* If your machining complex line work such as a logo then use the Engraving sequence

Common or Mill tab > 3 Axis Trajectory Milling  

* Don’t use the Custom Trajectory tool

 

 

 

Trajectory Milling will follow a defined path which is selected from edges or curves within your reference model. The shape of the tool, its position relative to the trajectory and z depth relative to the machine zero define the cavity formed.

Important – It is unlikely your cutter can take out all the material in one pass, make sure the total depth is removed in slices.  Ball nose cutters in particular will need more than one pass to give a good surface finish

 

Work through the options and tabs in the Trajectory Mill dashboard;

  1. Drop down the tool list in Tool window to select a tool from the Tool Library.  Edit Tools to create a new tool in the Tool Library.
  2. Parameters tab > set appropriate tool Parameters from the Machining Parameters page – be sure to set a Plunge feed
  3. To select trajectory – Tool Motions tab > Insert Here > Curve Cut

In the Curve Cut window;

  1. Trajectory Curve > select datum curve or edges as trajectory – use Shift for Chain of Edges selection
  2. Toggle the direction arrow at the end of the Trajectory to decide the position the tool will plunge – always plunge where there is no material if possible – extend the trajectory if needed
  3. Height > select surface or Datum plane to specify final depth of the sequence
  4. Options > Offset cut to offset the cut to the left or right of the trajectory by its diameter
  5. Start Height > select surface or Datum plane to specify start depth of the sequence
  6. Return to the Tool Motions tab

 

 

If setting a tart height surface does not have the desired effect then you may have to leave this selection blank and manually control the slices as above:

  1. Tool Motions tab > Parameters > All
  2. STEP_DEPTH > set slice increment
  3. NUMBER_CUTS > set how many cuts at previous increment
  4. this sets say, 6 cuts at 1mm from the depth set in the Height parameter upwards

Minimising tool travel – ZIG-ZAG parameter

By default the tool will only travel in one direction along a trajectory – see conventional or climb milling. To force the tool to travel in both directions and therefore stop it machining fresh air each time it returns to the start of the trajectory;

  1. Tool Motions tab > Parameters > All
  2. CUT_TYPE > ZIG_ZAG

To add subsequent trajectories to the current sequence;

  1. Tool Motions tab > Insert Here > Curve Cut
  2. Its important you highlight Insert Here before adding further trajectories
  3. Set up new trajectories as before

 

Play toolpath;