Search In: Doc:Documentation: Altium Designer
Altium DesignerAltium 365Altium MCAD CoDesignerAltium CircuitMakerCompany DashboardAltium On-Prem Enterprise ServerAltium Infrastructure Server
Ver: Version: 25
252423222120.220.1
Close
Suche Search on Documentation

Support for Import & Export in the Altium Designer CAM Editor

Created: Februar 06, 2023 | Updated: Februar 06, 2023 | Applies to versions: 23, 24 and 25

Importing Files Using Quick Load

The Quick Load command allows you to import all CAM files located in a single folder. Quick Load imports all traditional CAM documents (e.g., Gerber, ODB++, Aperture List Files (*.lst), and IPC-D-356 netlists) that are stored in a single folder. If your board has any holes, e.g., through holes or blind or buried vias, you must provide, at the very least, the signal layers (e.g., Gerber files for top and bottom) and one or more NC Drill file (Excellon 2 format).

The File » Import menu includes separate commands that allow the import of selected Gerber, ODB++, netlist (IPC-356-D), NC Drill, and Mill/Rout.

Setting Up Import Options

Before importing the Gerber, NC drill, and netlist files into the new CAM document, you may set up import options, such as the Gerber Import settings. To do so, select File » Setup » Import/Export from the main menu to open the CAM Editor - Import/Export page of the Preferences dialog.

Click on Import Settings from the Gerber Import (Default) area to display the Gerber Import Settings dialog, where you may set up the default import settings for Gerber files.

You may specify if you would like the CAM Editor to create new layers, even if layers with identical layer types already exist, or to use the existing layers. Using the existing layers may be useful when loading data for more than one board in the same files using different steps in order to panelize the loaded PCBs onto the same CAM panel, which is known as multi-step panelization.

To check the file extensions or add a new extension, click on the CAM Editor - Miscellaneous page of the Preferences dialog.

The file extensions listed here determine the type of an imported file, for example, a quick load of Gerber files will look for and load all files with an *.A, *.G . or *.PHO extension. You may add any additional extensions required, separated by a semi-colon (;) from the previous entry.

Importing CAM Files Using Quick Load

To import the Gerber, NC Drill, and netlist files into the new CAM document (File » New » CAM Document), select File » Import » Quick Load from the main menu to open the File Import - Quick Load dialog.

Use this dialog to browse to the folder containing the files you wish to import, and select the required files.

Click the Gerber Options button to open the Import Gerber Options dialog, from where you can set up various advanced import options with respect to Gerber files.

Click the Default Units button to open the File(s) Import Settings dialog, from where you can define the numerical formatting to be applied to imported Gerber files.

If the Gerber files you wish to import are in a format that do not include embedded apertures, you must load a separate aperture file. Use the drop-down in the lower section of the dialog to specify the aperture list format (template) to use during import.

After defining the file path and options as required, click OK to begin importing the files. If any errors are encountered during the import, they are listed in a text file (Log<Date><Time>.log), which is generated and opened as the active document in the design space.

When the Gerber files have finished importing, the Import Drill Data dialog will open.

Once completed, NC files will be imported into the CAM Editor and display in the design space along with a Quick Load Process Report log file. IPC netlist files will be loaded last.

  • The aperture list format/template you select should be for the tool from which your aperture and Gerber files were generated. If you do not know the source software used to generate the Gerber files, use the Auto-Detect Apertures entry (default).
  • File types will only be included in the import if they have been enabled for inclusion in the Quick Load region, on the CAM Editor - Miscellaneous page of the Preferences dialog.
  • The error log is generated and saved automatically in the \Users\<ProfileName>\AppData\Roaming\Altium\Altium Designer <GUID>\CAMtastic\LogFiles folder of your software installation. The report will appear in the Projects panel as a free document
  • When using Altium Designer's PCB Editor to generate fabrication outputs, options are available to auto-load generated Gerber/ODB++, NC Drill, and IPC Netlist files into the CAMtastic Editor, upon running a batch output generation.

Importing ODB++ Files Using Quick Load

The ODB++ import option imports ODB++ files into the CAM Editor. If the NC drill data has been generated from the PCB Editor, you must separately import the NC drill data after the ODB++ import has been completed. Other CAD/CAM packages should already have the drill hole data present in the ODB++ structure, therefore a separate import of the NC drill data is unnecessary.

To do so, select File » New » CAM Document from the main menu. Next, select File » Import » Quick Load to open the File Import - Quick Load dialog.

Once the files have been imported, the Steps Table dialog will open. This dialog displays all of the ODB++ steps that have been defined in the loaded ODB++ database for the current document. Steps are identified by Step Name and the Object Count associated with that step.

Once all default values for step assignment and the design are imported, a log file will be produced. The Steps tab in the CAM panel will be refreshed, where you may add or modify steps by right-clicking and selecting the appropriate command from the pop-up menu.

Importing Gerber Files

To import one or more Gerber files into the current document, choose the File » Import » Gerber command from the main menus. After launching the command, the Select Gerber File(s) dialog will appear. Use the dialog to locate and open the required Gerber file(s). Multiple files can be selected.

After clicking Open, the Import Gerber(s) - Options dialog will appear. Use this dialog to manually define import settings.

If the Auto Detect Gerber Formats option is enabled, all options and settings required for the Gerber format being imported will be detected automatically.

After setting options as required, clicking OK will proceed with the import, bringing the data from the Gerber file(s) into the current document - each file imported becoming an individual layer in the CAMtastic Editor.

  • You may want to open a new, blank CAM document, before importing the Gerber file(s).
  • If you have a folder containing multiple Gerber files, all of which you want to import, use the Gerber Quick Load feature.
  • RS-274, RS274X, and Fire9000 Gerber file formats are all supported by the CAMtastic Editor.
  • The Gerber RS-274 format requires a separate Aperture file to be included at import, while the extended versions (Gerber RS-274-X and Fire9000) use embedded apertures inside the Gerber files, and therefore do not require a separate Aperture file to be imported.

Importing ODB++ Data

To import ODB++ data into the current document, choose the File » Import » ODB++ command from the main menus. After launching the command, the Choose Directory dialog will appear. Use the dialog to browse to, and select, the ODB++ root folder.

After selecting the required ODB++ folder and clicking OK, the Steps Table dialog will appear. This dialog lists all of the defined steps that currently exist and gives an object count for each. Click OK - the ODB++ data will be imported into the current document. The currently defined steps will appear on the Steps tab of the CAMtastic panel.

  • ODB++ data can only be imported into a new, blank CAM document. If data already exists in the current CAM document - from a prior Gerber, or ODB++ import - a dialog will appear alerting you to this fact and you will be prompted to import into a new CAM document.
  • The ODB++ format uses a standard file system structure. A job in ODB++ is represented by a self standing directory tree, which means the job tree can be transferred between computer systems without loss of data. All files in ODB++ are readable ASCII files.
  • A database job is a single folder, composed of the following sub-folders: fonts, input, matrix, misc, steps, symbols, and user.
  • The steps folder contains a collection of layers - physical board layers, mask layers, NC drill, etc, and a collection of netlists.
  • The symbols folder has single layer graphic entities which can be referenced from within any graphical layer in a step.
  • The matrix folder has definitions of the physical order of the layers, and the relation of drill layers (through, blind, buried, etc.).

Importing Netlist

To import an IPC-D-356 formatted netlist into the current document, choose the File » Import » Netlist command from the main menus. After launching the command, the File Import - Netlist dialog will appear. Use the dialog to locate and open the required netlist file. After clicking OK, the file will be imported and the relevant netlist layers (*.ipc) will be added to the layers list in the CAMtastic panel.

  • Protel formatted netlists are not supported. The imported netlist must be in the standard IPC-D-356 format.
  • If the IPC netlist has been imported correctly, you will see two layers added to the layers list in the CAMtastic panel: <fabrication_testpoint_report_for_DesignName>.ipc_t and <fabrication_testpoint_report_for_DesignName>.ipc_b, reflecting netlist information for the top and bottom signal layers. (A third layer, <fabrication_testpoint_report_for_DesignName>.ipc_in, will appear if you have internal signal layers in your PCB design. Unless you have blind and/or buried vias involving these layers, this third layer will be empty and can be left, or deleted, from the layers list).
  • If using Altium Designer's PCB Editor, the IPC netlist is created by generating a testpoint report and selecting IPC-D-356A as the output format. The individual options available for this format should be left disabled.

Importing NC Drill Files

To import NC drill information related to your design, select File » Import » Drill from the main menu to open the File Import - NC Drill dialog. Use the dialog to locate and select the required drill file(s). Multiple files can be selected if necessary. The file extension for NC Drill data created in the Altium Designer PCB Editor is .txt.

The Import Drill Data dialog will display after the NC Drill files have been imported. In this dialog, you can specify start units, shape/default hole size and gain access to the Tool Table dialog.

Once the defaults are accepted, the NC drill data will be imported on a separate layer whose layer name is based on the file name, for example, _4_port_serial_interface.txt_. A log file will also be produced. The Tool Table dialog will be updated accordingly with the individual tools.

  • Each drill file contains tool numbers for each drill bit, and X and Y locations for each instance that bit is used on the board.
  • Clicking the Units button in the Import Drill Data dialog will open the NC Drill Import Settings dialog, from where you can specify exactly the starting units in terms of digits, units, type, and zero suppression.
  • The CAMtastic Editor imports ASCII drill files only. When NC Drill data has been generated from the PCB Editor, the file used has the extension .TXT. This file will be loaded automatically into the CAMtastic Editor after generation, if the Open outputs after compile option is enabled, on the Options tab of the Options for Project dialog.

Importing Mill Rout Files

Create a new CAM file by selecting File » New » CAM Document from the main menu, then select File » Import » Mill/Rout to open the File Import - Mill/Rout dialog. Use this dialog to locate and open the particular file(s) you wish to import.

After clicking OK, the Import Mill/Route Data dialog will appear. Click the Units button to open the Mill/Rout Import Settings dialog, from where you can define the numerical formatting for the imported data. Specify the default tool size to use on import, or click the Tool Table button to open the Tool Table dialog, from where you can modify drill tool definitions.

After clicking OK, the data will be imported on a separate layer whose layer name is based on the filename, for example, 'cam.rte'. A log file is also produced. If you want to modify the Mill Rout layer, you must be in the NC Editor mode. Select View » NC Editor to access the Rout menu options.

The following NC data file formats are supported: *.dr*, *.rou, *.rte, *.nc*, *.tx*. When generating NC Drill data from Altium Designer's PCB Editor, the drill data is stored in a file with the extension .txt.

See the Data Verification page for more details on working with and verifying imported data.

Importing Aperture Files

If there are no embedded apertures included in the files you want to import, you may use the following commands:

  • To import an aperture file, the contents of which are used during Gerber file import, using pre-determined template formats, select File » Import » Aperture File (using Wizard formats). After launching the command, the Open Aperture File dialog appears. Select the required aperture list format from the Existing wizard formats drop-down list. Either type the full path and name of the required aperture file directly into the Aperture file field or click on the Browse button to access a standard Open dialog, from where you can navigate to, and open, the required file.

    • When Gerber files have been generated using standard apertures and EDA tools, the CAMtastic Editor will automatically detect the apertures being used when importing the files. This command is useful when there is a problem with Gerber import - possibly because the format of the apertures is unknown, or the apertures have been customized.
    • The wizard format you select should be for the tool from which your aperture and Gerber files were generated. If no wizard format is selected, using the Browse button will run the Open dialog with file type *.LST selected. This is the default CAMtastic aperture file format.
    • Wizard formats can be edited and created in the Aperture Wizard dialog (Tables » Aperture List Wizard).
  • To import a Custom Aperture Library file (.lib) by selecting File » Import » Custom Aperture Library File (.LIB). After launching the command, the Open Custom Aperture .LIB File dialog will appear. Use this dialog to locate and open the particular custom aperture library file (*.lib), whose apertures you wish to import into the current document. The imported apertures will be available for editing in the Edit Apertures dialog (Tables » Apertures).

Exporting Files from the CAM Editor

All CAM Editor outputs are generated through the File » Export menu. You will need to export files when you have made modifications to the original outputs or if you require the Test Point or NC Drill data saved in Gerber format.

If you have generated files from your PcbDoc or Output job file, it is not necessary to regenerate these files again from the CAM editor if no changes have been made.

The following export options are available when in the CAM Editor:

  • Gerber

  • Netlist

  • IPC-D-350

  • Save Drill

  • Mill/Rout

  • DXF

  • Part Centroids

  • Aperture List

  • Library

  • Bitmap (*.bmp).

You must be in NC Editor mode to access the Drill export option.

If saving a file with the same name and in the same location as an existing file, the existing file will be overwritten without warning.

For more information about exporting to Altium Designer, see the Reverse Engineering PCBs page.

Exporting Gerbers

Select File » Setup » Import/Export from the main menu to open the CAM Editor Import/Export page of the Preferences dialog. Make sure the default export format is RS-274-X, which is the extended Gerber format that includes the aperture definitions, also known as embedded apertures.

Click the Export Settings button to display the Gerber Export Settings dialog, where you can set up the default export settings for Gerber files.

Select File » Export » Gerber from the main menu to open the Export Gerber(s) dialog.

Use this dialog to define various export options, including whether to use Step & Repeat Codes, whether to separate and export composite layers as individual files, and also to define the Gerber format.

By default, the exported Gerber format will initially be set to RS-274-X. By pressing the RS-274-X button repeatedly, you can cycle through the available Gerber formats: RS-274, RS-274-X, or Fire9000.

Press the Settings button to open the Gerber Export Settings dialog, from where you can define the numerical formatting for the exported files.

After defining the export options as required, click on the OK button - the Write Gerber(s) dialog appears.

Select the Gerber files you wish to export by enabling them in the Writer Gerber(s) dialog. Alternatively, you may select the files for exporting using the right-click menu selections or use the Spacebar key to toggle the selection. By default, all Gerber files are selected for export. Each file can be renamed by clicking within the name field. The associated file extension can also be changed to another if required, by again clicking directly within the name field or, alternatively, right-clicking on the entry and choosing File Extensions from the context menu. The new extension required can be typed into the subsequent Enter Value dialog that appears.

Choose a location for the exported files by clicking the Browse for Folder () button.

  • Note that the OK button is disabled if the format of the output file name is incorrect. The output file names must not contain any spaces or capitals and must not exceed 64 characters. Double-click on a filename to type in a new filename. To change the filename extension, select the Gerber filename and then right-click and select File Extensions. Enter a new extension (three characters maximum) in the Enter Value dialog and click OK.
  • Gerber format RS-274 files require a separate aperture file, while extended formats RS-274-X and Fire9000 do not (as all apertures are embedded inside the Gerber files).

Exporting ODB++

To export data from the current document in ODB++ format, choose the File » Export » ODB++ command from the main menus. After launching the command, the Write ODB++ dialog will appear. Use this dialog to define where the exported data is to be stored. By default, the data folder that is generated will take the name job. The folder can be renamed by clicking within the name field and modifying the name as required.

With name and storage location defined as required, click OK to generate the output.

  • The ODB++ format uses a standard file system structure. A job in ODB++ is represented by a self standing directory tree, which means the job tree can be transferred between computer systems without loss of data. All files in ODB++ are readable ASCII files.
  • A database job is a single folder, composed of the following sub-folders: fonts, input, matrix, misc, steps, symbols, and user.
  • The steps folder contains a collection of layers - physical board layers, mask layers, NC drill, etc, and a collection of netlists.
  • The symbols folder has single layer graphic entities which can be referenced from within any graphical layer in a step.
  • The matrix folder has definitions of the physical order of the layers, and the relation of drill layers (through, blind, buried etc).

Exporting Netlists

You may export netlists in two formats. To do so, use the File » Export » Netlist command to export a netlist in IPC-D-356 format (.net). You may also use the File » Export » IPC-D-350 to export an IPC-D-350 netlist (.ipc). You must have a netlist extracted from the imported data to utilize these commands. If you have not already extracted the netlist, select Tools » Netlist » Extract.

Select File » Export » Netlist to open the Write IPC-D-356 dialog.

From the Write IPC-D-356 dialog, select the .net file and choose a location and filename for this netlist report. By default, the data file that is generated will take the name cam.net. The file can be renamed by clicking within the name field. The associated file extension can also be changed to another if required, by again clicking directly within the name field or, alternatively, right-clicking on the entry and choosing File Extensions from the context menu. The new extension required can be typed into the subsequent Enter Value dialog that appears.

With name, extension, and storage location defined as required, click OK to generate the file.

  • For the netlist to export successfully, Top and/or Bottom layer types must be defined in the Layers Table dialog (Tables » Layers), as well as Drill Top, or Drill Bottom.
  • The physical order of the signal and plane layers must also be defined in order to successfully generate the IPC-D-356 netlist file. If a warning dialog appears alerting you to this fact, you will need to define this ordering in the Create/Update Layers Order dialog (Tables » Layers Order).

Exporting IPC-D-350

To export the current document in IPC-D-350 format, choose the File » Export » IPC-D-350 command from the main menus. After launching the command, the Write IPC-D-350 dialog will appear. Use this dialog to define where the exported file is to be stored. By default, the data file that is generated will take the name cam.ipc. The file can be renamed by clicking within the name field. The associated file extension can also be changed to another if required, by again clicking directly within the name field or, alternatively, right-clicking on the entry and choosing File Extensions from the context menu. The new extension required can be typed into the subsequent Enter Value dialog that appears.

With name, extension, and storage location defined as required, click OK to generate the file.

Exporting Drill Files

To export drill data with respect to one or all layers in the current document, enter NC Editor mode by selecting View » NC Editor from the main menu, then select File » Export » Drill to open the Export Drill Data dialog. Use the dialog to select a specific layer or all layers to export drill data for.

The Header region of the dialog allows you to specify the Part Program Header information required.

Click the Units and Tool Table buttons to make changes to the data format and defined tools respectively.

You can also choose whether or not to use Step & Repeat Codes in the exported data and also whether a report file is generated.

After setting up the export options as required, click the Save button - the Write Drill dialog will appear.

Use this dialog to define where the exported drill file is to be stored. By default, the data file that is generated will take the name cam.drl. The file can be renamed by clicking within the name field. The associated file extension can also be changed to another if required, by again clicking directly within the name field or, alternatively, right-clicking on the entry and choosing the File Extensions command from the context menu. The new extension required can be typed into the resulting Enter Value dialog that appears.

  • The Drill file contains tool numbers for each drill bit, and X and Y locations for each instance that bit is used on the board.
  • The report file that is generated will have the default name cam.rpt and contains a summary of the tools used and the number of instances that drill points for those tools are specified in the current document. It will be written to the same folder as the drill data file.
  • The Part Program Header is used to perform setup and initialization tasks, such as loading tool data and cutting information.
  • Step & Repeat commands are available for features such as panelization and data arrays. They basically enable the use of looped code instead of rewriting identical sequences, therefore reducing the size of generated files.

To export drill data with respect to a specified layer in the current document, enter NC Editor mode by selecting View » NC Editor from the main menu, then select the File » Export » Save Drill command from the main menus. After launching the command, the Export Drill Data dialog will appear. Use the dialog to select a specific layer to export drill data for. Click the Units button to make changes to the data format, through the NC Drill Export Settings dialog.

After setting up the export options as required, click the OK button - the Write Drill dialog will appear. Use this dialog to define where the exported drill file is to be stored. By default, the data file that is generated will take the name cam.drl. The file can be renamed by clicking within the name field. The associated file extension can also be changed to another if required, by again clicking directly within the name field or, alternatively, right-clicking on the entry and choosing the File Extensions command from the context menu. The new extension required can be typed into the resulting Enter Value dialog that appears.

The Drill file contains tool numbers for each drill bit, and X and Y locations for each instance that bit is used on the board.

Export Mill/Rout Data

To export Mill/Rout data from the current document, choose the File » Export » Mill/Rout command from the main menus. After launching the command, the Export Mill/Rout Data dialog will appear. Use the dialog to select whether you wish to export data for an individual layer, or for all layers in the current document. The Header section of the dialog is already loaded. If you need to change the header in any way, simply edit the information directly in the window.

Press the Units button to open the Mill/Rout Export Settings dialog, from where you can define the numerical formatting for the exported file.

Press the Tool Table button to open the Tool Table dialog, from where you can modify drill tool definitions.

If you have used any Step & Repeat arrays in the design, you can enable the option to Use Step & Repeat Codes (M25) in the exported data file.

After clicking the Save button, the Write Mill/Rout dialog will appear. Use this dialog to define where the exported file is to be stored. By default, the data file that is generated will take the name cam.rte. The file can be renamed by clicking within the name field. The associated file extension can also be changed to another if required, by again clicking directly within the name field or, alternatively, right-clicking on the entry and choosing File Extensions from the context menu. The new extension required can be typed into the subsequent Enter Value dialog that appears.

Exporting DXF

To export the selected layers of the current document in .dxf format, for use with AutoCAD, choose the File » Export » DXF command from the main menus. After launching the command, the Export DXF/DWG dialog will appear. The top section of the dialog allows you to specify which layers of the current document you wish to export information for. The Output Control section of the dialog allows you to specify whether lines will be exported as zero width outlines, or filled lines (with, or without end caps). You can also filter out any unwanted Dcodes and convert text to polylines (Plines).

After setting up the export options as required, click the Save button - the Write AutoCAD DXF dialog appears. Use this dialog to define where the exported file is to be stored. By default, the data file that is generated will take the name cam.dxf. The file can be renamed by clicking within the name field. The associated file extension can also be changed to another if required, by again clicking directly within the name field or, alternatively, right-clicking on the entry and choosing File Extensions from the context menu. The new extension required can be typed into the subsequent Enter Value dialog that appears.

With name, extension, and storage location defined as required, click OK to generate the file.

  • By default, all detected layers in the current document are selected for export in the Export DXF/DWG dialog.

  • The use of end caps with filled lines is a military specification, and causes the exported image to appear in AutoCAD exactly as it appears in the CAM document.

  • DXF files created from Gerber information can become very large. Using the Zero Width line output option will reduce the size of the resulting file.

  • Multiple Dcodes can be filtered out of the exported DXF file. Use a comma and/or space between Dcodes, when specifying them in the Dcode Filter field, and don't include the D prefix. For example, entering 10, 19 will result in all objects using Dcodes D10 and D19 not being exported in the resulting DXF file.

Exporting Part Centroids

To export the parts list for the current document, choose the File » Export » Part Centroids or Tables » Parts command from the main menus. After launching the command, the Export Part Centroids dialog will appear. Part information will only be listed if you have previously created and grouped parts (and optionally assigned reference designators). The following information is listed for each part:

  • Ref. Des. - the reference designator, if any, that you have assigned to the part.
  • X - the X coordinate of the center of the part's center cross.
  • Y - the Y coordinate of the center of the part's center cross.
  • Board Side - whether the part is surface mount (Top or Bottom) or thru-hole (Thru).
  • Rotation - the part's orientation.
  • Part Name - the description given to the part (e.g. DIP14).

Clicking the Export List button will open the Write Centroid Parts dialog. Use this dialog to define where the exported file is to be stored. By default, the data file that is generated will take the name cam.pcf. The file can be renamed by clicking within the name field. The associated file extension can also be changed to another if required, by again clicking directly within the name field or, alternatively, right-clicking on the entry and choosing File Extensions from the context menu. The new extension required can be typed into the subsequent Enter Value dialog that appears.

With name, extension, and storage location defined as required, click OK to generate the file.

Any information you change in the dialog will be applied during the export only, and not to the created parts in the document. If you make unwanted changes, simply close and reopen the dialog - the original information will be present.

Exporting Aperture List

To generate an aperture list for the current document, choose the File » Export » Aperture List command from the main menus. After launching the command, the Write Aperture List dialog will appear. Use this dialog to define where the exported file is to be stored. By default, the data file that is generated will take the name Aper.lst. The file can be renamed by clicking within the name field. The associated file extension can also be changed to another if required, by again clicking directly within the name field or, alternatively, right-clicking on the entry and choosing File Extensions from the context menu. The new extension required can be typed into the subsequent Enter Value dialog that appears.

The generated report (which by default is not opened automatically) contains numerical formatting information, as well as Dcode information for all used Dcodes in the design.

Exporting Aperture Library

To generate a custom aperture library file, containing all custom aperture shapes that you have defined for the current design document, choose the File » Export » Aperture Library command from the main menus. After launching the command, the Write Aperture List dialog will appear. Use this dialog to define where the exported file is to be stored. By default, the data file that is generated will take the name Aper.lib. The file can be renamed by clicking within the name field. The associated file extension can also be changed to another if required, by again clicking directly within the name field or, alternatively, right-clicking on the entry and choosing File Extensions from the context menu. The new extension required can be typed into the subsequent Enter Value dialog that appears.

Exporting Bitmap

To save data from the CAM document as a bitmap, choose the File » Export » Bitmap (*.BMP) command from the main menus. After launching the command, the cursor will change to a small square and you will be prompted to select objects to include in the bitmap. Simply position the cursor over an existing object that you wish to include in the selection and click. Clicking away from an object allows you to drag a selection area, for including multiple objects in the selection. Selection is cumulative.

Once all required objects have been selected, right-click. The Export Bitmap dialog will appear. Use the dialog to specify the resolution for the image (in Dots Per Inch) and the color scheme (either monochrome or color). As you change the DPI resolution, the final size for the bitmap, in pixels, will update accordingly.

After defining the options as required, clicking OK will bring up the Save As dialog. Define the storage path and name for the bitmap, and click Save - the bitmap will be generated.

The default background for exported bitmaps is white.

Exporting Graphite

To save data from the CAM document as a Graphite binary file (*.grz), choose the File » Export » Graphite command from the main menus. After launching the command, the Save As dialog will open. Define the storage path and name for the file, and click Save - the file will be generated.

If you find an issue, select the text/image and pressCtrl + Enterto send us your feedback.
Note

The features available depend on your Altium product access level. Compare features included in the various levels of Altium Designer Software Subscription and functionality delivered through applications provided by the Altium 365 platform.

If you don’t see a discussed feature in your software, contact Altium Sales to find out more.

Content