Import Altium Designer

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.

It is recommended to use EasyEDA Pro format converter for format conversion.

WARNING

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.
EasyEDA Pro 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.

options:

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.

Border source:

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.

Precautions

The difference before and after format conversion is as follows:

Schematic/Component library:

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

PCB/Footprint Library:

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 EasyEDA Pro
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

Other considerations:

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.

Common Problem

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.

method:

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 Altium files

Please refer to the method below.

Download the AltiumScript script. export-altium-to-ascii_v1.1.0.zip
After decompression, open the export-altium-to-ascii.PrjScr project in Altium Design, if the version of Altium 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.

Differences Before and After Import

Support for Format Conversion Primitives

Schematic/Component Library

Supported Primitive Types:

AD Element	After Import	AD Element Style	Converted Primitive Style	Description
Bus	Bus			-
Bus Entry	Bus Entry			Suspended Bus Entry is not supported during import.
Device	Symbol			-
Power Port	Network Identifier			-
Wire	Wire			-
Net Tag	Net Tag			The network label connection point in AD is light gray, and it becomes a blue cross after conversion.
Port	Network Port			-
Off-Graph Connector	Network Identity			The professional version does not support off-graph connectors. After import, the network ID is converted to a circle or triangle.
Page Character/Drawing Entry	Module Symbol/Pin			The professional version does not support drawing entries. They are converted to pins after import.
Text String	Text			-
Text Box/Comment	Text			Text boxes and comments are not supported in EasyEDA Pro. They are converted to text after import.
Drawing Tool - Arc	Arc			-
Drawing Tool - Circle	Circle			-
Drawing Tool - Elliptical Arc	Polyline			The professional version does not support elliptical arcs. After import, they are converted into multi-segment polylines.
Drawing Tool - Line	Polyline			-
Drawing Tool - Rectangle	Rectangle			Professional rectangles do not support transparent operations yet.
Drawing Tool - Rounded Rectangle	Rectangle			-
Drawing Tool - Polygon	Polyline			-
Plotting Tool - Bezier Curve	Bezier Curve			Continuous multi-stage Bezier curves are converted into multi-segment Bezier curves after import.
Indication - Generic No ERC Label	No Connection Identifier			-
IEEE Symbol	Polyline, Arc, Circle			After conversion, it is presented as a composite element composed of multi-segment polylines, arcs, and circles.
Manual Contact	Node			A suspended manual contact cannot be imported. A manual contact placed on a wire is converted to a node.
Theme Styles	Theme Styles	-	-	By default, the import dialog box uses the default theme of EasyEDA Pro. Rounded rectangles are converted to right angles, fill colors are not retained, and pixel colors are not retained to switch the schematic theme. If the original file theme is used, the color will follow the original file style, and the color will not change when switching themes.

Unsupported Primitive Types:

AD Graphic Element	Graphic Element Description	Description
Harness	Includes signal harness, harness connector, harness entry, predefined harness connector.	Schematic design does not support wire harness elements.
Indicators	Including the universal No ERC label, differential pairs, parameter settings, covering regions, compilation masks, probes (present in earlier versions).	The current schematic design supports only the conversion of the universal No ERC label connected to the device pin. The remaining indicators do not support conversion at this time.
Image	Image.	Altium Designer stores images in a local file path that does not contain images.
Hidden Pins	Hidden pins in the device.	EasyEDA Pro does not support hidden pins, which will be displayed after import.
Device Page Characters	-	EasyEDA Pro does not support device page characters.

Primitive Differences:

Text String Conversion Differences:

The strikethrough effect is lost after conversion.EasyEDA Pro text-related symbols do not support strikethrough effects, so all text-related symbol strikethrough effects will be lost.
The underline display effect is slightly different. The underline of text primitives in the EDA Professional edition is thicker than that in Altium Designer and will not cover the character content.
The locking information effect is lost. Since the symbol elements of the EasyEDA Pro do not support locking, all locking effects of elements with locking will be lost.
Font differences: If the operating system does not have the corresponding font installed, the text will be imported using the default font, and the text position may shift.
If the AD file is saved as ASCII, Chinese characters may become garbled. After the AD file is imported, the garbled characters are automatically converted to underscores (-).

Bus Conversion Differences:

The line width of the bus is significantly reduced after conversion. This issue will be addressed in a future version.

Altium Designer Bus with Different Line Widths

Bus Entry Conversion Differences:

The style of bus entry primitives is different after conversion.
The color of bus entry is different after conversion. Altium Designer allows the color of bus entry elements to be revised, but this operation is not supported by the EDA Professional Edition at present. The color of bus entry is green after conversion.

Device Component Conversion Differences:

The device is composed of multiple symbolic primitives, and any difference in symbolic primitives may cause conversion differences in the device.
There are differences in pin color. The pin color is the default color after import.
Pin electrical type import is not supported and will be lost after conversion.
When the custom attribute in the Altium Designer element is the same as the system attribute, the system attribute will be overwritten by the custom attribute after conversion.
The connection point style is different after conversion.

Different Pin Colors and Types in Altium Designer

Different Pin Colors and Types After Format Conversion

"Original package 1, original package 2, etc." will be generated after the component package is imported. The professional version is not associated with the package name but according to the package UUID. Therefore, the original associated multiple package names will be added as ordinary attributes when importing.
Component bit numbers: The professional version does not support the AD multi-component bit number method. Multi-component bit numbers such as U1A, U1B will be converted to U1.1, U1.2 after import.

Power Port Conversion Differences:

The EDA Professional network name only supports uppercase English letters and some common characters. If the network name contains Chinese, lowercase English letters, Greek letters, or other special characters, lowercase English letters will be converted to uppercase, and Chinese and special characters will be converted to underscores "_".
There is a difference in the style of the Power port between GOST Power Ground and GOST Earth, which will be addressed in future versions.
There is an offset in the position of the Power port names for GOST Power Ground and GOST Earth, which will be fixed in a future release.

Port Conversion Differences:

The name and value information of Port properties are lost after conversion. The EasyEDA Pro network port does not currently support property information.
The EasyEDA Pro network port does not support revising font, border width, border color, and fill color. Such information will differ after conversion.
The I/O attribute of the Port is lost after conversion.
If the Port in Altium Designer is connected to an unnamed wire or bus, the Port name is assigned to the wire or bus after conversion.
If both ends of the Port in Altium Designer are connected to a wire, both ends remain connected to a wire after conversion. If both ends are connected to a network ID, only one end with a pin can be connected after conversion.

Altium Designer Port connected to both ends

Format converted Port connected to both ends

Page Character Conversion Differences:

After the page character is imported, it will be presented as a module symbol. The EasyEDA Pro does not support revising the border of the module symbol, whether to fill, fill color, and lock operations. Therefore, there will be differences in the fill, border, and lock status after conversion.

Converted Page Character (Module Symbol)

Line Conversion Differences:

There is a difference in line style after conversion.
The Start Line Shape and End Line Shape in Altium Designer are not supported in the EDA Professional Edition, so they will be converted to multiple polylines.

Different Line Styles in Altium Designer

Converted Line Style

Different Start Line Shape and End Line Shape in Altium Designer

PCB/Package Library:

Supported Primitive Types:

AD Element	After Import	Description
Device	Component	-
3D Component Body	Contour Object	The professional version does not support importing 3D components. It is converted to a line or fill region depending on the layer it is on.
Fill	Fill Region	-
Solid Region	Fill Region	-
Arc	Line - Two Points Arc	-
Circle	Line - Circle	-
Line	Wire	-
String	Text	For now, only the first line of text will be imported; this will be supported in future versions.
Pad	Pad	-
Via	Via	-
Trace	Lead	-
Rectangle	Line	-
Graph	Contour Object	The kind set as polygon cut will be converted to a prohibited copper region.
Keepout	Board Frame	The default value is the board frame.
Copper	Copper Region	-
Polygon Copper Hollowing	No Region - No Copper Region	-
Drilling Table	Text, Lines	Converted to text and line composite primitives. The layer is converted to the drill layer.
Cascade Structure Table	Text, Line	Converted to composite primitives of text and lines.
Size	Size	The size styles are different. Some dimension layers are converted to document layers.
Teardrop	Teardrop	-

Some Layers/Features:

AD Layer/Function	After Import	Description
Board Shape	To the Document Layer by Default	EasyEDA Pro does not have a board shape but has a border layer. Most users use the Keepout and Mechanical Layer 1 as the board frame. Therefore, the board shape is converted to the mechanical layer.
Internal Electrical Layer	Block Network May Change After Import	The implementation of the internal electrical layer differs between AD and the professional version. When there are multiple internal electrical blocks, the block network may not be entirely consistent and needs to be carefully checked. After importing, the inner electrical layer will reconstruct the block, and the division of the inner electrical layer block may also differ.
KeepOut Layer	Default Plate Frame Layer	In the import window, you can set the source of the plate frame to be the Keepout layer or Mechanical Layer 1. Closed Keepout lines inside some boards are automatically converted to the corresponding prohibited region according to the action object. Open Keepout elements are imported into the mechanical layer. The Pro version does not support independent lines as prohibited regions.
Mechanical Layer	Mechanical Layer 1 to the Mechanical Layer, Other Mechanical Layers to the User-Defined Layer	The professional version uses the user-defined layer to implement the functionality of the other mechanical layers of AD.
Flying Lines	Flying Lines Appear After Import	Some places may be disconnected due to the reconstruction of copper after import, such as the absence of network elements, thermal welding not being generated due to DRC spacing, etc.
Element Solder Mask Extension	Only Through-Hole of Pad Supports Import	Other wire, arc, and other elements' solder mask extensions are not supported for import. In the case of independent primitives, an extended primitive will be generated in the solder mask or aid layer (solder paste layer).
Define Board Cutout	To the Border Layer or to the Grooving Region	This function corresponds to the grooving region of the professional version.

Unsupported Primitive Types:

AD Element	Description
Design View	The working view is not supported in EasyEDA Pro.
Work Wizard	This primitive is not supported in EasyEDA Pro.
Objects from a File	Such objects that call outside the file, are not contained in the file, and are not imported.
3D Volume	The Pro edition does not support 3D volume primitives.
Mosaic Array	Implementation logic is different; import is not supported.
Coordinates	EasyEDA Pro does not support coordinate primitives.
Room	Room primitives are not supported in EasyEDA Pro.

Primitive Differences:

Device Conversion Differences:

The device is composed of multiple package elements, and any package element difference may cause the conversion difference of the device.
If there are multiple packages with the same name but different sizes, the import will default to using one of them as a template to associate with other components.
There may be differences in the encapsulation layer after conversion:
- A. The layer property of the component in the professional version only supports the top or bottom layer. The layer property of the component is changed to the top layer after the conversion of other layer devices, but the pixel in the device is still in the corresponding layer.
Different layers of devices in Altium Designer
- B. If the encapsulated attribute drawn in AD is at the top level, but the whole is at the bottom level (belonging to the error data), the layer attribute will be automatically corrected to the bottom level after import.
- For example, the internal element of the device is transformed at the bottom level, but the package properties are transformed at the top level.
Altium Designer device properties at the top
Text/Text Box Conversion Differences:
If the font is not installed in the operating system or the font is not added in the Pro font settings, the default font (Arial and Song) will be used after the text import, and the text position may be offset.
Due to different font display logic, the same text font may not be exactly the same as the source file, and there may be differences in position and size.
The default font of Altium Designer is converted to the Default 2 font. Chinese characters that are not supported by the default font of Altium Designer will be displayed normally after conversion, and the font will be changed to typeface.
Text set in the solder paste layer in Altium Designer will become a mechanical layer after import.
The text box is converted to normal text, and only the first line of the text box is kept.
Altium Designer text box for multi-line text
Keep only the first line
Strokes and barcodes are converted to normal text. Pad Conversion Differences:
Rectangular drilling is not supported. Instead, slot drilling is used.
Altium Designer Rectangular Bore
The format is converted to an oblong circle
The electrical type attribute value will be lost after conversion.
The Professional pad does not support any layer. Unsupported layers will be converted to the corresponding fill region.
Altium Designer Inner Signal1 Pad
Format Converted to Fill Region

Hole Conversion Differences:

The EDA Professional edition does not support setting different outer diameters in different layers. After conversion, the top layer data is used as the outer diameter of the hole.

Altium Designer Holes with Different Outer Diameters

Paving Copper Conversion Differences:

The contour fill style of copper paving is not supported for import and is converted to a prohibited region.

Altium Designer Contour Fill Style Copper Placement

Non-copper layers and multi-layer copper are not supported for import and are converted to fill regions or other formats.

Altium Designer Silk Screen Coating Copper

There may be differences in re-copper placement after import due to different copper placement logic.
Since the Pro edition does not fully support the AD ply fill style, there may be differences in the ply fill style attributes after import.

Size Conversion Differences:

Radial, reference, lead, center, baseline, and diameter dimensions are not supported for import.
Dimensions of non-mechanical layers and screen layers will be converted to the document layer after import.
Dimensions and linear dimensions are converted to length dimensions after import.
There is a difference in the converted size style due to the difference between the Pro and Altium Designer size styles.

Design Rule Conversion Support:

Design Rules in AD		Import Corresponding Design Rules	Description
Electrical	Clearance	Spacing - Safe Spacing
Routing	Width	Physics - Wire	Extreme
	Routing Via Style	Physical - Vias Size
	Differential Pairs Routing	Physical - Difference Pair	Extreme
Mask	Solder Mask Expansion	Expansion - Solder Mask Expansion
Mask	Paste Mask Expansion	Extension - Weld Extension	Get SMD Pad Data
Plane	Power Plane Connect Style	Plane - Inner Electrical Layer
Plane	Polygon Connect Style	Flat - Copper Laying
Manufacturing	Board Outline Clearance	Spacing - Safe Spacing	Board Frame Safe Spacing

Note: "Take the extreme value" means that if there are multiple design rules applied to different layers in the imported design rule, the default design rule takes the smallest of the default values of the rules of each layer. The minimum line width/difference is the minimum value in the design rules of each layer. The maximum line width/difference is the maximum value in each layer's design rule.

Clearance

Safe Spacing (Simple) Conversion Table:

Altium Designer Element	Corresponding Professional Layout Element
Track	Wire
SMD Pad	Patch Pad, Single-Layer Test Point
TH Pad	Plug-In Pad, Multi-Layer Test Point
Via	Via
Copper	Fill Region/Teardrop, Line
Text	Text/Image
-	Drill a Hole

Safe Spacing (Advanced) Conversion Table:

Altium Designer Element	Corresponding Professional Layout Element
Arc	-
Track	Wire
SMD Pad	Patch Pad
TH Pad	Plug-In Pad
Via	Via
Fill	-
Poly	Line
Region	Fill Region/Teardrop
Text	Text/Image
-	Drill a Hole

Other Considerations:

Please do not repeatedly export your schematic or PCB to AD format and then import it again, as this operation may lead to loss of details.
When importing an Altium file, unsupported characters (such as garbled characters) are automatically converted to underscores. Therefore, underscores may be found in network labels, device names, package names, and attributes. These should be manually revised. When the current version of AD is saved as an ASCII file, Chinese characters may become garbled, so they will also be garbled when importing. You need to open the ASCII file with a text editor like Notepad and modify it before importing.
The maximum size of the imported AD file is 1GB. If the file size is larger, the import will take longer or may fail. It is recommended to reduce the file size manually. For example, delete the copper filling (set the copper filling type) before importing.

Import Altium Designer ​

Import Altium project file ​

Precautions ​

Common Problem ​

Batch import Altium files ​

Differences Before and After Import ​