[samualt]

I'm confused about CNC software.

I always thought the CAM software is what sent the G-code to the hardware. But Visual Mill (a prominent CAM program) evidently only takes the 3D file (IGES, Rhino, Dxf, Dwg, STL, VRML, RAW, Point Cloud) and makes a tool path or G-code file. Then you need yet another program to send the G-code to the hardware. Is that correct? If so, which program is best to send the G-code to the router (Hardware driver like Rutex or Gecko)?
I've already got my Rutex drivers, and I really like Rhino-3d which I'm told works best with Visual Mill. So I've already gone down part of the path.

Rhiono-3d --> Visual Mill --> ??? --> Rutex

Another problem I have is I'd like to design on my Desktop (a nice machine) but use a rather old laptop to control the router (Compaq Armada - Pentium 200Mhz, 128Megs ram, SVGA, Win98). Any control software work with that?

Also, what do I call a program that sends the G-code to the driver, if it's not CAD or Cam?

[turmite]

samualt I simply copy to disc or cd and transfer that way. I do have two seats of bobcad 17 and one is loaded on my cnc computer. If you have both together you can also use networking to do the transfer.

Mike

[ynneb]

Yes at first I was a bit confused too.
You will need a program like Mach2 that you can then load your Gcode into. Programs like Mach2 will then do all the talking to your servos/stepper cards and control your machine.
Fortunately Mach 2 is very cheap for what it does. ( Unilke many other expensive software programs)

As for what to call this software, I am not sure. I guess it could be called "Frontend machine operating software" ( Does anyone know the exact name for this sort of software? )

[drawbar]

I've heard of it being called NC software.
Took me a while, too, to figure out the different requirements of the different software.

Brian

[ynneb]

Yes NC software sounds like a good description.

Oh,.... about sending it to another computer. I also design on a better computer and just send the fiinished files to the operating computer via a cheap network setup.
I can't actually operate the router remotely though. Not that you would ever really want to do that. You can get cheap network cards these days for 10 bucks each if you settle for lower speed transfere. Most NC files are only small anyway. It should still only take seconds to transfere the files.

Because of the sort of computer you wish to use and the operating system you would have to use a program called Master5. This program is written by the same guy who wrote Mach2.

[HuFlungDung]

CNC controller software is what interprets the gcode and interfaces to your machine.

NC communications software is what is used to transfer gcode files from your PC into the memory of the cnc controller. This would be relevant only if your cnc controller software is installed on a remote computer.

[snaggletto]

Hello,
In your case Rhino is the CAD, Visual Mill is the CAM, Mach2/Linux EMC/many others is the control software, NC (numerical control) is correct also.

Depending on your performance needs, you may be able to use the slower PC to run Mach2 and the router. However, you will soon find out that your maximum speed with steppers or step servos is determined by your maximum pulse rate. Pulse rate is the speed of the step/direction signals coming from your PC control software. Pulse rate is largely based on CPU speed. For example, Mach2 will run in 3 modes, 25khz (demo only), 35khz and 45khz (full version, $150, does all three). However, a slow PC might only be able to run 25khz (25,000 pulses/sec on each axis), while your faster PC might easily run 45khz (45,000 pulses or steps/sec on each axis).

Say you have a high RPM servo with 1000 line quadrature encoder. That would be 4000 pulses/rev quadrature ( rising and falling edge detection on two distinct channels). Now say you have to gear reduce the servo 5 to 1. You now have 4000 pulses/rev of the motor X 5 = 20,000 encoder pulses/rev of the screw. Lets say your screw is 5TPI. Now you have 20,000 X 5 = 100,000 encoder pulses in 1 inch.

With a fast PC, Mach2 can only put out 45,000 pulses per sec, in other words your machine will travel a maximum speed of .45 inches/sec X 60 is 27 inches/min.

You can see how you can quickly use up your pulse rate, and how it can severly limit your speed.

Now lets take a low speed torque servo with a 250 line encoder and 2 to 1 gear reduction. The 250 line encoder is 1000 quadrature X 2 = 2000 pulses /rev of the screw X 5 TPI = 10,000 pulses/inch of table movement. At 45,000 pulses/sec, this system could operate at up to 4.5 inches/sec X 60 = 270IPM.

The Gecko G340 has a pulse multiplier, and Rutex has a multiplier of 1, 4, 10 and 20. This has the effect of moving X pulses for every pulse into the drive (from the PC). In my first example with a count of 100,000 pulses/inch would effectively become 10,000 pulses/inch (as in the second example) by setting the pulse multiplier to 10. The trade off is speed for resolution.

Routers and there size usually need high rapid speeds to be effecient. Try to figure out what rapid speed you want to run your table at and buy your screws, servos etc.. based on what is required to get your desired speed using calculations just like the above, but in the reverse order.

Consider what you want from your design. You may have to use your faster PC to run Mach2 at 45khz. Good luck.

[ger21]

The current testing versions of Mach2 are looking like they will require 500Mhz minumum CPU's. Also, you need to be running either XP or Win2K. You might want to consider using TurboCNC, but it must be run in DOS, not from a Win98 DOS prompt.

Another thing to consider is that some laptops parralel ports can't output enough voltage to run your drivers, so you may be out of luck with the laptop anyway. Both Mach2 and TurboCNC can be downloaded and tried before purchase, to see if they'll work with your laptop.

[Splint]

Isn't communication software known as DNC? What's the difference between CNC and NC software?
Splint

[HuFlungDung]

DNC may be a function of communications software. Uploading a program to the cnc memory is an example of regular comm function.

Drip feeding a program line by line from a PC to the CNC for immediate execution is what DNC is all about.

[Rekd]

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..

%
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.

[Al_The_Man]

Typically there is four stages in Cad/Cam to machine. First there is the CAD to draw the part up, second, CAM usually allows you to draw/enter the tool paths and supply tooling information etc then third to convert to G code you need to pass it through a post-processor (usually an extension of the CAM s/w) which has all the options that your particular machine might have, including unique M codes or ways of interpreting G codes etc such as circular interpolation methods. Fourth is the DNC program that sends it out the (serial) port to the machine e.g. http:www.cadem.com/.
Some programs have all the above options in one piece of s/w.
AL

[ger21]

Samault, be aware that if your using Mach2 or TurboCNC, then none of the above (what Rek'd said) is really necessary.

[samualt]

ger21:
"Another thing to consider is that some laptops parralel ports can't output enough voltage to run your drivers, so you may be out of luck with the laptop anyway."

Egads! Can anyone here recommend a laptop brand which seems to work for CNC? That is, sending the g-code to the hardware driver? Any particular model you have had luck with?

[imserv]

Egads! Can anyone here recommend a laptop brand which seems to work for CNC? That is, sending the g-code to the hardware driver? Any particular model you have had luck with?

If you switch your controller to DeskCNC, you can use either a serial or USB port. Then any 200 mhz or so laptop that will run Win 98 or later OS, will work fine at over 40000 sps (soon to be 125k).

Fred Smith - IMService
http://www.cadcamcadcam.com

[drawbar]

I use my Dell Dimension laptop to drive my CNC machine I built. I run TurboCNC through bipolar chopper boards I built myself around the ST L6208N chips. No optoisolators. Works great so far!

Brian

[samualt]

Well, I just bought a ECS 14.1" Notebook Computer with an AMD Athlon XP-M 1600+ with lots of built-in cool stuff including Wifi (wireless networking). It will just have to work with CNC! I will make it work if by nothing more than pure will-power!
BTW, they have those on sale at Walmart Online - ECS Special Buy for just 598 + state tax + 7 shipping. Not a bad deal for what you get and a 12 month warranty.
Now I'm off to Ebay to pick up a cheap Wifi router (for wireless network) and I'll be set. Wires? We don't need no stinking wires!
:banana:

The above runs WinXP and is much faster than the Mach2 requirements. I think I will download the demo of it and some others and see which works best. I'll keep my fingers crossed...

[Egar Twins]

usually the cam program I have worked with have a comm program integrated direectly into the CAM...Now this might be the integration of two distinct systems...but I have never seen them seperate...I believe MasterCAM has a COM program directly integrated as well....also something to think about...if your numeric controller possesses COM ports (rs232 format) you can use a regular serial cable with no line driver hardware directly from your laptop at distances of less then 60 feet(although I have done it at distances of up to 100 with no prob..

[ViperTX]

DNC is distributed numerical control.....which basically means that you have a network way to distribute CNC / NC software to either CNC or NC machines.

[Al_The_Man]

Actually the term DNC has now two meaning attached to it 'Distributed Numerical control' and 'Direct Numerical Control' The former is the networking distribution of Part programs and the latter has come to mean the drip feed of part programs to a machine that is unable to store the complete program in memory.
Al.