In this tutorial you will see how to perform a semi finishing operation and
edit leads and links after the toolpath has been created. The final section of
this tutorial is to produce an NC program. For this tutorial we will
require a new ball nose tool. In the tool database we can search by tool type.
Select ball nose as the type and search. Select the 16 millimeter ball nose and
press create tools. Close the database.
You may want to reuse tools in other projects and their associated holders.
We can add tools to our database by right clicking on the tool and saying add to database.
Update the database if prompted to do so. Note we are adding a tool and
its holder. The holder from our end mill can now be
applied to our ball nose tool making sure the ball nose tool is active, select
the holder database icon. Apply the holder and close the form. Edit the tool
and adjust the holder overhang to be 60 millimetres.
We now need the toolpath. From the toolpath creation dialog, select the
finishing section and choose a steep and shallow toolpath.
A steep and shallow toolpath is a combination toolpath which splits the
model into steep angled areas and shallow angled areas, automatically
applying two different toolpath types to those regions. For this part a
Constant-Z toolpath is used for the steep areas and we will be using a
3D Offset toolpath for the shallow areas.
Name the toolpath "Semi Finish".
We will then set the step down to be calculated using the cusps with a cusp height as
0.1 millimeters. The step-over will be set to two
millimeters since this is a semi finishing toolpath will also leave half
a millimeter of thickness on the part. Hit calculate to generate the toolpath.
Toolpaths will inherit some of the settings from the previously active toolpath
In this case leads and links of the semi finishing toolpath have been
inherited from the roughing operations. From the toolpath edit tab, select the
toolpath connections button to edit the leads and links.
Under the lead-in tab, choose a surface normal arc and set the angle of 90
degrees and a radius of 8 millimeters. Copy these settings to the lead out also.
In the links tab change the first choice to be a circular arc and increase the
distance to 50 millimeters to set the maximum distance over which this type of
link will happen. By selecting apply and accept the leads
and links will be modified. Note that the toolpath did not require any recalculation.
This toolpath can also be added to the
stock model and we can recalculate it.
Hiding the model, block and toolpath
reveals the stock model state after the semi finishing.
The final section of this tutorial is to produce an NC program.
To output NC code you will require the Autodesk Manufacturing
Post-processor Utility installed.
From either the explorer tree or the NC program tab in the ribbon, create an NC program.
Change the name to O0001.
For the option file, browse to the Manufacturing Post-processor Utility
folder in the public documents area and select a post processor from the generic
folder. In this case we will select a Fanuc post-processor.
Accept the form.
The toolpath can be added to the NC program
in many ways, either via the ribbon, the context-sensitive
right-click menu, or by simply dragging and dropping.
Once all three toolpaths have been added a summary list shows the major toolpath settings.
The NC program can be written by pressing the right button.
To see the NC program select the view file option.
The part is now ready for some finishing toolpaths.
Save the project to complete this tutorial.