|
The SIMPLE TURNING and SIMPLE BORING menus are very powerful and provide a quick way to create G code for shaft type machining with a strong variety of options for chamfering and radius edges. we will focus here on the SIMPLE TURNING menu but SIMPLE BORING functions the same way.
The menu form is divided into two main areas :
1)the geometry parameters that are used to describe the geometry of the workpiece
2)the machining or cutting parameters that describe the cutting conditions and parameters for machining.
Using the GEOMETRY PARAMETERS the user describes and provides coordinates for the three corners for every step of the part. In SIMPLE TURNING the geometry parameters start from the furthest point from the face and largest diameter and work toward the face of the part to the smallest diameter. In SIMPLE BORING, they work from the start from the furthest point from the face and smallest diameter and work toward the face of the part to the largest diameter.
Every "step" has three corners as illustrated in the image below. Corner 1 can have any corner radius and chamfer ... Corner 2 can have any radius ... and Corner 3 can have any chamfer or radius. As the user describes the part, each corner 3 becomes the next steps corner 1 ... allowing for an unlimited number of steps.
Using the drawing below ... geometry inputs would be as follows.
Diameter "A" = 4.500
Coordinate Z1 = -3.00
Diameter "B" = 2.500
Coordinate Z2 = -1.00
Corner 1 = Chamfer / Value = .250 / Angle = 45.0
Corner 2 = Radius / Value = .250
Corner 3 = Radius / Value = .250
ADD TO ELEMENTS
Diameter "A" = 2.500
Coordinate Z1 = -1.00
Diameter "B" = 1.000
Coordinate Z2 = 0
Corner 1 = Radius / Value = .250
Corner 2 = No R
Corner 3 = Chamfer / Value = .250 / Angle = 45
ADD TO ELEMENTS
This would define all the Geometry Elements
If an element requires editing ... select the element using the increment counter, then select EDIT ELEMENT.
If you wish to see the shape as defined, select the VIEW SHAPE which will load the G code program to finish the shape into the KipwareTP® plotter. Once loaded select the icon to plot a turning toolpath to see the finish toolpath per the shape as curretly defined.
The CUTTING PARAMETERS can now be entered in the appropriate fields in the Cutting Parameters areas of the form.
Once all inputs are complete, users have a couple more options to create the type of G code desired :
1)Users can select ROUGH and / or FINISHING to be performed per the shape. Rough / Finish Turning would result in depth of cut along the X axis and turning along the Z axis. Rough / Finish Facing would result in depth of cut along the Z axis and turning along the X axis.
2)The user can select to have the G code created as a canned cycle ( Fanuc or Okuma format depending on the SETTINGS ) or long hand G code. Long hand G code would be the preferred format for plotting in KipwareTP® and if your machine control does not support Fanuc or Okuma canned cycles.
|