In this tutorial you'll understand tool creation and the tool database, learn how
to create a roughing toolpath and how to define feeds and speeds, and be
introduced to toolpath editing. We'll begin with tool creation. Tools can
be created either by right-clicking on the tool section in the explorer window
or via the ribbon either in the home area or the dedicated tools tab.
To create a tool select the desired tool type. In this case we will select a flat
end mill to open the tool definition dialog box. The first page is used to
define the cutting portion of the tool. We will call this tool EM20, give it a
flute or cut length of 40 millimeters and a diameter of 20 millimeters.
Once a valid tool is created it will appear in the graphics window. It can be shaded or
unshaded again via the right-click menu or through the ribbon also.
Let's define the number of flutes as four but for now we will leave the tool
number unassigned. Non-cutting portions of the tool are defined in the shank tab.
We will add a shank of the same diameter and specify a length of 60 millimetres.
Finally we will add a simple holder from the holder tab. Add the first holder
component defining an upper diameter of 50 millimetres and a lower diameter of
40 millimetres. We will set a length of 5 millimetres. Both shanks and holders can
be made up of multiple components so we will add a second component with an
upper diameter of 80 millimetres, a lower diameter of 50 millimetres and a
length of 100 millimetres to complete the tool assembly. Close the form the
tool is now displayed in the explorer tree with the marker indicating that it is
active. Tools can also be saved to a database and reloaded when required.
Select the tool database icon. If we search we can see that the default tool
database is empty. Let's load a sample database. Select the tool database
manager icon, select database settings. From the folder icon we can load the
tool database in the examples directory. Select the sample tool database .MDB file
and select open. Close the form and then search again.
Note we now have a range of tools in our database. To narrow the search down enter
a maximum and minimum diameter of 50 millimeters and then search again.
Select the TR 50 tool and press create tools and then close the database. The new tool
has now appeared in the project. We will use this tool for our roughing toolpath.
As with tools, toolpaths can be created either by right-clicking on the tool
path section of the explorer window or via the ribbon in either the home area
or the dedicated toolpath tab. Select the toolpath creation button and from
the 3D Area Clearance section choose model area clearance.
Note that our workplane, block and tool are already defined. If you are not
continuing from the previous tutorial you may need to just recalculate your
block as before. Autodesk PowerMill has an incredibly high
degree of toolpath control and this form contains plenty of options to produce
the desired toolpath. From the model area clearance section we will define the
offset type to offset model, this will move the tool in towards the part with
the model defining the toolpath offset shape. Since we are using a 50 millimeter
tip radius tool we will use a 20 millimeter step over and a 3 millimeter
step down. A 1 millimeter thickness means the toolpath will leave one millimeter
of material around the part. Our tool is non center cutting so to protect it the
unsafe segment removal function will remove enclosed segments smaller than
95% of the tool diameter, preventing the tool from engaging its non cutting
region with unmachined stock. Automatic verification allows us to check against
the model and stock as the toolpath works its way down the part. Any areas of
collision will be automatically removed as the toolpath is calculated.
For the rapid moves, we will calculate the clearance planes and modify the lead-in
or approach to ramp into the part where possible. The final settings we will
change are the feeds and speeds. Spindle speeds and feed rates can be
modified to suit, for example from the tooling manufacturer's catalog values.
Simply enter the values for spindle speed, cutting feed rate etc. The full
feeds and speeds form can be accessed from the feed rate form icon, where
cutting conditions can be set based on other factors such as surface speed and
feed per tooth. Close the form and calculate the toolpath.
Rapid moves, leads and links, and feeds and speeds can all be adjusted later
without the need to recalculate the toolpath.
This quickly generates a toolpath to remove the majority of the material.
Note the warning indicates that some areas will have additional material than the
desired one millimeter thickness. This is as a result of our collision avoidance
so this is okay since we will be forming some rest machining later. The toolpath
slices can be viewed using the dynamic section tool, set the axis to be in Z
switch the back plane on and move its slider to the right. Lock the planes
together and then move them left and right to see the toolpath slices.
Close the form.
Autodesk PowerMill has a range of powerful
toolpath editing tools. On this part it is likely that these corners would be
machined in a different operation, possibly from the other direction, so we
have some toolpath segments that we wish to remove. This is a very quick
process. Hide the model for clarity and then simply select the segments you want
to remove by holding down the left mouse button and dragging over them. Hit the
delete selected button in the ribbon from the toolpath edit tab. This can
also be done from the context-sensitive, right-click menu by selecting edit
delete selected. Continue until all the unwanted segments are removed.
Note that any leads and links that are required will be automatically generated.
We can now save the project for use later to complete the tutorial