CNC milling
Introduction
Computer Numerically Controlled milling (CNC), is the process of machining physical objects from
2d or 3d digital information. The process of CNC milling is a 2-step procedure. The
first step is Toolpathing, the process of translating a 3D or 2D computer model into a series of
'paths' for the CNC mill bit to follow as it excavates the model from a block raw material. The second
step of the procedure is the actual machining, which involves translating the toolpaths into commands
to small 'stepper' motors in the milling machine that move the head of mill incrementally in the X, Y and Z directions.
This document will give a brief overview of using the CNC milling machine and includes basic information of Materials, Hardware
and Software.
Software
The procedure for generating toolpaths and machining a model uses two software programs, MasterCAM and
Techno, corresponding to the two steps in the machining process. MasterCAM is a full modeling software package as well
as a machining software package and can be used for producing a 3D or 2D model, though is easiest to use an separate program
such as form-Z or Alias. Modeling will be discussed later in this document. The MasterCAM program has several methods
for generating toolpaths from 2D data, 3D data and full 3D computer models. The second program, Techno, is a proprietary software
supplied by the producers of our milling machine. This program is for directly interfacing with the machining hardware. It can
interprets toolpaths into a series of stepped movements in the X, Y and Z directions; it can also be used to
manually position the machine head before machining.
Special Note: The software is operated with a hardware security key. This key is
the equivalent of the license, if it is misplaced another liscence will have to be purchased and the
milling machine will be inoperable. <
Reference Manuals
Manuals for MasterCAM Software should
be in both the library reserve desk as well as in the milling room. The manuals for the software are
in three sets:
-
- Reference Manual Set- Mill 386 This
volume contains the complete reference information for the software.
It's format is geared towards the well informed user.
-
- Basic Concepts - Tutorial
-
- Techno Isel Manual - This volume
is loose bound in a binder. It is provided by our distributor
of the software and is probably the most useful. It contains an
abridged version of the Reference Manual in an easier to use format.
It includes tips and excludes needless information and should
prove to be invaluable.
Modeling
If you are familiar with modeling software other than MasterCAM it is
often easiest to model in a separate modeling program. However - for the most
consistently correct results it is best to model in MasterCAM. For any 2D toolpaths
it is highly reccommended that you use MasterCAM for you modeling. Its drafting program
is similar to AutoCAD and it is a very powerful 3D modeler although its interface is rather
burdensome and slow to use. Modeling with MasterCAM will not be discussed here but the manuals
offere extensive information on the Modeling/Design module of the software.
Modeling in other software packages.
If you have chosen to use a different program to model you object it is important to note that the milling machine is
Vector based and it is best to used a software program that uses similar vector based geometry, the software best suited
for use with the mill (besides MasterCAM) is Alias. All other programs are polygon based and cause problems in generating toolpaths
as well as drastically slowing the machining process.
Alias
When converting from Alias use IGES file format. IGES format supports spline geometry and will convert the best from Alias to
MasterCAM. When saving your model from Alias use the File--->Export--->Save Active As option so that only the selected portions
of your model are saved. This will avoid any problems from exporting unwanted object that are ghosted or hidden in your Alias model.
Form-Z
While it is not recommended it is also possible to machine object from files created in form-Z. If you are using form-Z save your
models as IGES format and specifing the New Lines option to be MS-DOS.
Generating Toolpaths
Toolpaths are the information that the milling machine
uses to direct the drill bit through the material. These are the single most important thing in CNC milling. A full
understanding of these is critical for producing a good model.
Toolpaths operate as vectors. They have direction,
magnitude and position in space, these translate directly into the direction and postion of the milling bit in space.
Toolpaths come it two types, 2d and 3d. The 2d toolpaths are for cutting from 2d 'sheet' material, the 2d toolpath
works only in the X and Y direction and is the equivalent of a cookie cutter operation. Although these are not very complex operations, they are the toolpaths
that the mill is best suited for. Machining 2d cuts is, because there is less information and less material to remove, a much
quick process than machining 3d objects. Also - because the machine only works from the top down, it is very limit in the range
of 3d forms it can fabricate. 3D toolpaths work in the X, Y and Z direction and are for sculpting and excavating a material.
The toolpathing operation is critical to machining because it is the point where the real world contraints are applied to the
3D virtual model. When creating a toolpath aspects such as bit size, material type and the limitations of the machine must
be taken into consideration.
Direction - Each toolpath is generated from a surface or line. When generating 2d cuts from lines a direction must be specified.
Select the first part of the edge you wish to define.
A line will be added over top of your segment with a diamond marker
drawn at one endpoint. This node signifies the direction that
the vector is going. To control the direction, select on the end of the segment at which point you want the machine
bit to start. In other words, pick the end of the segment opposite that which you wish the diamond to appear.
Bit Size - When milling a 3D surface the object must be excavated from the material. To excavate the object the mill must
slowly remove layer after layer of material, the material cannot be removed in a single step or the bit will break.
This process of stepping slowly down into a model is called depth cuts. When milling from a solid block of
material a good rule of thumb is to never cut deeper than one half the diameter of the bit in any single cut, this means that
the depth of the depth cuts should be no deeper than one-half the bit diameter.
The diameter of the bit also dictates how fast the machine can move in the X and Y directions. In order to have a
smooth finish the bit must overlap itself each time it makes a pass on the milling machine. The amount of overlap is
equal to half the diameter of the bit. What this means is that a 1" wide model would have to be passed over 16 times with a
1/8" bit to cut the entire surface. What this means, in conjunction with the depth cuts limitations, the smaller the bits
size the slower and longer the object will be in the machining process
Special Note: When you are finished generating your toolpath you will be asked if you wish to Run the Post
Processor. Always answer NO.
Machining
The method of machining is identical for all models and is very methodical. Because the process can be scripted, it will
be explained in its entirety below. This process is very important and if done improperly can destroy the milling equipment as well as
cause bodily harm. Be careful at all times and wear protective eye and ear equipment. If you have any doubts about milling
please ask the DA or professor.
There are several sub-steps here, but I will present them as fluid.
They are interdependent and sequential, making it nearly impossible
to justly separate.
Once all your toolpaths are set and saved, you are ready to move
into production. With a fairly complex object, you may have several
toolpaths to run. You will need to run this sequence for each
toolpath.
Keep your finger on the ESC button
as a safety/kill switch during all adjustments to avoid damaging
the material and/or the machine!
- Make sure mill is on
- Exit MasterCAM software
- Double click on the Techno icon on the desktop
- Press F2 to select a file
- ENTER file name .NCI or scroll through the list of files with PageUp and PageDown as well as the arrow keys
- You will be prompted to set several parameters - the only ones you need to be aware of are:
- RAPID SPEED = <DEFAULT>
- CUTTING SPEED = This is the speed the bit will move
in the horizontal direction. This is determined by the material
type.
- PLUNGE SPEED = This is the speed the bit will move
in the vertical direction. This is determined by the material
type.
- F1 To save values
- You will be prompted to do a Trail? YES
- Jog? YES! This is the point at which
you will manually located the mill at the proper starting point
- You will see a series of measurements on the top of the screen
and a hot key menu in the middle. They are self-explanatory.
- F4 decrease speed to 2000
- F5 sets the step size. Step size is the unit by which
you want to move the drill bit when trying to line it up with
the edge of the material. Larger measurements can be used at first
and later, you will use very small movements.
- arrows, +, - Use as explained on the screen to direct
the bit towards the corner of the material. You are trying to
define zero for the machine. Zero should be at the surface of
the material in the z direction and at the origin of your drawing
in the x-y plane. Continue to use F5 to adjust the step a mounts
as you get closer to the target.
- Once close, reduce the step amount to the minimum and
begin creeping down towards the surface. Slip a piece of paper
between the bit and surface. When the paper resists movement,
you are 3/1000" away from the surface. That is 6 steps at
the minimum of 5/10000" or you can set it to go down that
exact amount.
- After Zero is achieved, write it down!
- F10 to save your values and return to the original
screen.
- Jog? NO MEANS GO! Choose no and the machine
will immediately begin milling.