Milling Tool planes: Mill-Turn
Use the Milling Tool planes, Mill-Turn dialog box to quickly create planes based on tool planes created
from a flat face or cylinder of the part. Naming and origin location of
the plane is automated with intelligent naming that relates to the machine's
position. This allows you to create many tool planes without exiting the
dialog box, making it an efficient way to set up your job.
The information you set in this dialog box is saved and can be used
in the Setup page
for milling toolpaths.
Use Prompt for origin to have
Mastercam prompt you for an origin when you select the geometry for the
tool plane. If you do not select this option, the origin will be set from
the selected Spindle origin.
Use Alternate B-axis solution
to name the plane to reflect the alternate B-axis solution (<0 or >180
degrees). This depends on the B-axis angle being within the machine limits
defined in the machine definition. If the angle is not within these limits,
the checkbox is ignored and the standard 0-180 solution is used. The Alternate
B-axis solution is used when there are two solutions, one solution from
0 to 180 and one solution less than 0 or greater than 180. When the angle
is zero then there is only one solution.
How to create a new plane
- Select the axis combination to which
you want to assign the new tool plane. Only axis combinations with a Y-axis
are displayed.If an axis combination has no Y-axis, only
C-axis work types can be used and the tool planes for C-axis work
types are automatically generated by job setup.
- If job setup is set to Single
pieces of stock – No pickoff, only axis combinations for
the spindle that holds the part are available.For example,
if the part is in the left spindle and there is no pickoff, only
left spindle axis combinations are available.
- Select a spindle origin from the Spindle
drop down list. If there is only one spindle origin
specified for the selected axis combination, you will not have
a choice.
- Select Prompt
for origin to have Mastercam prompt you for an
origin when you select the geometry for the tool plane. Use this option if you want the origin
to be used by the WCS when this plane is selected. If you do not
select this option, when you select the plane, the planar orientation
will be applied, but the origin will not change.
- Select Alternate
B-axis solution to name the plane to reflect the
alternate Z-axis solution (<0 or >180 degrees).
- Enter a value other than 0 in the Face tool plane C-axis angle field to control
the orientation of the tool plane.
- Use the Seed name
field to edit the default Machine Group name. This is used as
a prefix to the plane name.
- In the graphics window, select the flat
face or cylinder that you want to set the new tool plane to, and
then select its origin if prompted. The name of the new tool plane
appears in the list window at the bottom of the dialog. If there is already a tool plane designated
for the face or cylinder that you have selected, no new tool plane
is generated.
- Click Apply
to save the planes, remove the planes from the Milling Tool planes
dialog, but leave the dialog box open. Click OK
to save the planes and close the Milling Tool planes dialog box,
or just to close the dialog box if you have already saved the
planes.
- Click the tool plane name and a gnomon
is displayed on the screen showing the tool plane orientation at
the location of the tool plane origin
- Right click a tool plane name to open
a menu with an option to delete the tool plane. This is useful
if you select the wrong face or the wrong origin location.