EasyEDA Pro supports importing into Altium Designer.
Several versions of Altium Designer have been supported, supporting plaintext ASCII format. At present, there is a problem with importing binary format, which is not supported for the time being.
- Due to the inconsistency of the format and graphic element design, there may be some differences after the graphic element is imported, please check carefully. For specific differences, please refer to the help documentation.
- Jia Lichuang EDA is not responsible for any losses caused by format conversion differences, if you do not agree, please do not import.
Import Altium project file
Open the schematic diagram and PCB in Altium Designer, in “File - Save As”, select “altiumvanced Schematic ascii(*.SchDoc)” or “PCB ASCII File(*.PcbDoc)”
footprint the exported schematic diagram and PCB files into a compressed footprint ZIP format. Compression format only supports zip.
Note: It also supports the import of a single schematic or PCB, but the import of a single schematic cannot automatically bind the footprint, and it needs to be manually bound after import.
- On the professional version start page - import Altium to import.
Click OK and select the imported file.
When importing, you can choose different options according to your needs.
- Importing files
- Extract library files
- Import files and extract libraries
Via solder mask extension:
- All are covered with oil by default. It will force all vias to be covered with oil (solder mask extension is set to -1000)
- follow the original setting. It will be set according to the solder mask parameters of the vias in the original altium file.
- From the Keepout layer. Many users use the keepout layer to draw borders, so this layer is used as the border by default.
- From mechanical level 1. When mechanical layer 1 is selected, the closed keepout layer will be turned into a forbidden area, and the unclosed keepout layer will be transferred to the mechanical layer.
The difference before and after format conversion is as follows:
| Elements/Layers | After Import | Notes |
| :— | :— | :— |
| Bus/bus entry | Import is not supported | The bus and bus branch of the professional version are designed differently from altium and cannot be directly imported and used |
| Pictures | Import is not supported | altium pictures are stored in local file paths, and ASCII files do not contain pictures |
| Off Sheet Connector | Converted to Circular Network Identifiers | Offmap Connectors are not supported in Pro Edition |
| Sheet Symbol | Imported as hierarchical icons | Pin styles for page breaks are not supported |
| Sheet Entry | Does not support import | Professional version does not support drawing entry |
| Device Sheet symbol | Does not support import | Professional version does not support device page symbol |
| Harness | Import is not supported | Harness entities are not supported in Professional Edition |
| Directives | Some does not support import | The professional version supports No ERC labels, and does not support other indication entities (differential pairs, parameter settings, coverage areas, compilation shields) |
| Text/Text Frame/Comment| Import as normal text| The professional version does not support comments at the moment. If the corresponding font is not installed in the operating system, the default font will be used after the text is imported, and the position of the text may be slightly shifted due to different fonts; When the altium file is saved as ASCII, the Chinese may be garbled, and the garbled characters will be automatically converted to underscores after import |
| Bezier curve/ellipse arc/ellipse | Import as multi-segment polyline | Professional version does not support Bezier curve, Bezier curve, ellipse arc, ellipse |
| Component Designator | Multi-part designator as U1A, U1B after import is U1.1, U1.2 | The professional version does not support the multi-part designator method like altium |
| Pin type | Unsupported types are converted to input types | The professional version only supports three pin electrical types |
| Hidden pins | Show after import | Professional version does not support hidden pins |
| Component footprint | After importing, “original footprint 1, original footprint 2, etc.” will be generated | The professional version is not associated with the footprint name, but with the uuid of the footprint, so when importing, multiple previously associated footprint names will be altiumded as common attributes |
| Theme style | The default theme of the professional version is used in the import dialog box | The default theme is that the rounded rectangle is converted to a right angle, the fill color is not preserved, and the color of the primitive is not preserved, so as to switch the schematic theme, and the theme of the original file follows the original file Style, color does not change when switching themes |
| IEEE symbols | Some IEEE symbols are not yet supported for import | The new version of altium has new IEEE symbols, some of which are not supported for import |
| Elements/Layers | After Import | Notes |
| :— | :— | :— |
| Polygon Pour | polygon pour will be re-laid after importing | Because the polygon pour logic is different, the polygon pour filling of the PCB will also be slightly different. For example, heat welding generation method, heat welding width, whether heat welding is generated (priority will be avoided to avoid heat welding for graphics elements with wrong DRC spacing), and flying lines may be generated; horizontal and vertical polygon pour will be converted to grid polygon pour; altium polygon pour on the grid will heat and weld the vias separately, which is not supported by the professional version, and some vias may not be connected to the polygon pour after rebuilding the polygon pour (when the grid is relatively large); the professional version does not support non-signal layers polygon pour, so the polygon pour on other layers of altium will be transferred to the top layer polygon pour|
| Design Rules | Some design rules do not support import | For example, custom altiumvanced design rules, design rules not supported by the professional version, common safety spacing, etc., the parameters of the imported PCB file rules need to be altiumjusted by yourself |
| Text/Text Box| Font changes and positions will be slightly offset| If the corresponding font is not installed in the operating system and the professional version of the font setting does not altiumd the corresponding font, the text will use the default font (Arial and Times New Roman) after importing, due to the text There may be a slight offset in different positions of the font; if it is the same font, because the font display logic is different, it cannot be completely consistent with the original file, and there will be position offset and size difference; strokes and barcodes will be converted to normal text |
| Internal Electrical Layer | The network of the block may change after importing | The implementation of the internal electrical layer of altium and the professional version is different. When there are multiple internal electrical blocks, the network of the blocks may not be completely consistent, so you need to be careful Check; the internal electrical layer will rebuild the block after importing, and the internal electrical layer block division may also be different |
| keepout layer| is converted to frame layer by default| In the import pop-up window, it is supported to set whether the source of the frame is the keepout layer or the mechanical layer 1; the keepout closed lines inside some boards will automatically be converted to the corresponding forbidden area according to the target; Closed keepout primitives will be imported to the mechanical layer. The professional version does not support independent lines as forbidden areas |
| Board Shape | Go to the document layer by default | The professional version does not have a board shape but has a border layer. Since most people use keepout and mechanical layer 1 as the board frame, the board shape goes to the mechanical layer |
| Define Board Cutout | Go to the frame layer or convert to the cutout area | This function corresponds to the cutout area of the professional version |
| Polygon Pour Cutout | Convert to prohibited area | Convert to multi-layer prohibited area, the prohibited content is polygon pour |
| Mechanical Layer | Mechanical layer 1 is transferred to the mechanical layer by default, and other mechanical layers are transferred to the user-defined layer | The professional version uses the user-defined layer to realize the functions of other mechanical layers of altium |
| Ratlines | Flying lines appear after importing | It may be that the reconstruction of polygon pour after importing lealtiums to disconnection in some places, such as no network primitives, heat welding cannot be generated due to DRC spacing, etc. |
| Room | Does not support import | Professional version does not support Room primitives |
| Layer Stack Settings | Import is not currently supported | To be supported later |
| 3D Body/3D Model Library | Does not support import | The 3D binding design of the professional version is different from altium |
| Drill table | Import to Drill layer | Professional version has separate Drill layer |
| Solder Mask and Paste Mask Extension| Only pad/vias support import | Solder mask and Paste Mask extensions of other wires, arcs and other primitives do not support import. If they are independent primitives, they will be in the solder mask or solder flux layer (solder paste layer) generate an expanded primitive |
| Pad | Import to the bottom layer or top layer or multi-layer | Professional version of the pad does not support setting in any layer, the pad of the unsupported layer will be converted to the filling area of the corresponding layer; the rectangular drilling is not supported, it will be converted to Groove Drilling |
| Component/Footprint|Import to the top layer or bottom layer| If the footprint attribute drawn in altium is on the top layer, but the whole is on the bottom layer (belonging to wrong data), it will automatically correct the layer attribute to be on the bottom layer after importing; if there are multiple files with the same name but different sizes footprint, the import will take one of them as a template by default to associate with other components |
| Coordinates | Import as Text and Lines | Coordinate primitives are not supported in the Professional Edition |
| Dimensions | Partial support for import | Support for importing linear dimensions, angles, and dimensions, but not for partial import as text and lines |
| Object from file | Import not supported | This calls an object outside the file, not contained in the file, and does not support import |
| Work Guides | Import is not supported | This element is not supported in Professional Edition |
Please do not repeatedly export your schematic or PCB to altium format and import them again, this operation may cause loss of details! ! !
When importing Altium files, if there are unsupported characters (such as garbled characters), they will be automatically converted to underscores, so after importing, you may find that there is an extra underscore in network labels, device names, footprint names, attributes, etc. Please modify it manually. When the current version of altium is saved as an ASCII file, the Chinese will become garbled, so it is also garbled when imported. You need to open the ASCII file with a text editor such as Notepad and then import it after correction.
The imported altium file supports a maximum size of 100MB. Larger files will lealtium to longer import time or import failure. It is recommended to manually reduce the file size. For example, delete the copper filling first (set the copper filling to no filling type) and then import.
1.Chinese garbled characters appear when importing altium schematic
In versions below altium17, the encoding of the ASCII file saved as may be GBK2312, and the encoding of the ASCII file needs to be converted from GBK2312 to UTF-8. You can save as a UTF-8 encoded file using a text editor.
- Save as ASCII file with altium17, which defaults to UTF-8 encoding
- Or open the ASCII file with the system’s Notepad, and select UTF-8 encoding when saving as. Other text editors also have corresponding encoding conversion functions.
If after the text encoding is converted to UTF-8, there are still garbled characters when viewing the content with a text editor, then the import will also be garbled characters, please correct it in the text editor before importing.
2.After importing the altium file, there are wires and device pins that are not aligned with the grid, or the pins are biased
First set the unit of the schematic diagram in Altium Designer to imperial mil, in: view menu - switch unit
Then the canvas right-click menu or system settings: Options - Grid - set the display grid, electrical grid, altiumsorption grid to 100mil, switch grid to 100mil
Select all schematics CTRL + A , use Edit menu: Edit - Align - Snap to Grid function. Check for broken or wrong places to correct.
Save as ASCII and import
3.The footprint size will change after importing.
This is because the imported PCB has a footprint with the same name, but the footprint size is different. When importing, the bottom log will prompt that the footprint has the same name, and only one of them will be imported as a template.
Solution: It is recommended to manually modify the footprint names with the same name and different sizes in altium to ensure that the footprint names are not repeated.
Batch import Altum files
Please refer to the method below.
Download the AltiumScript script. AltiumScripts.zip
After decompression, open the alitumScripts.PrjScr project in Altium Design, if the version of AD is too low, it may not be able to run, please verify it yourself.
On the top menu - File or DXP - Run Script (File/DXP - Run Script) to open the script dialog box
Select the name of the script to be run, and click Run.
convertDesignToAscii.js: Convert the selected schematic and PCB files to ASCII format
convertLibToAscii.js: Convert the selected schematic library and PCB library files to ASCII format
- After running the script, the script will automatically create a schematic or PCB file, and put the libraries in the currently installed library file into the document one by one. During the period, there may be multiple pop-up windows, and you need to manually click Confirm to continue.
After completion, you will find the automatically generated ASCII file in the custom output directory.
Compress the generated schematic diagram and PCB file together into a zip package and import it into EasyEDA, and choose to extract the library or import the file.