MasterCAM Surfacing Tutorial

Avery Fabrication and Material Conservation Laboratory
MasterCAM Surfacing Tutorial
‘Surfacing’ is a machining operation in which a 3D contoured surface is carved from a block of stock material through a series of
cuts. Typically this is done in two operations, a ‘Rough’ pass and a ‘Finish’ pass. The purpose of the ‘Rough’ pass is to remove
as much material in as quick of time as possible, this is typically done with a large bit and gives a rough couduroy texture to
the material. Often the process is stopped after the ‘Rough’ process, and if the roughing operation is done with a small enough
bit the surface smoothness may be suitable for many applications. If a smoother finished surface is desirable a second series of
cuts can be made with a smaller bit at a tighter interval giving a smooth polished surface. This tutorial covers the basic operations needed to do a ‘Rough’ tool path based on a generic 3D surface.
Surface Creation
1) The creation of an appropriate surface for machining
is the first step in the ‘Surfacing’ operation. As you
prepare your surface the modeling environment should
be set so the Z-axis is vertical and the working units
are inches/feet. The optimal surface for machining is
NURBS based, this can be created in Maya, Rhino or
3DMax. The surface should be placed with the highest
point on the surface is just below the XY plane. The
mill will treat the XY plane as the top of the material,
anything above the XY plane will not be cut. The part
should also be positioned entirely in the positive XY
quadrant (upper right quadrant) of the axis
2) Once you have modeled a surface it must be exported
as a file in IGES format. If possible it is suggested
you select the individual elements to be CNC milled
and export only those pieces, avoiding the exporting of
lights, cameras, other objects, etc.
Positioning the surface in X,Y and Z
Exporting the surface as an IGES file
File Import and Preparation
1) Once you have an IGES file you can quit your 3D modeling application and open MasterCAM Mill. To import
your new file in the MasterCAM select ‘File’ -> ‘Converters’ -> ‘IGES’ -> ‘Read File’, a file dialog box should
appear. Locate your IGES file and open it. A second
dialog box with ‘IGES Read Parameters’ will appear,
leave all the settings as they are and click ‘OK’. You
will be prompted to ‘Delete Current Part’, unless you are
importing your file into an existing MasterCAM model,
click ‘OK”. Your model should now appear in plan view.
2) Zoom out to view the entire model by clicking the
‘Screen Fit’ button (the ninth button from the left at the
top of the interface). Once you can see your entire model
in plan it is a good idea to verify that it imported with
the correct scale and in the correct position. To verify
the scale measure the overall dimension of the piece, or
a know dimension of a portion of the piece. To measure
the piece, select ‘Analyze’ from the main menu. From
‘Analyze’ choose ‘Between Pts’ and ‘Sketch’. Click with
the mouse on two points on the piece, the distance between those points will be displayed in the dialog area
at the bottom of the screen. If the distance is correct
then your piece imported with the proper scale, if not,
you will need to scale your piece in MasterCAM before
you begin the tool-path.
Importing the IGES file into MasterCAM
Verifying the scale of the surface
3) Once you have verified the scale you can change the
view to a 3D view by clicking on the ‘GView Isometric’
button (the twelfth button from the left in the top row).
To verify the piece is in the correct position hit ‘F9’ on
the keyboard, the axis will appear. You piece should be
below the XY plane and in the top right quadrant of the
axis.
Verifying the part location relative to the XY plane
Creating the Tool-path
1) Return to the ‘Main Menu’ by clicking the ‘Main Menu’
button on the left side of the interface. From there
select ‘Tool-paths’ -> ‘Surface’ -> ‘Rough’ -> ‘Parallel’
-> ‘Unspecified’.
2) Next you will be prompted to select the ‘Drive Surfaces’,
these are the surfaces that you wish to machine. To
select the surfaces click on one of its edges using
the mouse. Once you have selected your surface click
‘Done’, a new dialog box will appear.
Selecting the drive surfaces for toolpathing
3) In the new dialog box right-click in the white box in
the middle, choose ‘Get tool from library…’ from the
contextual menu. Select the tool you wish to use. Since
this is a surfacing operation you will was an ‘Spherical’
or ‘Ball’ endmill, we’ll choose a 1/8” diameter. Click OK
to return to the ‘Tool parameters’ dialog box.
4) Next click the ‘Rough Parameters’ tab to bring up all the
rough surfacing settings. In this dialog box you must
enter the ‘Max Stepover’ and the ‘Max Stepdown’. The
‘Max Stepover’ is the distance the bit moves over each
time it makes a machining pass, this determines the
amount of overlap with the previous cut. The smaller
the stepover, the more overlap between cuts and consequently the smoother the finish on the piece – and the
longer the cut time. As a rule-of-thumb a good stepover
is one-half of the diameter of the bit. For example, a
quarter-inch bit would have an eighth-inch stepover.
The ‘Stepdown’ is the increment used for each vertical
step. This does not affect the finish as in the stepover,
but instead is a factor of cutting speed and material
hardness. Unless milling through a soft material the
machine cannot typically cut down to the level of the
finish surface with just a single pass, typically the material has to be taken off in layers. The thickness of the
layers is the stepdown increment. A good rule-of-thumb
for the step-down increment is to use the diameter of
the bit. For a quarter-inch bit the stepdown would be
one quarter inch. Using a larger stepdown will decrease
the cutting time, but you will run the risk of breaking
Choosing the proper milling bit
Setting the roughing parameters
the bit.
For this example we will use .125 inch step down and a
.0625 step over.
In the diaglog box you can also select whether to cut
‘One-way’ or ‘Zig-zag’. Using ‘One-way’ means that the
cutter will only cut in one direction as it moves backand-forth across the material. This may be important
if your material has a grain. The ‘Zig-zag’ method cuts
in both direction as it moves back-and-forth, making
the machining time quicker. Select ‘Zig-zag’ for this
example.
5) After entering the machining parameters and clicking
‘OK’ you will be prompted to select the ‘Tool Containment Boundary’, click ‘Done’. Your tool-path should be
automatically generated.
Generating the toolpath
Analyzing and exporting the tool-path
1) After you have created your tool-path you can use some
of the tools built into MasterCAM to analyze is performance. To view a simulation of your toolpath cutting
select ‘Operations’ from the ‘Toolpaths’ menu. If you
cannot find the ‘Toolpaths’ menu you can click on the
‘Main Menu’ button. The ‘Operations’ button will open a
dialog box listing all the paths in your model. You can
select ‘Verify’ and the toolpath will disappear and a
rendered block of material will appear on screen as well
as a playback controller. Clicking on the play button will
play the simulation. If the playback is too quick you can
adjust the slider on the right to change the speed.
Verifying the toolpath
2) To export your file for machining you must ‘post-process’ the file. This means that the generic tool-path
information must be converted to machining-code specific to the CNC milling machine that the school owns.
This post-process operation is found under ‘Toolpaths’>’Operations’ from the main menu. In the ‘Operations’
dialog box select the button labeled ‘Post’, this will
open the ‘Post processing’ dialog box. Check ‘Save NC
File’ and click ‘OK’. You will be prompted to save your
file, click ‘OK. The file will be saved and a text editor
will open with the Gcode for your review. Close the text
editing window. The NC file you have created can now
be transferred to the mill for cutting.
Post-processing the toolpath to generate the NC file