Injection Mold Project


Design, build and test functional injection mold – This lab counts as three lab grades.

NOTE 1: Keep it simple.  Small details (except engraving) will not work well.  They require very small tools and lots of time (we have neither).image2

NOTE 2: Keep it shallow (.125 thick or so).  Thick parts do not mold well.

NOTE 3: Properly DOCUMENT all operations.  Include a print of the tool path for each operation. Must show where origin is.

NOTE 4: Post operations as separate programs.  HEADERS Must include an indication of the nature of the operation as well as the tool required (SIZE, FLUTES, MIN STICKOUT).

NOTE 5: You must locate the sprue as shown in the examples.  Use the ball end mill to cut the sprue.  It must be about .090 deep, but can include a gate.


Blank Dimensions

  • Blank is 1.00 x 2.00 x [4.00 max long]
  • 6061 T6 aluminum

Tools available (ONLY USE THESE)

Click for larger view:


Face Milling

  • Use 2.0 face mill (floor/wall)
  • Use Face Milling operation
    • You could also use Face Planar Profile (to follow a curve or edge)

Cavity Milling

  • Use Cavity Milling operation to cut out main shapes
  • Pay attention to the cut levels


Note: You can insert text using “Insert -> Curve -> Text.”  I like to use planar text.  You can import geometry from AutoCAD if you like.

  • Use a 90 degree engraving tool
  • Use Planar Profile operation
  • The part Boundary Geometry mode should be the curve
    • When selecting text, it is a good idea to select letter curve loops one at a time, use “Create Next Boundary” (on Create Boundary dialog box) to add each additional letter curve.
  • Set tool position to “on”
  • Select the curve
  • The Floor is the level where the path will be.
  • You now need to adjust the non cutting moves to plunge engage /retract instead of leading in/out with arcs.
    • Under path settings
    • Non Cutting Moves
    • Engage: Closed area
      • Engage type “plunge”
    • Engage: Open Area
      • Same as closed area
    • Retract: Retract
      • Same as Engage
  • Be sure engraving tool does not cut away edges of mold.


  • Use standard workpiece as geometry (blank with workpiece inside)
  • Use 90 deg brazed carbide router bit
  • Use Planar Profile operation
  • Specify part boundaries
    • Type is Curve/Edges
    • Open type
    • Plane automatic
    • Material side is left
    • Tool position is tanto
    • Part Stock is negative amount (on path settings panel, cutting parameters dialog box).


  • Use Drilling operation
  • Be careful to retract above all check geometry
  • Setting peck cycle depth
    • Click on cycle type (even if it is already peck drill…)
    • Ignore “distance, ” click ok
    • Number of Steps is “1” click ok
    • Now click “increment-none”
    • Click “constant” enter increment (.50)


  • Use a Drilling or Reaming operation, be sure not to peck.

About Rest Milling (Using IPW)

If you need to do several operations in a row that sequentially develop geometry (like roughing, then finishing), you may need to restrict your cutting to the IPW (in process workpiece).

Here is how to do this:

  • On the  Edit Operation dialog box, go to Path Settings
  • Click Cutting Parameters then the Containment tab
  • Chang the In Process Workpiece to “Use Level Based

Note: Possible to extract IPW geometry.  Do this in toolpath verify.


Be able to demonstrate each of the following at the machine:

  1. Tool number
  2. Tool offset (H)
  3. Origin (e.g., G54)
  4. Orientation of CSYS (XM, YM, ZM)
  5. How will tool approach/depart
  6. Spindle speed
  7. Feedrate
  8. Tool minimum stick-out