Gerber Compare in Altium 365's Online Platform

The moment you push your Gerbers to a manufacturer for a DFM inspection, it can be a nerve-wracking experience waiting for a response. Once I push a totally new design to manufacturing, I spend a few sleepless nights waiting for a pro forma quote to come through and the design to pass qualification. It’s not until I get working boards that I breathe a sigh of relief. But before you receive your working boards, there will likely be some back-and-forth communication before your board hits the fabrication line.

When manufacturers and designers need to resolve problems in Gerber files before fabrication, it helps to have a Gerber compare utility. The newest version of Altium Designer now offers this feature through the Altium 365 platform, giving everyone visibility into changes to Gerbers before fabrication. This helps designers get to market faster, increases throughput for fabricators, and keeps everyone informed during the fabrication process.

What PCB Manufacturers Look For in Your Gerber Files

The extent to which a PCB manufacturer will review and modify your Gerber files depends on the level of service you need for your design. In full turnkey services, you’ll likely get a complete inspection, sourcing services, complete manufacturability and assembly review, in-circuit testing, and 

During a design review, your fabricator may look through your project files and your Gerber files to spot any problems that compromise board quality or yield:

• Standards conformance: Your design might need IPC Class 2, Class 3, 6012, or other inspection level. Fabricators will start looking for reliability defects in your Gerbers to ensure you’re compliant with your standards level and to ensure fabrication quality. 
• Footprint mismatches: If your PCB is being reviewed by an assembler, any PCB land pattern/footprint mismatches or other problems with footprints that impact assembly can be noticed in Gerber files. Note that the component package information must be contained in the BOM for a full comparison. 
• Drill hits: Overlapping drill hits, drill hits into pads, or mis-sized drill hits can be spotted in Gerber files and a drill table. 
• Clearances and feature sizes: Clearances between pads (smallest component pitch), between traces, and smallest feature sizes in general will determine some fabrication costs and potential for fabrication/assembly defects. 

In some cases, the Gerbers are simply outdated and need to be regenerated. In other cases, they may need to be manually modified and submitted back to the customer for review. Whenever files need to be regenerated or modified, the fabricator needs to get approval from the customer on the finalized files before starting a production run.

No matter who regenerates Gerber files and other manufacturing documents, it helps for the designer and fabricator to be able to compare each version of a file side-by-side to ensure all outstanding issues have been addressed. I’ve had fabricators send me Word documents with current and modified files for comparison, which I then had to comment on and send back. It’s easy for text to be misinterpreted, images could be unclear, or you may simply be unable to find the changes in files due to poor annotation. Altium Designer and Altium 365 solve this problem with integrated Gerber viewer and Gerber compare features.

Save Time With an Online Gerber Compare Tool

Gerber file comparison identifies differences between two versions of PCB fabrication artwork. Users can compare corresponding layers to inspect changes in traces, pads, copper pours, solder mask openings, and silkscreen. This comparison helps designers detect unintended modifications and outdated outputs before sending files to a PCB manufacturer. It also supports approval of artwork modified by a fabricator during manufacturing preparation.

To take advantage of this feature, you need to work with Project Releases within Altium Designer. The goal of a Project Release is to prepare a complete package for fabrication and assembly that includes all relevant fabrication files, including Gerber files.

Once two Project Releases are present in your managed content server, and both releases include a complete set of Gerber files, you can access the Gerber compare feature. Similarly, when Project Releases are sent to a manufacturer, the manufacturer can open each release and compare the Gerber files from these releases.

Three Ways to Compare Gerber File Outputs

Gerber Compare in Altium 365 Web Instance

Altium 365 allows users to compare Gerber files from successive project releases in their web browser without opening these files in Altium Designer. This is a simple way to access and compare Gerber files from multiple project releases from anywhere in a secure web platform. Comparisons can be run for any pair of Gerber layers in the project release files. After looking at this type of comparison, a designer or manufacturer can call out specific portions of the design in comments to ensure the designer will make changes before fabrication.

The image below shows one example of a Gerber comparison in Altium 365. The specific features that were modified between releases are highlighted in red. General areas in each layer are also marked for easy identification and inspection. This is a simple way for manufacturers and their customers to get a design through review and qualify any required changes before fabrication.

With a bit of layer manipulation, you can focus on the specific portions of the files that are different, both from the above comparison map and by flashing between the two compared layers. As another example, the image below shows a Gerber compare where some tracks were removed (shown in green) while some tracks and polygons were added (shown in red). This alternative view is a quick way to run a Gerber compare directly in fabrication files without downloading project releases. 

Since all files in a Project Release are stored on Altium 365, files from old revisions can still be accessed and downloaded directly. A manufacturer can also instantly open the new project release in Altium Designer and identify variations between two design documents using the Differences panel. Comments can also be left in the most current version to ensure they are seen and addressed by the design time. Once changes are made, a new Project Release can be pushed back to the manufacturer for a final review before production.

Standalone Gerber Compare Tool

Similar to the Altium Viewer, there is also a standalone Gerber Compare tool that allows users to compare file sets in a side-by-side or combined view inside a web browser. Altium’s standalone Gerber Compare tool provides a free browser-based comparison without software installation or registration. It supports RS-274X and Gerber X2 data generated by Altium Designer and other PCB design tools. Users can upload the approved files to the older Gerbers box and the revised files to the newer Gerbers box to generate visual comparisons in a side-by-side or overlay format.

Personally, I prefer side-by-side comparison in many instances because it can be easier to see changes in trace routing, such as in the example shown below. The combined tool can be useful for things like footprint changes, via/hole location changes, and some modifications to solid copper regions (polygons or fills).

• Access the standalone Gerber Compare tool for free

The standalone viewer is free to access and use, and it provides the ability to take 2D measurements of features in each layer. For a more granular analysis capabilities, users should perform a side-by-side comparison inside Altium Designer.

Gerber File Comparison in Altium Designer

Altium Designer already includes built-in file comparison features, and users can even compare Gerber files stored on their local machines or in Altium 356 (or both). Users can compare file sets stored locally, or a local Gerber file set against a project release in Altium 365; this would be performed by downloading releases from a project, importing both sets of Gerber files, and setting up a file compare in Altium Designer.

Users have long been used to doing a side-by-side comparison using the CAMtastic tool inside Altium Designer. CAMtastic also lets users compare corresponding layers and generate a separate layer showing their differences. This provides a way to inspect changes between Gerber outputs from different PCB revisions.

1. Create a CAM document by selecting File → New → CAM Document.
2. Select File → Import → Gerber, choose the first Gerber file, and click OK. Repeat to import the corresponding file from the second set.
3. Hold Ctrl and select both layers in the CAMtastic panel.
4. Right-click the selected layers and choose Compare.
5. Select Create New and click OK to generate a comparison layer showing the differences.
6. Inspect the comparison layer, then repeat the process for each additional pair of corresponding layers.

Differences between the compared layers are mapped onto a new layer inside the CAMtastic interface as shown in the image below.

The generated comparison layers are used to identify changes in the fabrication data. When comparing a local file set against an Altium 365 release, the release’s Gerber files will need to be downloaded to a local machine, and then the Gerber files can be imported to the CAMtastic tool before following the same process.

Before running the comparison, it is a good idea to list the intended design changes in each layer pair so that comparisons can be generated directly. The export settings should also be the same for both revisions, including the coordinate origin, and unit settings. Once you have identified the corresponding layers are paired correctly, and that neither package is missing an expected output, you will get useful results from the CAMtastic Gerber compare method.

Today’s PCB manufacturers and PCB designers can work together to get through production quickly, reduce defects, and streamline sourcing thanks to the Altium 365™ platform. This unique cloud-based platform integrates with the world-class design tools in Altium Designer®, making all your project data accessible to your manufacturer and collaborators in a secure environment. Designers and manufacturers can share PCB fabrication data, project files, and much more in a cloud-based platform.

We have only scratched the surface of what is possible to do with Altium Designer on Altium 365. You can check the product page for a more in-depth feature description or one of the On-Demand Webinars.

Frequently Asked Questions

What is Gerber file comparison, and why should I run it before sending files to a PCB manufacturer?

Gerber file comparison highlights differences between two versions of PCB fabrication artwork. Users can identify changes to copper, solder mask, silkscreen, and other exported layers before approving manufacturing. Comparing the final package against an approved baseline helps catch unintended edits, outdated outputs, and modifications introduced during fabrication preparation.

How do I verify that a Gerber revision matches the intended design changes and nothing else changed?

Users can compare the complete revised Gerber set against an approved baseline and match every detected difference to a documented design change. The review covers both modified layers and layers expected to remain unchanged, while also confirming that every intended change appears. Consistent export settings and correct layer pairing support accurate comparison. NC drill files and fabrication notes require review alongside the Gerber artwork.

Are there free online tools to compare two Gerber sets side by side before manufacturing?

Yes. Altium’s standalone Gerber Compare tool provides free browser-based comparison without software installation or registration. Users can upload RS-274X or Gerber X2 datasets from Altium Designer or other PCB design tools, then inspect the revisions side by side or examine overlaid differences in a combined view.

How do I generate a visual diff of two Gerber versions to confirm only the intended layers changed?

Users can upload the older and newer Gerber datasets to Altium’s online Gerber Compare tool, which automatically generates a visual diff. The Differences pane organizes changes by layer and provides numbered entries for inspecting individual locations. Users can check each difference against the intended modifications and review the remaining layers for unexpected changes.