Adjusting CAM Tolerance and Machine Modes to Fix Faceting Issues

Based on the list of fixes you shared, the troubleshooting so far indicates traditional chatter is not the culprit. If it was, all trials above should have changed the severity of the problem in some way. You also indicate the problem only exists on corners, and not the straight walls of the part. In addition, the problem also shows through the final finish, which means its inherent to the geometry, and not necessarily the surface finish. Therefore, I believe the issue you are facing is known as faceting.

Faceting means creating geometry through several flat surfaces. This could be on purpose, like the cut on a gemstone. In CNC machining, it generally means flat surfaces appearing where you would prefer it to be a smooth, more rounded surface. Faceting is a milling problem associated with more complex part geometry like 2D splines that can’t be programmed as a simple radius.

When it comes to part quality, faceting creates a lot of problems for us. In your case the problem is more cosmetic and customer facing after surface treatment, but faceting can also create issues with fitment of two parts, or sealing areas.

There are two ways to address this issue, and they can be independent or linked: the CAM tolerance and the machine mode. The CAM tolerance is how tightly the software is expected to generate code based on the CAD geometry. The machine mode is a setting on your machine’s controller that tells it how to prioritize its execution of that code. This typically means prioritizing speed, accuracy or a balance of the two. An issue is sometimes fixed on the CAM side, or other times on the machine side, but often it requires tuning both for full optimization and process reliability.

The CAM tolerance is one of those things you may not know about or appreciate until it manifests in an issue like this. For simple surfaces and shapes with clearly defined radii, the CAM system knows to offset for your chosen tool, apply the appropriate code as needed and cut the shape. For more complex shapes like 2D splines, or organic geometry like mold components and medical parts, this same approach will not work. The CAM system must recreate this surface in a series of points that a machine can execute. The CAM tolerance comes into play with how precisely these points must follow the CAD geometry by defining a boundary that all points must fall within. Depending on the complexity of the surface and the tolerance required, this could result in dozens or even thousands of points just to make a simple looking 2D curve.

When I’ve encountered faceting issues, it usually because the default CAM system tolerance is too loose, resulting in code that is more linear and segmented, rather than wrapping closely around the intended geometry. By significantly decreasing this tolerance, the faceting disappears as each line segment becomes invisible to the eye. In my CAM system, the default tolerance is 0.001", but I often run 0.00025" or less as needed on critical finishing passes.

It should be noted that decreasing this tolerance significantly increases program size, as it requires more points to hold a tighter line. Therefore, your machine memory may not be enough, and you’ll need to run from a DNC.

Machine modes typically are set by a G or M code in the program, and they tell the machine what to prioritize as they execute code. For the most part, the available options are some type of sliding scale from speed to accuracy, with options in between for more granular tuning. The speed setting will prioritize maintaining programmed feed rate, but may take some liberties with the code along the way. This means potential for overshoot (gouging), or rounding off what should be sharp edges. This is recommended for roughing only with appropriate stock left for finishing. The accuracy setting will prioritize the code and hit each point perfectly, even if it means significantly slowing the programmed feed rate to do so.

My recommended corrective actions are first to improve the CAM tolerance to see the effect on the issue, then try different machine settings for further tuning. The machine mode can go a long way in fixing an issue like this on its own, but I’d caution the reader to understand it cannot fix bad code. The machine is limited in that it doesn’t know what you’re trying to cut, it only knows to execute the code it’s given, so make sure the CAM tolerance is set properly and feeding the machine with the toolpath it needs. From here, the machine can optimize things a little further.

For the most pristine finish requirements, it is recommended to run a very tight CAM tolerance and run the machine in its highest accuracy setting. If the resulting cycle time is not acceptable, you can then adjust the machine setting while checking that your parts still have a suitable finish to find the upper limit you can accept. This knowledge will inform your future projects.

This concept of CAM tolerance and machine modes can also be used to optimize program size, and even improve cycle time in roughing operations. While you and your customer will certainly be happy with the process improvements, I encourage you to dig in on the issue with your suppliers to learn more, and make sure software and hardware are working together for the best quality and efficiency.