CNC-Calc v6 can generate CNC toolpaths for face milling, with or without finishing passes and using different cutting strategies.
You can watch the related video for this part of the tutorial here:
Creation of Facing Toolpaths
First, in the Operations toolbar, select the programming format of the NC-program in the File Type drop-down menu. Select ISO Milling.
Then click on the icon Face Milling to generate a CNC-Toolpath for face milling.
Write the text FACING in the Comment field of the CNC-Calc pane Face Milling. This text will be included at the start of the final NC code for this operation. When multiple operations exist in the same NC program, the comments will help to locate and identify the start of each operation.
Click on the outlining contour of the drawing. This will select the bounding contour that the facing operation will operate on.
Click on the button Parameters in the CNC-Calc pane Face Milling. This will open the configuration dialog for setting the face milling parameters.
Enter the values into the dialogs as shown in the pictures below.
Depths Tab
Cutter Diameter: This is the diameter of the cutter. Here it is a 30 mm Face Mill.
Start Depth: This is the top of the part.
End Depth: The final depth (will be corrected by Stock to Leave).
Retract Height: When the operation is finished, this is the height that the tool will retract to.
Roughing Stepdown: The maximum roughing cuts that the operation will take.
Finish Stepdown: If Finish Cuts is larger than zero, this is the cut that will be taken in each finishing cut.
Finish Cuts: The number of finishing cuts that the operation will perform. If the value is left at zero, only roughing cuts will be made.
Stock to Leave: The amount of stock that is left at the end of the operation (after both roughing and finishing cuts).
Strategy Tab
Cutting Method: The method used to perform the face operation. It is possible to select Zigzag, Climb, or Conventional.
Move Between Cuts: Is only used for the Zigzag Cutting Method, since the other methods will move free between cuts.
Overlap Across: The amount that the mill will hang out over the side diagonal to the cutting direction.
Overlap Along: The distance that the tool will move out over the end before the high speed loops are taken.
Entry Distance: The distance that the tool will start out at before the actual cut is taken.
Exit Distance: The distance the tool moves out after the final cut is taken.
Facing Angle: The angle at which the operation is performed. An angle of zero is along the X-axis, and an angle of 90 is along the Y-axis.
Stepover: The distance between each of the parallel cuts of the facing operation.
After entering the values, close the parameters dialog with OK. To show the generated toolpath click on Show Toolpath button in the Face Milling pane.
Now click on the button Export Editor to export the generated NC code to a new window in the Editor. The following screen should now be displayed.
See next section to know how to insert a tool using the Feed and Speed Calculator.