Axis Y operations on lathe

Minimal version to use to get this feature v5.0.237

In this post :

Radial axis Y operation

Here an example , starting from an empty project file .

1) Add Lathe Axis Y Setup.

From Menu click on LATHE button and then on "New Setup"

Select [ Lathe CY Axis ] machine type.

Define the Y axis workplane

From menu, click on workplane button, click "Add New" 

You can set "Axis Y orientation" as workplane description. 

You can choose a description of your choice.

In the case of empty project file , the fastest way to define the Y axis orienation is select "Cylinder-Angle" mode .

Set 60 as diameter and 90° as angle. See image below.

Draw a slot

If not already selected , from workplane grid, activate the just created workplane , 

To activate a workplane, click on the checkbox in the "Active" column.

Now from menu click on CAD TOOLS > Other Shapes > Slot

Define a slot shape like this. Press OK when done.

Add a pocket operation

From Menu > MILL > Pocket > Select existing geometry

Click on the slot to link the geometry to the machining.

Turn OFF the geometry selection by pressing right mouse button or uncheck the "Selection ON/OFF " checkbox.

Define Tool Orientation

Enable the "DEFINE TOOL ORIENTATION" feature.

Select "From existing workplane" and select the newly created "Axis Y Orientation" workplane.


  • Tool orientation feature is only available if you have selected a compatible machine kind in setup screen as lathe with y axis, mill 4th axis, mill 5 axis .
  • Only the Z direction of the tool orienation plane is important. It will be used to calculate the rotation angle . The X and Y direction will be ignored.

Select a compatible tool diameter

Select a compatible tool diameter . In this case an 8mm end-mill. 

You can already see the generated toolpath.

Update the workplane origin and orientation (OPTIONAL)

Since the slot geometry and the operation tool orientation are referenced to "Axis Y Orientation" workplane,

if you change the workplane origin and orientation , both the geometry and the operation are updated accordingly.

From workplane grid, select the "Axis Y Orientation" row and press "Edit Origin"

Change the origin and orientation values.

You can see the origin system is updated accordingly.

Press OK.

Both the geometry and machining operation are updated with new workplane origin.

Axial operation

With axial operation ( frontal direction ) is not needed to define the tool orientation.

Select the geometry and define machining property as usual.

Is possible choose to machine the operation with XC axis system (G112 / G113) or with XY axis system.

Edit this property from machining screen.

Repeat operation around the revolution axis

Often is necessary to repeat the same operations around the revolution axis.

Instead of defining new operations, is possible take advantage of the clone toolpath feature , more info on this page > CLONE TOOLPATH ARRAY


Select [Circular pattern] .

You can increment the repetition count and edit other properties .

Press OK when done.

From HOME screen ,  DRAG and DROP the operation you need to clone over the clone toolpath item.

Now if you edit the parameters of original operation, the changes are applied also to cloned operations.

G-Code notes

Since every machine has different system to activate / deactivate the Y axis plane system, send me a working example of gcode that run ok in your machine. I'll help to fixing post processor.

You can probably find some working example in your machine manual.

Workplane definition

With Lathe Y axis operations is necessary to define the correct workplane for each operation,

So with turning operations you will need the G18 ZX plane.

With radial milling operations , you will need the G19 YZ plane.

For frontal milling operations you will need the G17 XY plane.

You need to define the workplane in the [Operation Head Code] template, with the tag


It will write the operation workplane system , usually 

G17 for XY

G18 for ZX

G19 for YZ

Take a look here :


Define C Axis angle direction

You need to define the axis C direction angle at which the operation is perfomed.

This angle is calculated by the defined tool orientation axis direction.

The tags used to add this code in post processor are :



This tag should be used in the  [OPERATION HEAD CODE (WITH LIVE TOOL)] template.

Turn ON / OFF the C axis brake

When permorming Y axis operations , the C axis need to be blocked with brake.

You can add the brake command with these tags : 



The {BRAKE_ON_PLACEHOLDER} will print the code to activate the axis c brake.

It's available only when the lathe Y axis is used.

You can customize brake command through post properties [Enable spindle brake ] and [Disable spindle brake]

Should be used in the [OPERATION HEAD CODE (WITH LIVE TOOL)] template.

Meanwhile the {BRAKE_OFF_PLACEHOLDER} it's available in the disengagement templates.

Still need help? Contact Us Contact Us