In this unit, we discuss the kind of machining modules that can be carried out on a CNC milling machine. Depending on the softwares that is being used, the name of these modules varies. As we are using Pro/NC as our demonstration software, we will also identify the name used under Pro/NC. We will discuss 3 modules in detail and introduce to you what is needed to work in these modules. 1. Profile Milling Other softwares may call this contour milling. Under this module, the software need to know how you want to approach/retract from the workpiece. How much you want to leave behind (or overcut, if needed), and how many rounds that you want to loop. 2. Pocket Milling Pro/NC has a powerful module called Volume Milling, and it has also a Pocketing module. We are using the Volume Milling to create Pocket Milling. Regardless of the name, what is required include, approach point, cutting method, cutting direction and how deep you want to cut. We will also discuss about the problems arises from the inclusion of an island. 3. Cycles Pro/NC called this module, Holemaking. As the name suggests, it is mainly in the making of holes, countersink hole, tap hole ream hole, deep hole, etc. What the module requires include the initial height, retract height, depth of the hole, peck drilling parameters etc.
Monday, January 31, 2011
Monday, January 24, 2011
Machining and Tooling Parameters
To machine efficiently, we need to specify parameters that are required by the individual machines. Furthermore, depending on the process that is being performed, the parameters may vary. Some parameters have special meaning when applied to certain toolings. For example, step over distance for a ball endmill need to be much smaller than a flat endmill. Zig zag or spiral tool path need to be specified when we are removing material inside a cavity. Profile increment need to be specified when finishing and roughing need to be done in profile milling. This chapter aims at explaining these parameters one by one.
Sunday, January 23, 2011
Calculating of step over distance and scallop height
Whenever there is an area to be cut, the cutter need to traverse back and forth in order to cover the whole area. Most of the time the surface area to be cut is much bigger than the diameter of the cutter. As such, the cutter need to "Step Over" in order to cover the whole area. At the same time, the "Step Over" must be smaller than the diameter of the cutter in order not to leave a ridge of uncut material behind. Further complication is the use of a ball end mill, which can affect the surface roughness when the area is being machined. The waviness of the surface can be defined by the term "Scallop Height". With all these considerations, a set of mathematical procedure has been developed to help us to calculate the appropriate values. The video below is supposed to illustrate that. REMEMBER, when you are watching the video you can always pause it for you to think and absorb the detail.
Monday, January 17, 2011
NC Motion Control
NC control system can be categorized into the following:
1. Point to point system
2. Straight cut control system
3. Contouring control system
Contouring, being more complicated, can also be divided into 3 subsystems.
3.1 2D Contouring system
3.2 2½D Contouring system
3.3 3D Contouring System
In order to cut along the contour, the computer need to run an utility called an interpolator.
There are 5 types of interpolators:
1. linear interpolator
2. circular interpolator
3. helical interpolator
4. parabolic interpolator
5. cubic interpolator
1. Point to point system
2. Straight cut control system
3. Contouring control system
Contouring, being more complicated, can also be divided into 3 subsystems.
3.1 2D Contouring system
3.2 2½D Contouring system
3.3 3D Contouring System
In order to cut along the contour, the computer need to run an utility called an interpolator.
There are 5 types of interpolators:
1. linear interpolator
2. circular interpolator
3. helical interpolator
4. parabolic interpolator
5. cubic interpolator
Monday, January 3, 2011
Introduction to PC-CAD/CAM
As manufacturing continues to go for more sophistication, parts are getting smaller and more complex. Modern design also incorporates fancy, curvy shapes into their products. Conventional machining processes can no longer be used to achieve the kind of precision and fanciness that modern parts require. In order to assist manufacturers to deliver their products timely, accurately with the fancy look, softwares are used to turn computer-designed parts into machine codes, and subsequently, the codes are used in CNC machines to machine the intricate parts. By integrating the design and machining process, the process becomes faster and less-prone to error. Before the codes are used in actual production, the machining process could be simulated on screen to make sure that the code actually delivers the final product that the designer has dreamed of. Please refer to Unit 1 in the handout and complete the tutorial at the end of the unit. You can now view the answer to the tutorial from the following slide.
Additional assignment:
Write your comment and suggest what the world could be like if there were no computers to help us to design and manufacture. Look around you and suggest something that could not even exist if there were no computers to help.
Additional assignment:
Write your comment and suggest what the world could be like if there were no computers to help us to design and manufacture. Look around you and suggest something that could not even exist if there were no computers to help.
Saturday, February 6, 2010
Questions about Fixed Cycle
CNC mill exercise 4C: this is a sample question to illustrate the use of G81 and G83 commands. It is purposely made to change tool to demonstrate the two commands. If you do not need to change tool, it is not necessary to go home (G28).
Using G98 is never wrong. In fact, by default, it is always G98. It goes to the initial plane, making it safe, but wasting time. If you use G99, the danger is there.
You typed polit hole, I think you misspelled the word. It should be pilot hole. It is a hole that is used to guide subsequent drilling. In your first year, you may have leant centre drill. A centre drill acts the same as a pilot hole.
Both G81 and G83 are used to drill through holes, the difference is that if you r drilling a deep hole, you use G83, it may be blind or through hole.
Mostly, holes are drilled using twist drills. In our course, if it is not specified, all holes are drilled using twist drill, tip angle 118 degrees.
Countersink hole can be drilled before or after. However, by drilling countersink hole first, one can use it to serve as a pilot hole, thus saving the effort of machining a pilot hole to guide the subsequent operations.
It is not wrong, if you forget to turn off the coolant and the spindle at the end of the program because G2 or G30 command will turn these off at the end of the program. However, some tools feed the coolant through the tool itself, especially drills. If you forget to turn off the coolant at the end of the machining operation, the tool will carry the coolant when it goes home. (G28) So, it is advisable to turn the coolant off immediately after all the machining operations are done.
G81 is modal, you do not need to repeat it if it is not changed. Same for G98 or G99. So both ways of writing will not be considered wrong. Only that it is not necessary to repeat what is being modal.
Using G98 is never wrong. In fact, by default, it is always G98. It goes to the initial plane, making it safe, but wasting time. If you use G99, the danger is there.
You typed polit hole, I think you misspelled the word. It should be pilot hole. It is a hole that is used to guide subsequent drilling. In your first year, you may have leant centre drill. A centre drill acts the same as a pilot hole.
Both G81 and G83 are used to drill through holes, the difference is that if you r drilling a deep hole, you use G83, it may be blind or through hole.
Mostly, holes are drilled using twist drills. In our course, if it is not specified, all holes are drilled using twist drill, tip angle 118 degrees.
Countersink hole can be drilled before or after. However, by drilling countersink hole first, one can use it to serve as a pilot hole, thus saving the effort of machining a pilot hole to guide the subsequent operations.
It is not wrong, if you forget to turn off the coolant and the spindle at the end of the program because G2 or G30 command will turn these off at the end of the program. However, some tools feed the coolant through the tool itself, especially drills. If you forget to turn off the coolant at the end of the machining operation, the tool will carry the coolant when it goes home. (G28) So, it is advisable to turn the coolant off immediately after all the machining operations are done.
G81 is modal, you do not need to repeat it if it is not changed. Same for G98 or G99. So both ways of writing will not be considered wrong. Only that it is not necessary to repeat what is being modal.
Monday, January 4, 2010
Coordinate System
In this first lesson, we talk about Coordinate System. Every workpiece that we machine must have a workpiece coordinate system (WPC) and is defined using G54. There are 3 axes on every coordinate system, one is X axis, running left-right along the machine, one is Y axis, running towards-away from the operator, one is Z axis, running up and down vertically. Once we have this coordinate system, any point or line can be fully described using their corresponding X, Y and Z values. If the points are always defined with reference to the workpiece zero point, it is called absolute position programming (G90). If the points are defined with reference to the current position, it is called incremental position programming (G91).
For every points in the diagram above, write down their respective X and Y values using G90 method, followed by using G91 method.
To machine the workpiece based on the coordinate system, we need to instruct the machine how to cut, from where to where. These instructions are called progamming codes. Every program comprises of blocks, words and addresses.
To instruct the machine simply to move from one point to another, we use the command G0. When we move in air, we can move very fast, making use of the maximum feed rate as provided by the machine builder. To instruct the machine to cut into the workpiece (removing metals along the way), we use the command G1. In this case, however, we need to tell the machine how fast it can move. This is to be defined using the F word. This value depends on what material we are cutting and what kind of tool we are using.
We also need to define the spindle rotation using the S word.
An example program for Mazak machine is as follows:
G0 G90 G40 G94 G21 G17
T1 M6
G90 G54 S597 M3
G0 Z100.0
G0 X-30.0 Y-30.0
G0 Z10.0
G1 Z-20.0 F119
G1 X0.0 Y-30.0
Y110.0
X57.0
Y147.0
X155.0
Y65.0
X42.42 Y0.
X-30.0
Y-30.0
G0 Z50.0
M2
Based on the program given above, can you draw the shape of the workpiece on a piece of paper as an additional exercise?
For every points in the diagram above, write down their respective X and Y values using G90 method, followed by using G91 method.
To machine the workpiece based on the coordinate system, we need to instruct the machine how to cut, from where to where. These instructions are called progamming codes. Every program comprises of blocks, words and addresses.
To instruct the machine simply to move from one point to another, we use the command G0. When we move in air, we can move very fast, making use of the maximum feed rate as provided by the machine builder. To instruct the machine to cut into the workpiece (removing metals along the way), we use the command G1. In this case, however, we need to tell the machine how fast it can move. This is to be defined using the F word. This value depends on what material we are cutting and what kind of tool we are using.
We also need to define the spindle rotation using the S word.
An example program for Mazak machine is as follows:
G0 G90 G40 G94 G21 G17
T1 M6
G90 G54 S597 M3
G0 Z100.0
G0 X-30.0 Y-30.0
G0 Z10.0
G1 Z-20.0 F119
G1 X0.0 Y-30.0
Y110.0
X57.0
Y147.0
X155.0
Y65.0
X42.42 Y0.
X-30.0
Y-30.0
G0 Z50.0
M2
Based on the program given above, can you draw the shape of the workpiece on a piece of paper as an additional exercise?
Subscribe to:
Posts (Atom)
