CNC G-code wants

There's no tricks to programming. But there is tricks to setups. Here's one... Lets say you hava a big semi flat area to machine. Because of corner radii or angular floors you are forced to use a ball mill. Tilt the thing on a sine plate, say 5 or 10 degrees. Now you will be cutting on the ball as opposed to the tip, quadrupling cutter life and greatly increasing surface finish. Bore a hole somewhere to draw on your cam proggy for pickup.

Programming tricks...hmmmm maybe x and z shifts on a lathe? Maybe doing math like picking up an arc with 3 points? Or using cutter load in programming, or adding music to the end of programs using beeps or blinking lights? be specific?

Ok Vinny here goes

Let say we are going to make a plate flat on top then drill 4 holes, then countersink each of them.

[ a practical version or altered version of a 4 hole domino. ]

What is the brute force way ? What is the smart to be expanded upon way ? What is the smart way to do it with nominal issue to expand?

Not everyone is a master of all CNC programing code or G-code as some say.

I'm just starting - I do CAD and CAM and CAD-CAM most any day and have done it for a while with 10 and 15 mil endmills.

Martin

Mart> On-Topic

Martin K.

Probably manual programming at the control.

Probably programming in a CAM system.

Here's the code Gibbs spits out for a Fadal. From startup screen to posting the code took 9 min. 36 sec. That's drawing the geometry, choosing tools, selecting the processes. I must be slipping (I did have a couple of false starts), I didn't think it would take over 5 mins.

That's face milling the surface with a 3" inserted face mill. Spotting the holes with a .375 90 degree spot drill, to leave a .275 chamfer diameter. Drilling the holes .250 dia X .600 deep. Assuming the plate to be .500 thick after facing.

============================================================ % N1O1*PLATE.NCF N2* FORMAT: CNCVIS1 [M8] M756.15.1.PST N3* 2/23/09 AT 8:26 PM N4* OUTPUT IN ABSOLUTE INCHES N5* PARTS PROGRAMMED: 1 N6* FIRST TOOL NOT IN SPINDLE N7T1M6 N8* OPERATION 1: ROUGHING N9* WORKGROUP001 N10* TOOL 1: 3. FACE ENDMILL N11S10000M3 N12G17G90G0X3.472Y1.8333E1 N13Z1.H1M8 N14Z.1 N15G1Z0.F200. N16G8 N17X-1.5 N18Y.6667 N19X1.5 N20Y-.5 N21X-3.5 N22G0Z1. N23G0G90M5M9 N24G53Z0 N25M1 N26T2M6 N27* OPERATION 2: HOLES N28* WORKGROUP001 N29* TOOL 2: .375 SPOT DRILL N30S7500M3 N31G17G90G0X0.Y1.E1 N32Z1.H2M8 N33M46 N34Z.1 N35G81G99X0.Y1.Z.0875R0.1F40. N36X1.Y0. N37X0.Y-1. N38X-1.Y0. N39M47 N40G0G80Z1. N41G0G90M5M9 N42G53Z0 N43M1 N44T3M6 N45* OPERATION 3: HOLES N46* WORKGROUP001 N47* TOOL 3: .25 DRILL N48S7500M3 N49G17G90G0X0.Y1.E1 N50Z1.H3M8 N51M46 N52Z.1 N53G83G99X0.Y1.Z-.6518R0.1Q.25F40. N54X1.Y0. N55X0.Y-1. N56X-1.Y0. N57M47 N58G0G80Z1. N59G0G90M5M9 N60G53Z0 N61X0Y0Z0E0H0 N62M30 % ============================================================

Oops. Forgot the minus sign on my spot drill. Should have been -.462 on the depth. I would have caught that if I had rendered it, but shortcuts, ya know. LOL

Face mill, drill, c'sink.

Facemill, integrated drill-c'sink.

Semifinish facemill, integrated, drill-c'sink, finish facemill. The trick here is you now have a perfectly flat face that's not affected by any mushrooming that might occur with tool wear.

I bring this up since I am assuming there are 10 other shops within 3 miles that can do it just as fast and just as cheap. It's never about the code or the control.

-- Bill

I had that happen to me few times. Did not want to waist time rendering (specially if it took few minutes) and it cost me dearly. I have a bad habit of finishing pockets bottoms by cheating with the depth value. Say pocket is roughed out 0.99" deep I finish by telling Gibbs to start at 0.9" and finish at 1.00" in 2 cuts. The problem is if there is a rad on my tool. Than Gibbs compensates to whatever dia at

0.005" or 0.01" from cutters end. I try now to make it a point to render even simplest of programs. Jerry

Jerry:

Yeah, I ALWAYS render when making parts, it catches a lot of simple boo-boos. But for a newsgroup posting that no-one would ever use I just left it out, both times. Double Oops. I drew and programmed the whole thing over from scratch in 5 min. 41 sec. put the holes in a different location AND rendered it. Corrected code is below. I will say the exercise was informative in that it showed me how quickly you can lose your edge in just 4 months of non-use of a CAM system. But it comes back pretty quick.

=================================================== % N1O1*PLATE 2.NCF N2* FORMAT: CNCVIS1 [M8] M756.15.1.PST N3* 2/23/09 AT 10:56 PM N4* OUTPUT IN ABSOLUTE INCHES N5* PARTS PROGRAMMED: 1 N6* FIRST TOOL NOT IN SPINDLE N7L0100 N8* SUB NUMBER: 1 N9Y-.7071 N10X-.7071 N11Y.7071 N12M17 N13M30 N14T1M6 N15* OPERATION 1: ROUGHING N16* WORKGROUP001 N17* TOOL 1: 3. FACE ENDMILL N18S10000M3 N19G17G90G0X3.472Y1.8333E1 N20Z1.H1M8 N21Z.1 N22G1Z0.F200. N23G8 N24X-1.5 N25Y.6667 N26X1.5 N27Y-.5 N28X-3.5 N29G0Z1. N30G0G90M5M9 N31G53Z0 N32M1 N33T2M6 N34* OPERATION 2: HOLES N35* WORKGROUP001 N36* TOOL 2: .375 SPOT DRILL N37S7500M3 N38G17G90G0X.7071Y.7071E1 N39Z1.H2M8 N40M46 N41Z.1 N42G81G99X.7071Y.7071Z-.1375R0.1F40. N43L0101 N44M47 N45G0G80Z1. N46G0G90M5M9 N47G53Z0 N48M1 N49T3M6 N50* OPERATION 3: HOLES N51* WORKGROUP001 N52* TOOL 3: .25 DRILL N53S7500M3 N54G17G90G0X.7071Y.7071E1 N55Z1.H3M8 N56M46 N57Z.1 N58G83G99X.7071Y.7071Z-.6518R0.1Q.25F40. N59L0101 N60M47 N61G0G80Z1. N62G0G90M5M9 N63G53Z0 N64X0Y0Z0E0H0 N65M30 % ===================================================

Thanks!

I have code to verify my code and another. So somewhere I learn more and more.

Wish I had a mill in the shop. Someday I will. Just have to make more room and more big bucks!

Mart>