Contents - Index

Face Profiling


The majority of external turning is done along the surface of the billet with cutting being along the Z axis. The only cutting usually done across the end of the billet and along the X axis is facing-off. The tools for this external turning are all aligned parallel to the lathe's X axis. In the WELturn main menu, in Set the Tool Offsets, tools 1 to 6 are shown aligned with the X axis. Only the internal turning tools are shown aligned with the lathe's Z axis.

                              

There are times when it is necessary to turn a profile on the right-hand end face of a job, as shown above.

                             

The profile on the end face of the job is shown above: it is an arc. From a toolpath creation and coding point of view, this feature is a pocket.

The billet is initially rough turned in the usual way with a right-hand tool. This leaves the part with a flat end face, parallel to the X axis, and a flat surface, parallel to the Z axis.

                             

The pocket can be machined by a neutral tool. However, as shown above, the tool must be mounted on the lathe parallel to the Z axis. The tool can still be identified as Tool 3. However, if the job also requires the use of a neutral tool parallel to the X axis for surface turning, let that tool be Tool 3, as would normally be the case, and give the neutral tool which is parallel to the Z axis a different number. Use the number of any tool which is not being used (not 1, which is the right hand tool, and which is always used at the start of every job).

Please note that only the 5PC and 5CNC lathes with manual tool change permit the mounting of the standard tools parallel with the Z axis. For a 5CNC lathe with an auto toolchange turret, special tooling will need to be purchased: please consult tooling catalogues, eg Plansee Tizit and Sandvik.

A tool aligned with the Z axis must be appropriately defined in whatever CADCAM software is being used to generate NC code. (Note for AlphaCAM users on Defining the Tool in AlphaCAM: open and display the lathe tool drawings. Make one copy of, say, tool 3, the neutral tool. Rotate this copy of the tool so that its tip points to the left: the result should be as shown above. Define the tool in the usual way. Save the tool with a name such as "Neutral Tool 3 Z axis".)

Create code for the machining of the part.

Ensure that the toolchange position is far enough in the +Z direction from the end of the part to actually permit a change of tooling.

Before machining can be done, the offsets of the Z-axis neutral tool must be measured. Assign the offset measurements to whichever tool number has been used in the NC code. The fact that the tool does not match any of the tool pictures shown in WELturn does not matter.

                             

The picture above shows the tool tip as viewed through the Emco tool setting microscope. Users of the DM1 microscope will see the image turned through 180 degrees with the tool tip pointing to the left.

Prepare for machining in the usual way.

At the moment, WELturn is not able to correctly display profiles machined on the face of a billet. Therefore:

1) you will find that the shape of the job will not be shown correctly in the part preview screen. This does not matter.

2) you will also find that running a simulation does not display the job correctly. This does not matter.

3) you will also find that the real-time on screen display of machining does not show the job correctly. This, too, does not matter. You may like to turn off this feature: go to File - Settings - and turn off Show real-time graphics.

Provided that the NC code is correct, WELturn will machine the job correctly.

The neutral tool is not the only tool which can be used to machine profiles on the face of a job. Any other appropriate tool can be setup and used in a similar manner.

Defining Tools in AlphaCAM
Lathe Tools
Other Lathe Tools
Set the Tool Offsets
Tool Change Position
Tool Setting Microscope