Inquire: Call 0086-755-23203480, or reach out via the form below/your sales contact to discuss our design, manufacturing, and assembly capabilities.
Quote: Email your PCB files to Sales@pcbsync.com (Preferred for large files) or submit online. We will contact you promptly. Please ensure your email is correct.
Notes: For PCB fabrication, we require PCB design file in Gerber RS-274X format (most preferred), *.PCB/DDB (Protel, inform your program version) format or *.BRD (Eagle) format. For PCB assembly, we require PCB design file in above mentioned format, drilling file and BOM. Click to download BOM template To avoid file missing, please include all files into one folder and compress it into .zip or .rar format.
How to Convert OrCAD Files to Altium Designer: A Complete PCB Engineer’s Guide
If you’ve spent years building designs in OrCAD and now need to migrate to Altium Designer, you’re probably wondering how painful this process will be. I’ve been through this exact situation multiple times across different companies, and I can tell you that converting OrCAD files to Altium Designer is more straightforward than most engineers expect—but there are definitely some gotchas you need to know about.
This guide covers everything from preparing your OrCAD files for conversion to troubleshooting common issues that pop up during the import process. Whether you’re migrating a single reference design or moving your entire design library, you’ll find actionable steps that actually work.
Before diving into the technical details, let’s address the elephant in the room: why switch at all? Having worked with both platforms extensively, I’ve seen several scenarios that drive this migration.
Company standardization is probably the most common reason. When organizations merge or acquire other teams, consolidating on a single EDA platform makes collaboration much easier. Nobody wants to maintain licenses for multiple tools when one will do.
Feature requirements also push engineers toward Altium. The unified design environment, where schematic capture and PCB layout live in the same application with real-time synchronization, appeals to teams tired of juggling separate tools. The routing engine in Altium handles high-speed designs and HDI boards with less manual intervention than older OrCAD Layout.
Reference design adoption creates migration needs too. Semiconductor vendors often publish reference designs in specific formats. If you receive an OrCAD design but your shop runs Altium, conversion becomes necessary.
Understanding OrCAD File Types You’ll Need to Convert
Before starting any conversion, gather all the files associated with your design. OrCAD uses several file formats, and missing even one can result in an incomplete import.
OrCAD File Type
Extension
Contains
Altium Equivalent
Capture Design
.DSN
Schematic pages, design cache
.SchDoc (one per page)
Schematic Library
.OLB
Symbol definitions
.SchLib
Layout PCB
.MAX
Board layout, routing
.PcbDoc
PCB Library
.LLB
Footprint definitions
.PcbLib
PCB Editor (Allegro)
.BRD
Board layout (Allegro format)
.PcbDoc
Allegro ASCII
.ALG
ASCII export of Allegro PCB
.PcbDoc
Drawing
.DRA
Footprint drawings (Allegro)
.PcbLib
Important distinction: OrCAD Layout (.MAX files) and OrCAD PCB Editor (.BRD files) are different products. OrCAD PCB Editor is actually based on Cadence Allegro technology, so those files use the Allegro importer in Altium, not the OrCAD importer.
Preparing Your OrCAD Files for Conversion
Proper preparation prevents most conversion headaches. Spend a few minutes on these steps before launching the Import Wizard.
Step 1: Back Up Everything
Create a complete copy of your OrCAD project folder before any conversion attempt. The import process doesn’t modify your original files, but having a clean backup gives peace of mind and a rollback option.
Step 2: Check OrCAD Version Compatibility
Altium Designer’s Import Wizard supports OrCAD files up to version 17.2. If you’re running a newer OrCAD version, you may need to save files in a compatible format first.
The file format for .DSN files changed significantly in OrCAD Capture 10.x. Files created in version 10.x or later may show “Unrecognized Project File Version” errors when importing into older Altium Designer releases. For best results, use Altium Designer Summer 09 or later for these files.
Step 3: Verify Design Integrity
Open your design in OrCAD and run a design rules check. Fix any errors before conversion—problems that exist in OrCAD will carry over to Altium, and they’re easier to fix in the original tool.
Step 4: Locate All Library Files
The Import Wizard handles library conversion automatically, but only if it can find the libraries. Note the locations of your .OLB and .LLB files. If your design uses company-standard libraries stored on a network drive, ensure you have access during the conversion process.
Step-by-Step OrCAD to Altium Designer Conversion Process
With files prepared, the actual conversion follows a wizard-driven process. Here’s how to navigate it effectively.
Enabling the OrCAD Importer
The OrCAD importer may not be enabled by default in your Altium Designer installation. To check and enable it:
Go to DXP → Extensions and Updates
Click Configure under the Installed tab
Scroll to the Importers\Exporters section
Check the OrCAD option if not already enabled
Click Apply and restart Altium Designer
Launching the Import Wizard
You have two options for starting the import:
Method 1: Import Wizard Navigate to File → Import Wizard. This gives you the most control over the conversion process.
Method 2: Direct Open Simply open an OrCAD file (.dsn, .max, .olb, or .llb) using File → Open. Altium automatically launches the Import Wizard with that file pre-selected.
Walking Through the Import Wizard Steps
Select File Type: Choose “Orcad Designs and Libraries Files” from the list of available importers.
Add Files: Click the Add button to select your OrCAD files. You can add multiple files of different types in one session. The wizard groups related files automatically.
Configure Layer Mapping: For PCB files, the wizard presents a layer mapping screen. This is critical—OrCAD and Altium use different layer naming conventions.
OrCAD Layer
Recommended Altium Mapping
Top
Top Layer
Bottom
Bottom Layer
SMT
Top Overlay / Bottom Overlay
SST
Top Overlay / Bottom Overlay
Assembly 1
Mechanical Layer 1
Assembly 2
Mechanical Layer 2
Inner layers
Mid Layer 1, 2, etc.
The wizard offers default mappings that work for most designs. You can save custom mappings to an .ini file for reuse across multiple projects.
Schematic Options: Configure how net connectivity translates. The option “Convert Orcad Off-Page connectors as Altium Ports” is particularly useful when converting flat designs that you intend to restructure as hierarchical in Altium.
Execute Import: Click Finish to begin the conversion. The wizard processes files and displays progress. For large designs, this may take several minutes.
Post-Conversion Cleanup and Verification
The Import Wizard does excellent work, but no automated conversion is perfect. Plan for these cleanup tasks.
Reviewing the Migration Log
After import completes, review the migration log carefully. It lists any elements that couldn’t convert or required modification. Common logged issues include unsupported font substitutions, missing library references, and layer mapping anomalies.
Verifying Schematic Connectivity
Open each imported schematic and run Project → Compile PCB Project. Check for:
Unconnected pins that should be connected
Net name discrepancies between sheets
Missing or incorrect component references
Power and ground connectivity
OrCAD uses globals for power/ground nets throughout designs, while Altium uses Power Ports. The importer handles this translation, but verification catches edge cases.
Checking PCB Design Integrity
For imported PCB files, perform these checks:
Enable all layers using View Configuration (press L)
Step through each layer in single-layer mode (Shift + S) looking for:
Missing copper features
Polygon pour anomalies
Silk screen placement issues
Missing or misaligned reference designators
Run Tools → Design Rule Check to catch clearance violations
Synchronizing Schematic and PCB
If you imported both schematic and PCB files, synchronize them:
Ensure both schematic project and PCB are open
Execute Design → Import Changes From [Project Name]
Review the Engineering Change Order (ECO) dialog
Ideally, no changes should be needed if both files originated from the same design
If the ECO shows unexpected changes, investigate before accepting. Mismatches often indicate component reference issues or net name problems that need manual correction.
Handling OrCAD PCB Editor (Allegro) Files
If your PCB was created in OrCAD PCB Editor (also called OrCAD PCB Designer Professional), you need the Allegro importer instead of the OrCAD importer.
Direct Import with Allegro License
If you have Allegro PCB Editor installed on your workstation, Altium can directly import .BRD files. The Import Wizard detects the Allegro installation and handles the conversion automatically.
ASCII Conversion Without Allegro License
Without an Allegro license on your Altium workstation, you can still import designs using ASCII extraction:
Locate Allegro2Altium.bat and AllegroExportViews.txt in your Altium installation’s System folder
Copy both files to the folder containing your .BRD file
Open a command prompt and navigate to that folder
Run: Allegro2Altium your_file.brd
Import the resulting .ALG file using the Import Wizard
This batch conversion must run on a machine with Allegro installed, but the resulting ASCII file can be imported on any Altium workstation.
Common Conversion Problems and Solutions
Even with careful preparation, issues arise. Here are the problems I encounter most often.
Missing Footprints After Import
Symptom: Schematics import correctly, but components show no footprint associations.
Cause: The .DSN file contains schematic data but footprint references point to external library files that weren’t included in the import.
Solution: Import .OLB and .LLB library files along with the design files. The wizard links them automatically.
Polygon Pours Not Displaying Correctly
Symptom: Copper pours appear incomplete or have unexpected voids.
Cause: Polygon pour settings don’t translate perfectly between tools. OrCAD and Altium use different algorithms for thermal relief and clearance calculations.
Solution: Select each polygon in Altium, access its properties, and Repour the polygon. Adjust clearance rules if necessary.
Component Values Not Visible in Layout
Symptom: PCB shows reference designators but not component values in silk screen.
Cause: OrCAD Layer mapping may have placed value text on an unexpected layer.
Solution: Enable all layers and search for the missing text. Move it to the appropriate overlay layer, or regenerate it from schematic parameters.
Version Incompatibility Errors
Symptom: “Unrecognized Project File Version” or similar errors during import.
Cause: OrCAD file version is newer than what your Altium version supports.
Solution: Update Altium Designer to the latest build. If that’s not possible, resave the OrCAD files in an older format (available via Save As in OrCAD Capture).
Large Selection Rectangles on Components
Symptom: Selecting a component in PCB view shows an enormous bounding box.
Cause: Footprints contain oversized primitives on certain layers, often from layer mapping issues.
Solution: Export footprints to a PCB library (Design → Make PCB Library), then edit each footprint to remove or correct the oversized elements.
Read more How to convert PCB Files in different Design software:
Migrating isn’t just about current designs—you likely have years of OrCAD libraries you want to continue using. The Import Wizard handles library conversion, but consider these optimization steps.
Batch Library Conversion
Import all your .OLB and .LLB files in a single wizard session. Altium creates corresponding .SchLib and .PcbLib files, automatically grouped into a project.
Library Validation
After conversion, open each library and verify:
Pin assignments on schematic symbols
Footprint pad sizes and shapes
3D model associations (these rarely survive conversion)
Parameter data attached to components
Integrating with Altium’s Component System
Consider migrating converted libraries into Altium’s integrated library system or database-linked libraries. This enables:
Real-time supply chain data
Automatic footprint and 3D model linking
Centralized component management across projects
Useful Resources for OrCAD to Altium Migration
These resources provide additional help when standard conversion steps don’t solve your problem.
AltiumLive Community Forums: Active community where engineers discuss migration issues and share solutions
Altium Knowledge Base: Searchable database of technical articles covering specific import scenarios
Component Resources
Altium Component Portal: Access manufacturer-verified components with schematic symbols and PCB footprints already in Altium format
SnapEDA: Third-party component library with Altium-compatible downloads
Ultra Librarian: Component search engine with multiple export formats
FAQs About Converting OrCAD Files to Altium Designer
How long does the OrCAD to Altium conversion process take?
The actual Import Wizard processing typically completes in a few minutes for small to medium projects. However, plan for additional time reviewing and cleaning up the imported design. Simple designs may need only 30 minutes of post-import work, while complex multi-sheet schematics with dense PCB layouts could require several hours of verification and adjustment.
Can I convert my OrCAD libraries to use in future Altium projects?
Yes, the Import Wizard converts .OLB schematic libraries to .SchLib format and .LLB PCB libraries to .PcbLib format. Once converted, these libraries work exactly like native Altium libraries. You can reference them in any future project, add them to integrated library systems, or use them as templates for creating new components.
Will my original OrCAD files be modified during conversion?
No, the conversion process reads your OrCAD files but never writes back to them. Your original .DSN, .MAX, .OLB, and .LLB files remain unchanged. After conversion, you’ll have both the original OrCAD project and a new Altium project containing the translated design data.
What OrCAD versions does Altium Designer support for import?
Altium Designer’s Import Wizard supports OrCAD Capture and Layout files up to version 17.2. For OrCAD PCB Editor (Allegro-based) files, support extends to Allegro versions 15.2 through 16.x and later versions depending on your Altium Designer release. Always check Altium’s documentation for the latest compatibility information if you’re working with very new OrCAD releases.
How do I handle designs with both OrCAD schematics and Allegro PCB files?
This mixed scenario is common when teams use OrCAD Capture for schematic entry but OrCAD PCB Editor (Allegro) for layout. Import them as separate operations: first import the .DSN schematic file, then import the .BRD Allegro file using its respective importer. After both imports complete, copy the PCB file into the schematic project folder and add it to the project through the Projects panel. Finally, run Design → Import Changes to verify synchronization between schematic and layout.
Final Thoughts on OrCAD to Altium Migration
Converting OrCAD files to Altium Designer isn’t the nightmare it might seem at first glance. The Import Wizard handles most of the heavy lifting, and with proper preparation, you can have a working design in Altium within an afternoon.
The key is treating migration as a two-step process: automated conversion followed by manual verification. Don’t assume the wizard caught everything—spend time checking connectivity, reviewing layer mappings, and validating footprints. This upfront investment prevents costly errors when your converted design goes to manufacturing.
If you’re migrating an entire design library rather than a single project, consider this an opportunity to clean house. Not every legacy OrCAD component needs to move to Altium. Evaluate each library against current needs and retire obsolete parts rather than converting them.
The effort pays off. Once your designs are in Altium, you gain access to unified design tools, better collaboration features, and a modern component management system. Engineers who’ve made the switch typically report faster design cycles and fewer data integrity issues—benefits that compound over every project that follows.
Inquire: Call 0086-755-23203480, or reach out via the form below/your sales contact to discuss our design, manufacturing, and assembly capabilities.
Quote: Email your PCB files to Sales@pcbsync.com (Preferred for large files) or submit online. We will contact you promptly. Please ensure your email is correct.
Notes: For PCB fabrication, we require PCB design file in Gerber RS-274X format (most preferred), *.PCB/DDB (Protel, inform your program version) format or *.BRD (Eagle) format. For PCB assembly, we require PCB design file in above mentioned format, drilling file and BOM. Click to download BOM template To avoid file missing, please include all files into one folder and compress it into .zip or .rar format.
