Originally Posted by Splint Isn't communication software known as DNC? What's the difference between CNC and NC software?
Splint |
This could get complicated, but should help you understand how/what communications are, what types are most popular, and the differences between CNC and NC.
DNC is a
type of communication. It's a protocol, not software. There are 2 basic ways of sending data to the machine, (this data is in NC format, typically called an NC File, more on that later.)
The most common way is via a standard RS-232 cable connection. You connect a cable from the computer to the machine and transfer the NC data from the computer to the machine one line/block/char at a time using one of many many different kinds of transfer programs, (I made my own for this), until the entire program is stored in the machine. (This works for NC Files that are small enough to fit into the memory of the machine.) Once the entire program is stored in the machine, you can run it as many times as you need, start in the middle, make edits to it, etc etc.
You can also, if you've made changes to the NC File while it was in the machine, send it BACK to the computer to be stored as a 'proofed' or 'proved' program. So if you run the same parts 3 months from now, you'll have the same program you made changes to by sending out the 'proofed' program again.
DNC is
Direct
Numerical
Control. It is used in cases where the NC File is too big to fit into the machine all at once. It allows you to run bigger programs by sending as much data as it can, then waiting for more room to be made available so it can send more.
This method has several drawbacks, some that can be over-come with high-end DNC Software. With DNC, you set the machine up to recieve, and start sending the program out and you can begin running it while it's still sending.
Once the machine's memory is full, the DNC Software will stop sending data and
wait for part of the program to be run, (after a portion of the program is run, that data is thown away which frees up more room on the machine), and when more room is made on the machine, the DNC Software will send more data until the machine is full again. You have to make sure you can send the data faster than the machine can process it, or you will get 'pauses' while the machine waits for it's next move to be sent.
Drawbacks to this method are that you can only run the program once before having to send it out again. You can't (unless you invest in high-end DNC Software) generally start in the middle of the program. You can't make changes to the NC File after it's sent.
You asked the difference between CNC and NC; CNC,
Computer
Numerical
Control is a process in which a machine is controlled by computer data instead of by using hand wheels and knobs.
NC is the
type of data that the machine reads, typically called G-Code. It has all the codes that the machine uses to cut your parts.
This NC code is generated from a CAD/CAM program;
Computer
Aided
Design/
Computer
Aided
Manufacturing. CAD programs don't generally create G-Code, and not all CAM programs allow you to do CAD. Many do both. There are hundreds of different kinds of CAD/CAM Software, ranging from free to tens of thousands of dollars, depending on what you want to do.
Basically what you do is create the geometry that will represent the part's shape, and apply toolpaths to it. Once you've applied all the toolpaths, you run it thru what's called a "post processor". This is the process that converts the stuff you did in the CAD/CAM program into the NC File that the machine reads. (NC Files are almost alway in 'human' readable format, unlike normal computer programs that look like gibberish when a human looks at it.)
Here's a sample of some NC Code generated with Mastercam..
Code:
%
O0001
(HOUSING.NCF)
(AUG 07, 2004 09:17)
(MC8 FILE: -G_HOUSING)
(MACHINE: PRESTAGE 4 AXIS)
(MATERIAL: ALUMINUM INCH - 6061)
(STOCK SIZE: X 4.45 Y 3.5 Z 1.)
(TOOL 1: DIA 0.5000 .500 HSS EM 2FL)
(TOOL 12: DIA 0.1875 .1875 CB EM 4FL)
(TOOL 2: DIA 0.1250 .125 CB EM 4FL)
(TOOL 3: DIA 0.0312 R0.0156 .0312 Ball EM)
(TOOL 4: DIA 0.2500 1/4 C'Sink)
(TOOL 5: DIA 0.0670 .067 Drill)
(TOOL 6: DIA 0.0780 .078 Drill)
(TOOL 7: DIA 0.1400 .140 Drill)
(TOOL 8: DIA 0.0730 #1-72 Tap Roll Tap)
(TOOL 9: DIA 0.0860 #2-56 Tap Roll Tap)
(TOOL 10: DIA 0.1250 .125 x 90 Deg Spot Drill)
(TOOL 11: DIA 0.2500 .250 Drill)
(OVERALL MAX Z1.)
(OVERALL MIN Z-.8634)
N1 G00 G17 G40 G49 G80 G90 G20
N2 T1
N3 M01
( OPERATION: 1 CONTOUR )
N4 ( TOP OP 1 )
N5 M06(T1: .500 HSS EM 2FL)
(MAX-DEPTH | Z-.72)
( TOOLPATH - CONTOUR)
( STOCK LEFT ON X & Y = -.35)
( STOCK LEFT ON Z = 0.)
N6 M03 S7500
N7 G00 G90 G54 X-4.8 Y-2.175 A0.
N8 G43 H1 Z1. M08 T12
N9 Z.11
N10 G01 Z0. F50.
N11 G41 D1 X-4.75 F65.
N12 G03 X-4.25 Y-1.675 I0. J.5
N13 G01 Y-.1
N14 X-.1
N15 Y-3.25
N16 X-4.25
N17 Y-1.675
N18 G03 X-4.75 Y-1.175 I-.5 J0.
N19 G01 G40 X-4.8
N20 G00 Z1.
(OPERATION: 2 CONTOUR)
N21(OUTLINE OP 1)
(T1: .500 HSS EM 2FL)
( TOOLPATH - CONTOUR)
( STOCK LEFT ON X & Y = 0.)
( STOCK LEFT ON Z = 0.)
N22 X-4.71 Y-3.4
N23 Z.1
N24 G01 Z-.72 F50.
N25 G41 D1 X-4.66 F45.
N26 G03 X-4.61 Y-3.35 I0. J.05
N27 G01 Y0.
N28 G02 X-4.35 Y.26 I.26 J0.
N29 G01 X0.
And here's a couple of pictures from the CAD/CAM program, one showing the lines/arcs etc that represent the part,
the other showing the part as it will appear while it's being cut. (This is typically called rendering or verifying)
There's a lot more to it than this, but it should give you a better understanding.