This is the most used machining operation in turned part.
You need to select existing geometries or defining new one . Take a look here for more info
One useful geometry pattern, available only in turning operations , is the [STEP PROFILE]
In turning operation , when the profile is similar to a staircase, you can use this geometry pattern.
In this way you have to insert only diameter value, length and the initial chamfer / fillet .
See below an example image.
To define the initial chamfer / fillet you can use , for example:
- 5x30 , to define a chamfer width of 5mm , tapered at 30°
- -5 , a negative value to define a fillet with radius of 5 mm
- 5 , a positive value, to define a chamfer width of 5mm.
Sometime you need to use inversed direction to correctly cut the profile.
In this case change [Turning Direction] in Reversed
Probably you need to set a additional secure distance to your tools, in order to approach the stock without collision.
To define this additional secure distance :
1) Open tool parameter screen , click on ROUGHING for example
2) Open tool dialog screen , click on tool description
3) Define ADDITIONAL SECURE DISTANCE field
You can find a really good explanation of G71 cycle here
By default is used the "two lines" G71 macro.
To insert macro , check the Roughing Macro field . Is possible to add also the G70 finishing cycle, select Finish with same tool
Here there is the Lathe axial turning template.
And here there is Finishing Lathe Axial Turning template.
You can edit both from post processor dialog. Write macro in search box to filter the post processor properties.
Here an example of g-code output :
G71 U2.5 R0.5 G71 P10 Q15 U1. W1. N10 G1 X80.989 Z0. G1 X55. Z-32.162 N15 G1 Z-61. G70 P10 Q15
When you have macro enabled you can't see the allowance material in path preview , since it's managed directly by G71 macro.