Need Help!- New to C.N.C. code

[Gerald Sande]

I have a very basic question when writing a C.N.C. program, let's say drilling one .500hole in a part .100 deep. X=0 and Y=0. I'm trying to get a understanding in referencing the part "fixture"and tool compensation reference. How ? and what reacts with what? I have a tool compensation of -11.250, that's from the top of the tool holder to the bottom of the drill. I placed that into DT. I also jogged the "Z" with the tool holder, chuck and drill in the spindle to the fixture "0" point or .100 above the part. This number is -7.150. I placed that into DF. I removed the drill from the tool holder "about 4" long" and run the program without the part and my chuck ends up about 3" above the bed and moves .100 down. I need a better understanding of the basics. When you put a E1 or H1 in a program, what table does it look at. I think H1 looks at the DT table and if it does, I don't have a understanding in measuring the "0" point of either the fixture, "part" or tool "0". I realize these a very basic questions, but I would like to get a foot hold in working with a C.N.C. I have a Fadal 4020HT.
Simple program
N1 o358(drill hole
N2 T1 M6
N3 G0 G90 S400 M3 X0. Y0.
N4 H1 D1 M8 Z-.1
N5 G98 M30
Thanks Jerry

[dpark1]

The H is your tool length offset(the distance from machine zero to the top of your part with any given tool in Z) The E is your fixture offset(also the same as G54,G55,etc....) So if you wanted to save a x0 y0 position that you are already at you would goto eg setup-fixture-select fixture and locator diameter-fixture 1 for E1,and 0 for locator diameter- set x and y) then in your program use E1 x0 y0 and it will use what you set and also use H for the tool you set and it will pick-up the tools offset.You do not need D in a drill program, and use a g81 for spot drilling or g83 for peck drilling, then a g80 to cancel drilling operations.

N1 O358 ( DRILL )
N2G20
N3G0G17G40G80G90
N4 ( CENTERDRILL )
N5T1M6
N6G0G90S1200M3E1 X0 Y0
N7H1Z1.M8
N8G81G98X0Y0Z-.1R0.1F4.
N9G80
N10M5M9
N11G90H0Z0.
N12E0X0Y0
N13M30

[carbidecraters]

Here is how I would do it

M6T1
M3S800
G0X0Y0
Z.1H1M8
G1Z-.1F6.
G0Z.1
M5M9
Z0H0
M30

[Gerald Sande]

Thanks for the information. I'll work with it this coming week. I've been waiting on the chiller pump and it should be here today. After I make sure the spindle coolant system is working and a few other problems, I'll get to the basic programming. I put together a CAD/CAM computer using Turbo CAD/CAM version 11, but I need to understand the basic code first. I do have a spindle air leak to look into, but my Fadal VMC 4020HT has been minding it's manners when chucking in the tool holder lately. It's dropped the tool holder twice. Jerry

[SDK73]

Hi Jerry,

I myself work on Fadals too, if you are on your program edit page, you can hit the "F" for functions then type in all your information, they have everything on that page, from drilling to milling, to math. Fadals are probably the easiest CNC to program, IMHO, make sure that when you do set your x and y axis that you actually got through the proper set fixture pages, I would not suggest to type SET X0 and SET Y0, this is how you would set your cold start positions. Also fyi M7 for thru coolant, check your spindle filter prior to running it. Good Luck !!!

[fizzissist]

As fine the answers you can get here are, there's no substitute for having the manuals....

Someone here posted a link for the Fadal manuals that should have everything you need for programming...

http://www.compumachine.com/Support/DL-Fadal.htm#User

The 'User' manual has all the coding.

Don't know Fadal's current policy, but I'd think if you schmoozed Neal he might give you the contact info to get the manual on CD (most handy....I have it on all my computers for quick access).

I use Format 1 exclusively, and it does everything I need it to do....and a lot more. I'd also recommend it for just starting out and getting your feet wet.

One thing I've done is put together a small "library of operations" in a single Notepad .txt file. I just open it up alongside a bland Notepad file, and copy/paste the operations I need, then edit to suit the part. For basic parts, it's quick and easy. (when done, just rename the file without the extension to load into the control)

For advanced stuff, you'll want to configure the post on your Turbocad to minimize editing....for that you'll really need the manual to know how the Fadal likes it's code seasoned and what it will swallow.

If you'd like, I'll post my 'library' for you when I get to work Monday.

[Neal]

If you go to www.fadal.com you can down load any of the manuals in PDF form. Select service then Documentation Support and fill the registration form then log in anytime you wish. Manuals for Operators, maintenance, and installation are there for the Fanuc control, Fadal control, and Siemens controls.

Neal

[ImanCarrot]

One small detail: you're drilling through 0.1 (I assume inches). The drill you use should have a large included angle so that the edges of the drill engage the material before the tip of the drill breaks through.

Otherwise you'll get chatter and vibration.

Just a little tip!

[Gerald Sande]

Thanks for your information, After fixing a couple coolant leaks, I finally have 1 4020HT up and running, so I can work with the C.N.C. programming code. I successfully made a simple program to drill two different size holes in two different locations. Jerry

[Joe S.]

Hi Jerry,
tool offsets in the Fadal, I work with operate as follows:
G43 tells the machine to use length offsets from the tool table, H1 would tell it to use offset 1 for tool 1, so the code block : G43Z1.0H1 will send the cutter to 1.000 above the top of part.
G41 in conjunction with D1 will offset the cutter to the left of the programmed path by 1/2 the diameter defined in the tool table for tool 1. G42 will offset the cutter to the right, and G40 cancels all tool offsets,(right and left assume clockwise rotation ). I would suggest you wait until you feel proficient in G CODE before venturing into using G41 and G42 unless you just have to. It can really do some strange things.
G43 is a must use offset however, instead of using DT to set your tools try UT and follow the directions.
your sample program:

N1 O358         (drill hole... O should be CAPITAL LETTER) 
N2 G90 G17 G20 G40 G80 
N3 T1 M6        ( CHANGE TO TOOL 1)
N3 S400 M3      ( SPINDLE ON CLOCKWISE)
N4 G0X0.Y0.E1   ( RAPID TO PART X0 Y0 )
N5 G43 H1 Z1.0  ( RAPID Z TO 1" ABOVE PART)
N6 Z0.1         ( RAPID TO .1 ABOVE PART)
N7 G1Z-.1F2.0   ( FEED DRILL INTO PART .1 AT 2 IPM)
N8 G91G28Z0     ( RETURN Z AXIS TO Z 0, MACHINE 0)
N9 G91G28X0Y0   ( RETURN X AND Y AXIS TO MACHINE ZERO)
N10 M5          ( TURN OFF SPINDLE)
N11 M9          ( TURN OFF COOLANT)
N12 M30         ( END OF FILE - REWIND)

[carbidecraters]

Originally Posted by Joe S. Hi Jerry, tool offsets in the Fadal, I work with operate as follows: G43 tells the machine to use length offsets from the tool table, H1 would tell it to use offset 1 for tool 1, so the code block : G43Z1.0H1 will send the cutter to 1.000 above the top of part. G41 in conjunction with D1 will offset the cutter to the left of the programmed path by 1/2 the diameter defined in the tool table for tool 1. G42 will offset the cutter to the right, and G40 cancels all tool offsets,(right and left assume clockwise rotation ). I would suggest you wait until you feel proficient in G CODE before venturing into using G41 and G42 unless you just have to. It can really do some strange things. G43 is a must use offset however, instead of using DT to set your tools try UT and follow the directions. your sample program: N1 O358 (drill hole... O should be CAPITAL LETTER) N2 G90 G17 G20 G40 G80 N3 T1 M6 ( CHANGE TO TOOL 1) N3 S400 M3 ( SPINDLE ON CLOCKWISE) N4 G0X0.Y0.E1 ( RAPID TO PART X0 Y0 ) N5 G43 H1 Z1.0 ( RAPID Z TO 1" ABOVE PART) N6 Z0.1 ( RAPID TO .1 ABOVE PART) N7 G1Z-.1F2.0 ( FEED DRILL INTO PART .1 AT 2 IPM) N8 G91G28Z0 ( RETURN Z AXIS TO Z 0, MACHINE 0) N9 G91G28X0Y0 ( RETURN X AND Y AXIS TO MACHINE ZERO) N10 M5 ( TURN OFF SPINDLE) N11 M9 ( TURN OFF COOLANT) N12 M30 ( END OF FILE - REWIND)

I am curious what version of control you are using. In 15 years of programming I have never used a G43 or G28. I think you may be over complicating the program. Like posted above this has done the job just ifne for us for years.

M6T1
M3S800
G0X0Y0
Z.1H1M8
G1Z-.1F6.
G0Z.1
M5M9
Z0H0
M30

[DareBee]

Definitely many slight variations that work.
I never use G43 code with my H either, but I do use the G28.