How to Create a 3D Picture CNC Machine Relief

• 1
  Key takeaways
• 2
  Prepare the image before you touch a 3D picture CNC machine
• 3
  Choosing material and relief depth
• 4
  Set up the CAM toolpath in six numbers
• 5
  Pick the cutter and hold it short
• 6
  Checks that catch problems before the finishing pass
• 7
  Step by step from photo to finished relief
• 8
  Which relief approach fits the job

The machine never reads a photograph. It reads coordinates. Between the two sits a height map, usually a grayscale image where each pixel value becomes a Z value. That single conversion decides how much of the original picture survives into metal or plastic. So the first hour of work goes into the file, not the machine.

Start in Photoshop, GIMP or Affinity Photo and convert the image to 8-bit grayscale. Apply a levels adjustment rather than a brightness slider, because levels let you set the black point and white point independently. Push the white point until the brightest highlight clips slightly. That gives the tool a clear top plane to face off later.

Blur matters more than sharpening. A 1 to 2 pixel Gaussian blur removes sensor noise that would otherwise turn into thousands of tiny Z moves. Sharp edges are a problem in relief work: they force the CAM software to generate near-vertical walls, which no ball nose cutter can produce cleanly. Soft transitions cut faster and look better.

Remove the background or mask it to a flat value. A busy background eats toolpath and often reads as random texture. Crop to the subject, then decide the outline. If the finished part needs a defined border, add a raised frame in CAD after machining rather than trying to machine the photo edge itself.

• 1
  8-bit grayscale16-bit adds nothing on a 3-axis height map and slows CAM calculation.
• 2
  Levels, not brightnessSet black and white points separately to control the depth range.
• 3
  1–2 pixel blurKills noise that becomes Z-axis chatter.
• 4
  Flat backgroundMask it out; background detail is wasted cycle time.

Depth range depends on the material and on how the part will be used. A shallow relief of 1 to 3 mm reads well under raking light on a plaque or a decorative panel. A deeper 5 to 10 mm relief starts to look sculptural and needs a thicker blank so the base does not flex during cutting.

Aluminium 6061 and 7075 hold fine detail well. They cut cleanly with a ball nose cutter at 8,000 to 12,000 rpm and a feed of 800 to 1,500 mm/min for a Ø3 mm tool. Brass C36000 is the friendliest relief material: chips break short, finish comes out bright, and a 0.1 mm stepover leaves almost no visible tool marks.

Harder materials change the numbers, not the method. Stainless 304 wants lower surface speed, so expect 2,000 to 4,000 rpm with a carbide ball nose and generous coolant. Titanium and Inconel are possible but rarely worth it for a decorative relief; the cycle time climbs fast and the tool wear is real.

Plastics behave differently again. PMMA and POM cut with a sharp, polished cutter and give a clean matte surface. PEEK is expensive for relief work and its chips are abrasive. For a first article, machine the job in POM to validate the toolpath, then move to the final material once the depth range is confirmed.

• 1
  1–3 mmPlaques, panels, shallow decorative faces.
• 2
  5–10 mmSculptural relief; needs a thicker blank.
• 3
  6061 and C36000Easiest materials for fine detail.
• 4
  POM firstCheap way to prove the toolpath before cutting metal.

Import the grayscale image into CAM software that supports relief machining. The common options are Vectric Aspire or VCarve, Autodesk Fusion with an image-to-relief add-in, ArtCAM successors, and DeskProto. All of them work the same way: the image becomes a mesh, and the mesh becomes a toolpath.

Six numbers control almost everything. First, model height: the Z range in millimeters, typically 2 to 6 mm. Second, base height: a flat floor below the relief, usually 0.5 to 2 mm, which gives the cutter somewhere to start. Third, tool diameter. Fourth, stepover, as a percentage of tool diameter. Fifth, stepdown, the vertical bite per pass. Sixth, machining strategy: raster, offset or hybrid.

Raster passes run back and forth along one axis and finish fastest on flat-ish relief. Offset passes follow the contour and leave fewer directional marks on a face or a curved form. Hybrid runs a raster roughing pass and an offset finishing pass, which is the safest default when the image has both broad areas and fine lines.

Set the machining boundary slightly larger than the model. A 2 to 3 mm margin prevents the cutter from leaving a ridge where it lifts at the edge of the image. For a recessed relief, cut the pocket wall in a separate 2D operation so the boundary stays crisp instead of following the height map.

• 1
  Model height 2–6 mmTotal Z travel from the floor to the highest pixel.
• 2
  Base height 0.5–2 mmFlat floor under the relief; keeps the cutter engaged.
• 3
  Raster strategyFastest on broad, shallow relief.
• 4
  Offset strategyCleaner on faces and curved subjects.

A ball nose cutter is the standard tool for relief. Its radius blends adjacent passes, so scallop height stays low even at a moderate stepover. A flat end mill leaves a stepped surface and only works for the roughing pass or for flat-bottomed pockets around the picture.

For a 100 mm wide relief, a Ø6 mm ball nose for roughing and a Ø3 mm ball nose for finishing covers most jobs. Detail smaller than about 1.5 mm needs a Ø1 mm or Ø0.5 mm cutter, and that changes the whole setup: lower feed, higher rpm, and a much smaller stepdown.

Hold the tool as short as the geometry allows. Relief cutting runs the cutter over a contoured surface for hours, and every extra millimeter of gauge length amplifies deflection. On a long, thin tool, deflection shows up as a shadow line along one edge of the relief.

Check runout before the finishing pass. A ball nose with 0.01 mm of runout cuts a visibly wider path on one side. On a finishing pass with a 0.1 mm stepover, that is a stripe. Measure with a dial indicator on the flute, not on the shank.

• 1
  Ø6 mm rough, Ø3 mm finishStandard pair for a 100 mm wide relief.
• 2
  Ø1 mm and belowDetail under 1.5 mm; reduce feed and stepdown.
• 3
  Short gauge lengthDeflection shows as shadow lines in the finish.
• 4
  Check runout0.01 mm runout is visible at 0.1 mm stepover.

Inspect after roughing, not after finishing. The roughing pass reveals chatter, workholding movement and unexpected hard spots in the material. Fixing those after a three-hour finishing pass is expensive. Stop, check the surface, and only then change the tool.

Measure the relief depth at three points: the highest intended point, the flat floor, and one mid-tone area. The floor should sit within 0.05 mm of the programmed value across the part. If it drifts, the blank moved or the Z zero was set on a dirty surface.

Look at the surface under a raking light, not straight on. A phone flashlight held at about 20 degrees to the surface shows scallops, missed areas and tool marks that are invisible under normal light. This is the fastest visual inspection for relief work and it needs no equipment.

For parts that will be inspected formally, we run 100 percent inspection before shipment with reports on request. Relief depth, floor flatness and surface finish are the three measurements that matter. Tolerance on machined features is held to ±0.005 mm where the drawing calls for it, though a decorative relief face is usually judged on appearance rather than a number.

• 1
  Stop after roughingChatter and movement are cheap to fix at this stage.
• 2
  Measure three depthsHigh point, floor, mid-tone.
• 3
  Raking lightA flashlight at 20 degrees reveals scallops.
• 4
  Reports on requestDepth, flatness and finish are the key measurements.