Why a bad file ruins good material
A CNC router does exactly what the file tells it to do. If the file contains a mistake, the machine will reproduce it quickly and precisely, across an entire sheet of 18 mm plywood. Below are the seven mistakes we see most often in the lab. Every one of them can be caught at the computer, before you ever switch the machine on.
1. Open contours and duplicate lines
A CAM program needs a closed contour to figure out which side of the part is the inside and which is the outside. If two lines miss each other by even a hundredth of a millimeter, the contour is open: the pocket toolpath either won't be generated or will come out wrong. A duplicate line means the bit will cut the same spot twice.
In VCarve, after importing the file, run Join Vectors and the tool for deleting duplicate vectors. Then select the parts one at a time and confirm that each one is closed.
2. Inside corners and bit diameter
A round bit can't cut a sharp inside corner. It always leaves a rounded corner with a radius equal to half the bit diameter: 3 mm for a 6 mm bit. If that corner belongs to a joint slot, the mating part won't fit.
The fix is a dog-bone cutout: a small circular relief in the corner that "opens up" the corner for the bit. VCarve's fillet tool has a mode for this. Also make sure that even the narrowest gap in the design is wider than the bit diameter.
3. The wrong side: inside, outside or on the line
A profile toolpath gives you three options. If you cut an outer contour "on the line," the part will shrink by half the bit diameter on each side. With a 6 mm bit, a 300 mm shelf comes out at 294 mm.
The rule is simple: cut outer contours on the outside, and holes and slots on the inside. Save "on the line" for decorative grooves.
4. Material thickness "on paper"
18 mm plywood is rarely exactly 18 mm. It usually varies from 17.4 to 18.3 mm, even within a single sheet. If you set the cut depth to the nominal thickness, some parts won't cut all the way through in places.
Measure the thickness with calipers at several points across the sheet. Set the cut depth 0.2–0.5 mm deeper than the thickness, and always put a spoilboard underneath: a sheet of MDF that takes the damage from the bit instead of the machine table.
5. An unsecured sheet and parts without tabs
On the final pass, a small part breaks free from the sheet, and the bit catches it and throws it. In the best case, the part gets damaged. In the worst case, the bit snaps, and the flying piece can hit someone standing nearby.
- Add 3–4 tabs to every small part. A tab is a strip a few millimeters thick that holds the part to the sheet. After cutting, you trim the tabs by hand and file them smooth.
- Secure the sheet around its entire perimeter. Drive screws only into the waste area, well away from the toolpath.
- Mark the screw locations on a separate layer in the file, so you know exactly where they go when you're at the machine.
6. The zero point
The zero point in the file is at the bottom-left corner of the sheet, but on the machine you set it at the center. Or Z zero in the file is measured from the table, but on the machine it's set from the material surface. Either way, the result is the same: the bit either cuts air or plunges into the table.
In the project settings, set X/Y zero and the Z zero reference exactly the way you set them on the machine. It's best if the whole team follows one convention, for example the bottom-left corner and the material surface.
7. "Default" feeds and speeds
The values stored in the tool database may not suit your machine or your material. Here's how to read the signs: burned MDF edges and dust instead of chips mean the feed rate is too slow. Vibration, noise and a broken bit mean the load is too high.
Starting formula: feed rate = spindle speed × number of flutes × chip load per flute. For example, 18,000 RPM × 2 flutes × 0.1 mm = 3,600 mm/min. Start with a depth per pass of half the bit diameter, and increase it only after a test cut.
Check the toolpaths in the simulation first. VCarve's 3D preview shows you how the part will come out. An open contour, a forgotten tab or the wrong cutting side is right there on the screen. A 2-minute simulation saves you a sheet of plywood and a bit.
Quick check before you save the G-code
- All contours are closed, with no duplicate lines.
- Inside corners have dog-bones, and all gaps are wider than the bit.
- Outer contours are cut on the outside, holes on the inside.
- The thickness has been measured, and the cut depth is 0.2–0.5 mm deeper.
- Small parts have tabs, and the screw locations are marked.
- The zero point is the same in the file and on the machine.
- Feeds and speeds have already been tested on this material.
Course at TDSCNC Machining: 3D Design, CAM & Operation8 weeks · 48 h · Starts 11 NovDetailsIn the CNC Machining: 3D Design, CAM & Operation course, students practice every one of these rules on real projects: a sign, a 3D panel and a furniture part, on a 1300×2500 mm bed. Preparing vector files is the same skill for the laser, which is why many students take the laser cutting course first.
