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 Create PCB from Schematic in Altium Designer (Step-by-Step)
The moment you finish drawing your schematic and run a clean ERC, there’s a certain satisfaction knowing your circuit is electrically complete. But the real work begins when you need to create PCB from schematic in Altium Designer and turn that circuit into a physical board. This transition trips up many engineers, especially those coming from other EDA tools where the process works differently.
I’ve transferred thousands of schematics to PCB layouts over my career, and Altium Designer handles this better than any other tool I’ve used. The synchronization is direct, there’s no intermediate netlist file to manage, and changes flow both ways when you need them to. This guide walks through the complete process from prepared schematic to components placed on your PCB, ready for routing.
Before you can create PCB from schematic in Altium Designer, your schematic must be properly prepared. Skipping these prerequisites leads to failed transfers, missing components, and frustrating error messages.
Schematic Checklist Before Transfer
Requirement
How to Verify
Why It Matters
All components have footprints
Tools > Footprint Manager
Components without footprints won’t transfer
Unique designators assigned
Tools > Annotate Schematics
Duplicate designators cause transfer conflicts
No ERC errors
Project > Compile PCB Project
Errors indicate electrical problems
All pins connected or marked no-connect
Visual inspection + ERC
Floating pins create DRC warnings
Net names assigned to important signals
Check net labels
Named nets are easier to work with in layout
Project saved
File > Save All
Unsaved changes won’t transfer
Running the Electrical Rule Check (ERC)
Compile your project before attempting the schematic to PCB transfer. Navigate to Project > Compile PCB Project or use shortcut C, C from the schematic editor.
The Messages panel displays any violations. Pay attention to:
Errors (Red): Must be fixed before proceeding. Common errors include unconnected pins, duplicate designators, and missing footprint assignments.
Warnings (Orange): Should be reviewed. Some warnings are acceptable (like intentional floating inputs on unused op-amp sections), but most indicate real issues.
Hints (Blue): Informational only, but worth reviewing for best practices.
Don’t proceed to PCB creation with outstanding errors. Fix them in the schematic first.
Verifying Footprint Assignments
Every schematic component needs an associated PCB footprint. Check assignments using Tools > Footprint Manager from the schematic editor.
The Footprint Manager displays all components and their assigned footprints. Look for:
Components with no footprint assigned (blank footprint column)
Components with incorrect footprints (wrong package size)
Footprints that don’t exist in your libraries
To assign or change a footprint, select the component, click Add or Edit, and browse to the correct footprint in your libraries.
Step 1: Create the PCB Document
With your schematic prepared, create the blank PCB document that will receive the design data.
From the Projects panel:
Right-click your project name
Select Add New to Project > PCB
A blank PCB document opens
Save the PCB immediately:
Right-click the new PCB entry in the Projects panel
Select Save As
Name the file (typically matching your project name)
Click Save
The PCB document must be saved before the transfer will work. Altium Designer needs to know where to write the imported data.
Step 2: Configure the PCB Document
Before importing schematic data, configure basic PCB settings. This prevents issues later when components arrive with nowhere appropriate to go.
Setting Up the Board Shape
Your PCB needs a defined outline. For a simple rectangular board:
In the PCB editor, select View > Fit Board to see the default board shape
For complex outlines, draw the shape on a mechanical layer first, select the objects, then use Design > Board Shape > Define from Selected Objects.
Configuring the Layer Stackup
Access the Layer Stack Manager through Design > Layer Stack Manager. Configure your layer count based on design requirements:
Design Type
Recommended Layers
Notes
Simple through-hole
2 layers
Top and bottom copper
Standard SMT
2-4 layers
Add internal planes for power/ground
Mixed analog/digital
4 layers
Separate analog and digital grounds
High-speed digital
4-6 layers
Controlled impedance routing
Complex systems
6+ layers
Multiple power domains, dense routing
For a basic two-layer board, the default stackup works fine. For multi-layer boards, add signal and plane layers as needed.
Setting the Snap Grid
Configure an appropriate snap grid for component placement:
With no objects selected, the Properties panel shows document properties
In the Grid Manager section, select Global Board Snap Grid
Click the pencil icon to edit
Set Step X and Step Y to appropriate values (1mm or 0.5mm for metric, 50mil or 25mil for imperial)
Using a consistent grid makes component alignment much easier.
Step 3: Transfer Schematic Data to PCB
Now comes the core process to create PCB from schematic in Altium Designer. This uses the Engineering Change Order (ECO) system to synchronize data between documents.
Initiating the Transfer
From the schematic editor, select Design > Update PCB Document [YourPCBName].
Alternatively, from the PCB editor, select Design > Import Changes From [YourProjectName].
Both commands accomplish the same thing: comparing the schematic data to the PCB data and generating a list of changes needed to synchronize them.
Understanding the Engineering Change Order Dialog
The Engineering Change Order (ECO) dialog opens, showing all proposed changes grouped by type:
Change Type
What It Does
Add Component
Places component footprint on PCB
Add Net
Creates net connection in PCB
Add Net Class
Creates net class definitions
Add Room
Creates component room definitions
Add Parameter
Transfers component parameters
For a new PCB, you’ll see Add operations for every component and net in your schematic.
Validating Changes
Before executing, validate the proposed changes:
Click Validate Changes button
Watch the Check column in the Status region
Green checkmarks indicate valid changes
Red X marks indicate problems
Common validation failures include:
Footprint not found: The specified footprint doesn’t exist in available libraries. Add the library containing this footprint or create the footprint.
Pad doesn’t match pin: The footprint pad names don’t match the schematic symbol pin names. Edit the footprint or symbol to make them consistent.
Duplicate component: A component with this designator already exists. Usually indicates annotation problems in the schematic.
Executing Changes
Once all changes show green checkmarks:
Click Execute Changes button
Watch the Done column for execution results
Green checkmarks indicate successful execution
Close the dialog when complete
Your components now exist in the PCB document.
Step 4: Locate and Organize Imported Components
After executing the ECO, your components appear in the PCB editor, typically clustered together outside the board outline. They need to be moved onto the board and arranged logically.
Finding Your Components
Components usually appear near the origin point (0,0) or in a cluster to one side of the board. To locate them:
Press V, F (View > Fit All) to zoom out and see everything
Look for the cluster of footprints connected by ratsnest lines
The ratsnest (white connection lines) shows required electrical connections
Initial Component Arrangement
Before detailed placement, do a rough arrangement:
Select all components by drawing a selection box around them
Drag the group onto the board area
Release to drop them on the board
The components are now on the board but need proper placement.
Step 5: Understanding the Ratsnest
The ratsnest displays unrouted connections as straight lines between pads that need to be connected. This visual guide is essential for component placement.
Ratsnest Display Options
Shortcut
Action
N
Toggle ratsnest display on/off
N, S
Show all connections
N, H
Hide all connections
Ctrl + Click component
Show connections for selected component only
Using Ratsnest for Placement
As you move components, the ratsnest dynamically updates. Use this to guide placement:
Short, uncrossed ratsnest lines indicate good placement
Long, crossing lines suggest components should be repositioned
Clustered connections help identify which components belong together
Step 6: Place Components on the PCB
Component placement significantly impacts routing difficulty and signal integrity. Take time to place components thoughtfully.
Placement Priority Order
Priority
Component Type
Placement Consideration
1
Mounting holes
Fixed mechanical positions
2
Connectors
Board edges, cable routing
3
Critical ICs
Central location, thermal considerations
4
Crystals/oscillators
Close to their ICs
5
Decoupling capacitors
Adjacent to IC power pins
6
Remaining passives
Fill available space logically
Placement Shortcuts
Shortcut
Action
Spacebar
Rotate 90°
X
Flip horizontally
Y
Flip vertically
L
Move to opposite layer
J, C
Jump to component by designator
M
Move selected component
Tab (while placing)
Open properties to change designator
Placement Best Practices
Group functional blocks: Keep related components together. A voltage regulator and its capacitors should be adjacent, not scattered across the board.
Minimize trace lengths: Position components to reduce the ratsnest line lengths, especially for sensitive signals.
Consider thermal management: Power components need space for heat dissipation. Don’t crowd them with temperature-sensitive parts.
Plan for routing channels: Leave space between component groups for traces to pass through.
Orient components consistently: Polarized components (diodes, electrolytic capacitors) and ICs with a pin 1 indicator should follow a consistent orientation for easier assembly.
Step 7: Set Up Design Rules
Before routing, configure design rules that match your fabrication house capabilities and design requirements.
Access the PCB Rules and Constraints Editor through Design > Rules.
Essential Design Rules
Rule Category
Rule Type
Typical Value
Electrical
Clearance
0.2mm (8mil)
Routing
Width
0.25mm preferred, 0.15mm minimum
Routing
Via Style
0.8mm diameter, 0.4mm hole
Manufacturing
Minimum Solder Mask Sliver
0.1mm
Manufacturing
Hole Size
0.3mm minimum
These values work for standard PCB fabrication. Check with your specific manufacturer for their capabilities, as some support finer features.
Step 8: Keep Schematic and PCB Synchronized
During layout, you’ll often need to make changes. Altium Designer supports bidirectional synchronization between schematic and PCB.
Can I create PCB from schematic in Altium Designer without creating a new PCB file first?
No, you need a PCB document in your project before transferring schematic data. The ECO process compares the schematic to an existing PCB document and generates changes to synchronize them. If no PCB exists, create one using Add New to Project > PCB, save it, then run the Update PCB Document command. The PCB doesn’t need any configuration before the transfer, as components will simply appear at the origin point.
Why do some components show red X marks when I validate changes in the ECO dialog?
Red X marks indicate validation failures, meaning those changes cannot be executed. The most common causes are missing footprints (the specified footprint isn’t in any installed library), pad-to-pin mismatches (footprint pad names don’t correspond to symbol pin names), and existing components with the same designator already in the PCB. Check the specific error message in the ECO dialog, fix the underlying issue in your schematic or libraries, then re-run the transfer.
How do I transfer only specific components from schematic to PCB?
The Update PCB Document command transfers all differences between schematic and PCB. However, in the Engineering Change Order dialog, you can uncheck specific changes before executing. Disable the components you don’t want to transfer by unchecking their Enable checkbox, then execute. Only enabled changes will be applied. This is useful when you want to add components incrementally or exclude test points from initial transfer.
What happens to my PCB layout if I make schematic changes after initial transfer?
Running Update PCB Document again generates a new ECO containing only the differences. Existing components and routing remain untouched unless specifically affected by your schematic changes. If you add a component to the schematic, only that component transfers. If you delete a component, the ECO will propose removing it from the PCB (you can disable this if needed). Net changes update the ratsnest accordingly. Your existing placement and routing stays intact for unchanged portions of the design.
Can I transfer the same schematic to multiple PCB documents?
Yes, but each PCB must be a separate project or you need to manage them carefully. The simplest approach is creating separate projects for each PCB variant, with the schematic files copied or linked. Alternatively, use Altium’s design variants feature if the PCBs share most components but differ in specific configurations. Each PCB document maintains its own synchronization state with the project’s schematic, so changes affect all PCBs in the project unless you use variants.
Moving Forward After Schematic to PCB Transfer
Successfully importing your schematic data into the PCB is just the beginning of the layout process. With components placed and the ratsnest visible, you’re ready to proceed with routing, polygon pours, and design rule checking.
Take the time to verify everything transferred correctly before investing effort in routing. Use the component filter (J, C to jump to component) to spot-check that designators match, footprints are correct, and all expected components exist. A few minutes of verification prevents hours of rework later.
The direct synchronization between schematic and PCB in Altium Designer means you can iterate freely. Found a problem during layout that requires a schematic change? Make the change, run the update command, and your PCB reflects the modification immediately. This bidirectional flow keeps your documents consistent throughout the design process.
This guide reflects Altium Designer functionality as of early 2026. Menu locations and dialog appearances may vary slightly between versions, but the fundamental ECO-based synchronization process remains consistent across Altium Designer releases.
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.
