From words
to deeds. 3 axis
milling practice
Now is time to discover, thanks to a guided practice, which are the best
working strategies in order to obtain the best finish for the detail shown
below.
You’ll need to download the file in a .MC9 format which contains the
mathematic pattern to use as a useful geometry for setting all the various
workings.
Click HERE to download the file
Once you open the geometry in the file, you can go on with the
creation of the other workings required for the production of the detail at
issue.
Introductory working settings
First of all you need to create a new profile where to hold all the
following operations, then you can choose the
One edge
function
from the
Create menu.
The following picture shows the chain you must build to contain the
workings.
After this operation you can define the shared technological parameters far
all the workings, which are in the
Job setup menu.
Select
Toolpaths
and then
Job setup
from the MAIN MENU,
to go to the specific windows where you’ll have to put the following
parameters:
-
Stock
Size
Put in the specific boxes the following values: Y = 166mm; X
= 166mm; Z = 48mm
-
Stock Origin
Leave the X and Y coordinates to 0 and set the Z coordinate to 48mm,
making sure that the positioning point is set as shown in the picture
below:
-
Check
the Display
stock
option
-
Material:
press the Select button and set an ALUMINIUM mm 7075
-
Feed
calculation:
from Material
Once you made your choice in the
Job setup menu, you
can go on in the creation of your workings.
Surface roughing
The first operation you’ll have to do is the surface roughing thanks to the
specific function that is activated by:
After choosing the right options from the
Select drive surfaces
menu, select all the existing surfaces and then press
Done to reach
the window with the workings’ parameters.
Choose from the Tool parameters table of the Surface Rough Pocket
window a End Mill Ø 15 mm tool and go to the Define tool
window so that you can set the right cut parameters by pressing the Calc.
Speed/Feed
button. Then you can return to Tool parameters to insert
“Surface Rough” in the Comment box and then pass to
the next table.
-
Make the following
changes in the Surface parameters table, :
-
Start the Clearance and
Retract options with an Absolute
value of 50mm.
-
Set the Feed plane with the
Incremental option and make sure it has a
value of 5 mm.
-
Insert a value of
1 mm in the
Stock to leave on drive surface
box
-
Set the Tool
containment on the "center" option
Now you can can go to the
next table.
Set the parameters of the Pocket parameters table as follows:
-
Total tolerance
= 0.1 mm
-
Maximum stepdown
= 3 mm
Press the Entry - helix button and go to the
Helix/Ramp parameters windows, then
you can insert in the Ramp table the following parameters:
Make sure that the
If ramp fails
box is set on Skip
and that the Entry feed rate is set on Feed rate.
Choose as working strategy the Constant Overlap Spiral in the
Rough
box.
After having set all the parameters press OK without making any other
changes to the settings of the various tables. Mastercam will ask you to
select an order to follow as control profile for the working; choose the
profile you just create and press Done to evaluate the tool course.
The so set working must be
similar to the one shown below.
Sides semi-finish
Now choose Toolpaths,
then
Surface finish and then again
Contour from the quick
menu of the Operations Manager and select all the existing surfaces;
press Done to go to the Surface Finish Contour window.
Select a End Mill Ø 10
mm tool from the Tool parameters window and then go to the
Define tool
window to set the right cut parameters by pressing the Calc. Speed/Feed button. Return to the
Tool parameters window and
put
“Sides semi-finish” in the Comment
box. Once you filled all the settings of this table, you can go to the
following one.
Insert the following
parameters in the Surface parameters window:
After this you can go to
the last window of the Finish contour parameters table, set the
Transition
box on the Follow surface option and then insert the following
settings:
Once you set these
parameters, press the Gap settings button to go to the Gap
settings
window and make the following changes:
-
Start the
Use
plunge and retract rates in transition motion option
-
Start the
Check transition motion for gouge option
-
Start the
Check retract motion for gouge option
Then, without making any
other changes to the existing parameters, leave the working window. Choose
always the same order as control profile and then press Done to create
the tool course.
The working result must be similar to the one shown below.
Flats semi-finish
Once you checked the
working, return to the Operations Manager window and choose
Toolpaths,
Surface finish and then Shallow from the quick menu; select again
all the surfaces and, by pressing Done, go to the Surface Finish
Shallow window.
Choose a Bull Mill Ø
10 mm tool with a 4mm Corner radius from the
Tool parameters
table and then go to the
Define Tool window in order to set the right cut parameters by
pressing the Calc. Speed/Feed button. Return to the Tool
parameters table and insert “Flats semi-finish” in the
Comment box. Once you made all the settings in this table, you can go
to the next one.
In the Surface
parameters table, set the Tool containment always on "center" and
then make sure that the Stock to leave on drive surface is on 0.2 mm before going to the following table.
In the Finish shallow
parameters table, set the following parameters in the right
boxes.
Then press the Gap
settings
button to go to the Gap settings
window and make the following changes:
-
Start the Use plunge
retract rate in gap option.
-
Start the
Check gap motion for gouge option in the Motion<Gap size, keep tool
down box.
-
Start the
Check retract motion for gouge option in the Motion>Gap size,
retract box.
-
Start the
Optimize cut order option just under the box.
Once you made these
changes, return to Finish shallow parameters and, after selecting the
control profile, leave this window in order to let the system evaluate the
tool course .
The final result must be similar to the one shown below.
Sides and flats finish
By this point, you'll need
to finish the surfaces. To
make so, looking at the fact that you'll need to use the
Surface finish Contour and the
Surface Finish Shallow again, instead
of setting all over again, you can redo the last two operations made to
avoid useless passages.
After having doubled the operations and edited the comments, the operations
list will look as follows.
Now go to the Parameters
window of the
Surface finish Contour
operation and make the following changes:
-
In the Tool
parameters window, select a Bull Mill Ø 8 mm tool with
a 3mm Corner radius and then go to the Define Tool
window to set the right cut parameters by pressing the Calc. Speed/Feed button. Once you made so, you can go to the next table.
-
In the Surface
parameters window, set the Stock to leave on drive surface
to 0 mm leaving unchanged the other options before going to the next table.
-
In the Finish contour
parameters window, put the following parameters in
the right boxes:
-
Total tolerance
= 0.02 mm
-
Maximum stepdown
= 0.2 mm
-
Corner rounding radius
= 0 mm
Then press OK to
return to the Operations Manager window.
Within the blank area of
Operations Manager, the just edited working has been invalidated so
you must press the Regen Path button to update it.
Now select the Parameters table of the Surface Finish Shallow operation and use the same
Bull Mill Ø 8 mm tool
with a 3mm Corner radius of the previous operation.
Within the Surface
parameters table, set the Stock to leave on drive surface box with a value of 0.
Then set the following parameters in the right boxes of the Finish
shallow parameters
window :
Then press OK to
return to the Operations Manager window.
Within the blank area the just edited working has been invalidated so
you must press the Regen Path button to update it.
Graphic simulation
Before creating the
machine program, Mastercam gives you the possibility to check the created
tool course thanks to the Backplot and Verify functions.
Thanks to these
simulations you can see if your working follows the right planning
necessities or if you made some mistakes which lead to the creation of a
wrong piece. In the case you made some mistakes,
you can quickly return to the wrong working and make the necessary changes.
Backplot
Verify
If you had some problems
with this drill, you can download the presentation file where all the
different phases are shown step by step.
Click HERE to download the file
|
