Altium Designer 6.0提供了导入向导工具，可以很方便地导入以往Protel的设计文档和其他EDA设计工具的设计文档。包括原理图设计文件、PCB设计文件、原理图库文件和PCB设计文件。并可以把修改后的设计文件反存回需要的格式。
AD6.0 目前支持的设计文件格式如下：
原理图文件
Sch
- V4 (Protel 99 SE) - This format can also be opened in all Windows versions of the schematic editor.
PCB
- V4 (Protel 99 SE)
- V3 (Protel 98)
- V2.8 (PCB 2.8)
- Check that the PADS PCB file has been exported in ASCII format. The PADS Importer is only capable of translating ASCII file format.
- View the PADS ASCII PCB file in Notepad or similar and check the file version and units displayed in the file header. This is typically found on the first line in the ASCII file. Compare this to the versions the PADS Importer is capable of translating.
The translator imports the following PADS® PCB ASCII file formats:
- PowerPCB® V1, V1.1, V1.5, V2, V3.0, V3.5
- PADS® Perform
- PADS® 2000 V3, V4
- PADS® PCB V5
When you export the file from the PADS Software, ensure that you Select All sections to be exported instead of selecting particular primitives to export.
- Check that the exported file loads back into PADS Software correctly.
- Map the layers adequately. You will need to assign internal planes manually. Once the PCB file is translated, associate the internal planes in the layer stack manager with the approriate net. Split planes will need to be replaced and setup in Protel.
Altium Designer Knowledge Base
________________________________________
Query: How do I Import and Export Altium Designer Schematic and Schematic Library files to and from OrCad Capture?
Answer:
Exporting Schematic documents to Orcad Capture:
You cannot export a Schematic sheet as a single entity to Orcad Capture. You have to export the whole project from Altium Designer to Orcad Capture. You can do this by following the steps below:
1. Within the Projects Panel, right click on the project and select the Save Project As... command.
 |
2. Within the Save As dialog, set the Save as type field to Export Orcad Capture Design (*.DSN) and click the Save button.
 |
Importing Orcad Capture Schematic files:
1. Go to File » Open and then select OrCad Capture Design (*.DSN) from the dropdown box and click on Open.
 |
Importing Orcad Capture libraries:
Altium Designer can Import Orcad Schematic (*.OLB) and PCB (*.LLB) libraries:
- Go to File » Open.
- In the Choose Document to Open dialog under Files of type, select either OrCad Capture Library (*.OLB) or OrCad Max Library file (*.LLB) respectively to open an OrCad Schematic or PCB library in Altium Designer.
Query: How can I export a PCB board to HyperLynx (*.HYP) format?
Answer: PCB documents can be saved in HyperLynx format using the File » Save As command and then selecting the Export HyperLynx (*.HYP) option in the Save as type drop down list of the Save As dialog.
Note:The Stackup information is not exported properly for multilayer boards so this section will need to be updated manually in a text editor.
- Open the exported *.HYP file in a text editor and locate the STACKUP section at the beginning of the file
- In the PCB editor, select the Design » Layer Stackup Manager command
- Looking at the Layer Stack Up in the Layer Stack Up Manager, edit the STACKUP in the *.HYP file from top to bottom using the syntax below
For Top/Bottom Layers and MidLayers:
(SIGNAL T=0.0014 P=0.0000 C=1.724e - 8 L=Top_Layer M=COPPER)
T = copper thickness of the layer in Inch
C = resistivity of the conductor of the layer in Ohm x m
L = name of the Layer
M = material of the layer - COPPER for signal layers
For isolation substrate
(DIELECTRIC T=0.0200 C=4.8000 L=DE_Internal_Plane_1 M=FR4)
T = dielectric thickness of the layer in Inch
C = dielectric constant
L = name of the Layer
M = material of the dielectric
For Internal Planes
(PLANE T=0.0014 C=1.724e - 8 L=Internal_Plane_1 M=COPPER)
T = copper thickness of the layer in Inch
C = resistivity of the conductor of the layer in Ohm x m
L = name of the Layer
M = material of the layer - COPPER for internal planes
Query: How do I import P-CAD libraries into Altium Designer?
Details: To bring in ASCII formatted libraries from P-CAD 2002 to Altium Designer, make sure that, in P-CAD 2002 in the Library Executive, lib files translate to the .lia file format using the Library » Translate command.
To open a P-CAD Schematic library in Altium Designer, go to File » Open then set the Files of Type to PCAD V16,V17 ASCII Schematic library . Now browse to find the .lia file generated from P-CAD and click on Open. This should open the schematic library in Altium Designer.
To import the PCB library into Altium Designer, go to File » New » PCB Library then Save the library by going to File » Save As.... After saving the library , go to File » Import » PCAD V16 ASCII library . From the PCAD ASCII Lib File dialog box, make sure you choose the .lia file which is the same .lia file from which you extracted the component symbols for the schematic library and click on open. This should populate the PCB Library with the footprints in the library.
