. The underlying macro script can be edited at any stage.

Reports

A number of reports can be generated from the CAM Editor's Reports menu, including:

• Drill report (Drill.rpt) - lists, for each drill tool that has been defined, the drill size and the number of drill points existing in the design document
• DCode/Layer Usage report (Dcode-Layer.rpt) - lists D code and layer information for the current document. For each D code, shape and size information is listed, as well as usage, in terms of the number of flashes and draws. For each layer, extent information is listed, as well as a breakdown of the number of flashes and draws contained thereon.
• DRC/DFM report (DrcReport.rpt) - provides a summary of the violations found and, for each rule check that has been violated, the number of violations Found , Fixed and Remaining are listed. Note : A Design Rule Check (DRC) must be performed before such a report can be generated.
• Netlist report (Netlist.rpt) - used to export simple netlist information from the current document, in ASCII format. The name and extension of this report can be changed if required.
• Rout/Mill report (Rout.rpt) - lists all defined rout/mill paths for the current document with tool numbers, sizes, number of instances for each tool and the distance of each routing/milling path.
• X:Y Coordinates report (X-Y List.rpt) - lists each point, line and arc currently selected in the workspace, in terms of XY coordinates within the workspace.

Document Navigation

The main design window for the CAM Editor does not include any scrollbars. Navigation of a document can easily be achieved however, using a combination of the keyboard and the mouse:

• PAGE UP / PAGE DOWN - zoom in/out
• CTRL + Mouse-wheel - zoom in/out
• Mouse-wheel - pan up/down
• Mouse-wheel down & drag/Right-click & drag - pan the workspace in any direction.
• SHIFT + Mouse-wheel - pan left/right

Workspace Preferences

Many commands that pertain to workspace preferences and setup options will, when launched, give access to the relevant page of the system-wide Preferences dialog. Define the options on these pages as required. Preference settings can be saved and loaded into this dialog, allowing you to always have you favorite/required workspace settings at your fingertips.
This dialog can also be accessed from DXP » Preferences .