Hi Neil,
not sure if the picture showed up. I am sure what code I am using. I fimd my enges then calculate to put my holes in the right place. On my screen the center of my hole is X-4.7540, Y-1.9090,Z-0.5000. I am going to use a 1" Dia. x 3.0000" cutter to make a hole 1.3750" Dia. x 2.125" deep.
Rick
Odd. Your pic showed up the first time I viewed it, but not now. No matter- your screen shows Heidenhain conversational.
I'm assuming from the screen that you've gotten through the startup and homing procedures OK.
I'll prob give you too much info here. I'm not intentionally insulting your level of knowledge or your intelligence, just trying to be sure you've got it all and erring on the side of redundant.
See the second page in the manual entitled "operating panel" to locate and identify some of the mode buttons, see also beginning of page E7 "operating modes and screen displays" for the rest of them.
....is X-4.7540, Y-1.9090,Z-0.5000. I am going to use a 1" Dia. x 3.0000" cutter to make a hole 1.3750" Dia. x 2.125" deep.
I'll use your x and y coordinates, but your z number is dangerous, IMO. I'll use the top of the part as Z0 and .050 as clearance.
Before programming, find your edges and enter your reference coordinates, using the end of the endmill to set your Z reference at 0. Shout if you need help here, but this has to be done first.
Start programming by pressing the programming and editing (PROG) mode button.
Press the "PGM NR" button. In the highlighted line after "program number" enter whatever numbers you like. (I use the date (120518) and keep a notebook with an index of the numbers in front and setup sheets following. Once you get ten or so programs, you'll need to be able to keep track of them and the 151 has no place for comments, AFAIK.)
Press ENT
Press NO ENT to use inch dimensions
Press TOOL DEF
Press 1, ENT, key in 3.000, ENT, .500, ENT. (You've defined the tool dimensions for the control.)
Press TOOL CALL, 1, ENT, Z, ENT.
Key in your spindle speed, whatever's appropriate for carbide or HSS. (If you have a DC spindle, this entry controls spindle speed. If you have the AC spindle, like me, with air powered speed change, entering the rpm does nothing but keep a record. 500 is the lowest possible speed in high range. Low range is noisy (er!) so I don't use it unless absolutely necessary. )
Press ENT
Press the gray button marked L. (For linear move)
Key in target coordinates X-5 Y1. (Or where ever you want the tool to park between parts. Be sure the tool isn't gonna hit something at its height the first time it moves to this position.)
Press ENT
Press NO ENT for Tool radius (cutter) comp
Enter 3999 in the box marked F (for feed. This is a rapid move, 3999 is the fastest rate the 151 will accept, and the 3999 represents the feed rate 399.9 ipm. The decimal is implied and is one place to the left of the last digit entered. True for all feed rates on this control.)
Press ENT
In the box M, enter 3. (Clockwise spindle rotation)
Press ENT
Press L. Enter Z1
Press END block button. (Lowest right hand button on the group of numerical keypad buttons. Skips having to hit NO ENT for the feed, cutter comp and M functions every time a coordinate block is entered.)
Press L. Enter the target coordinates. X-4.7540 Y-1.9090
Press END block.
Press L. Press Z, enter .05, press END Block. (When you run this the first time, slow the feed rate way down for this block with the feed rate knob. It's headed straight for the part and if something's wrong, you're in for a crash. If it appears to stop just above the part, you're good to go and can crank the feed rate back up to 100%.)
Press CYCL DEF. (Cycle definition)
Press the arrow down button (the button just above the CYCLE DEF button) till you get to the circular pocket cycle.
Press ENT.
In the SET UP box, enter -.05. (That's the setup distance, where you've already brought the tool. It must be a negative number or the control will not accept it. Think of it as directing the spindle down from the setup position.)
Press ENT
In the depth box, enter total depth of the hole. -2.125. (Must also be a negative value.)
Press ENT
IN the PECKG box, enter your pecking depth. ( With a 1" diameter, 3" long endmill, I'd enter -.2653 for a pecking depth. Negative number required here, too. My machine's spindle isn't very stiff and has only a CAT 30 taper. Dunno what you have for a spindle- if CAT 40, increase the peck depth, obviously.
.2653 is 2.125/8 pecks, leaving .003 for the ninth (finishing) pass that'll finish the floor and also the walls. No separate finishing cycle needed. )
Press ENT
Then feed rate box for the peck speed comes up. (If it were me, I'd have drilled a 1/4" pilot hole first. Again, wimpy spindle and chips have to clear. If this were a later machine, helical interpolation would be in order, but this control doesn't have it. If you haven't drilled a pilot hole, you're on your own. At minimum, a center cutting EM and a very low pecking feed rate is required, or maybe a peck drill cycle before the pocket cycle. Chips clearance issues, again.)
Enter 50 (5 ipm. This is prob high, but when you run it the first time, just play with the feed % knob to get an acceptable feed rate, then go back after the first try/hole and edit the value.)
Press ENT
In the RADIUS box , enter .6875.
Press ENT
In the F box, enter 45. (4.5 ipm, if using carbide 4 flute EM. YMMV. This feed rate is at the center of the tool, not the periphery. Doesn't matter much here, but important in smaller diameter holes.)
Press ENT
In the DR (direction of rotation) box, enter + (toggle the +/- button) for counter clockwise. (Climb milling.)
Press ENT.
Press CYCL CALL
Press END block.
Press L. Key in Z1. (There's a rapid move coming up and I like plenty of clearance for it. You don't have to enter a feed rate here because the last move of the cycle is a rapid and feed rates are modal on this control.)
Press ENT
Press END block
Press L. Key in X-5 Y1. (Back to between-parts position.)
Press END block
Press STOP button and in the M box, key in 25. (This retracts the spindle, shuts the motor off and engages the brake, at least for the AC drive model)
Yer done programming!
I do a dry run (be sure to power the servo up for this, otherwise the poor thing will just sit there and do nothing, without giving indication of the problem) then lower the knee and do a test run in PROGRAM RUN/FULL SEQUENCE mode before cutting iron, then bring the knee back up for the real thing, keeping a hand close to the E-stop and the other on the feed rate knob.
Let us know how it goes....
Neil
.
