stepping into part help..

[vtecyoyo1a]

First off I'm using a Haas EC1600...I'm machining these simple parts..(just plan forming them). And I'm using the program and at the end I'm having to wait for the machine to stop then adjust the tool offset .25 inches each time (4 times total per part). Anyone able to help me make the machine step into the part on it's own?? I know there's a block of code that will do this I just don't have it...any help is welcome..and thanks!

[stevo1]

Are you turning or milling? What kind of control are you using? I would use a variable to keep adjusting the diameter/offset 4 times to work its way in.

If you were turning a part to say 10" in diameter and you were starting out at 11" adjusting in .25" everytime until you reach 10" (4 times).

#1=1.
WHILE[#1GE0]DO1
G0X[10.+#1]Z.1
G1Z-2.
G0X12.
Z.1
#1=#1-.25
END1
M30

Stevo

[vtecyoyo1a]

I'm milling .....and I'm taking .25 inches of material off on each pass...and need it to go a total of 4 passes on each part...using the same planform...thanks for the reply

[stevo1]

What type of control are you using? Can you use macro programming?

What exactly are you doing to the part? Are you just running a mill across the face .25” deep each pass or is the material being removed in the X,Y direction?

If you are milling on a face removing in the Z axis .25” each pass the same program will work with a few changes to movements and axis. Z0 is top of part and you want to remove 1” with .25” passes.

#1=0
WHILE[#1LT1]DO1
#1=#1+.25
G0X0Y0Z.1
Z-#1
G1X5.
G0Z.1
END1
M30

Stevo

[vtecyoyo1a]

I'm using a haas controller..and I'm taking material off of the out side of a part in the x and y directions...and I need to adjust the z depth 4 times to finish the part

[stevo1]

Ok I am not sure what else you need. Does this make sense to you? Do you need more explanation on how the program works? The first Z right before your machine code will be Z-.25” it will run your code then move to your starting position then drop to Z-.5” and it will run your code again. This will continue .25” increments until it reaches Z-1.”

Z0 is top of part

T()M6
G0G90G80--safe start lines
#1=0
WHILE[#1LT1]DO1
#1=#1+.25
G0G90X()Y()Z()--place your numbers to position tool
Z-#1
G1…----your machine code for your part profile goes here.
…
G0Z.1
END1
M30

Stevo

[vtecyoyo1a]

Steveo sorry man..a couple things I'm un clear about..if you have AIM or yahoo messenger I can be reached at vtecyoyo1a on aim....and vtec_the_shredi on yahoo...if you have time to explain it in real time.(sorry I'm posting this from in front of my machine on a cellphone)..if not no big deal I'll catch you around another time

[stevo1]

Thats no problem. Sorry I don't messanger or Aim. I am just about to leave for the day but will be back in tomorrow morning and Sunday. I usually check in at night from home so if you get around a computer ask all the questions you need I will try to answer when I catch them.

Stevo

[dcoupar]

Put your XY contour in a sub program and call the sub as many times as you need. This sample should mill a 2 x 4 rectangle. If you specify the D (CRC #) outside the sub, you can use the same sub with different tools.

T01 M06
G54 X-0.5 Y-0.5 S5000 M03
G43 Z0.1 H01 M08
G01 Z-0.25 F20. D1
M97 P101
Z-0.5
M97 P101
Z-0.75
M97 P101
Z-1.0
M97 P101
G00 Z5. M09
M30
N101 G01 G41 X0 F10.
Y2.0
X4.0
Y0
X-0.5
G40 Y-0.5
M99

[Geof]

Originally Posted by vtecyoyo1a ... And I'm using the program and at the end I'm having to wait for the machine to stop then adjust the tool offset .25 inches each time (4 times total per part). Anyone able to help me make the machine step into the part on it's own?? I know there's a block of code that will do this I just don't have it...any help is welcome..and thanks!

You do not need anything complicated.

Put the facing program in a subroutine and do an incremental step before each call to the subroutine. Here is an outline for program that starts facing near one corner of the part and increments down to take four 0.25" cuts for a total removal of 1":

O00000
All the normal safety stuff and comments, starting spindle etc.
G43H01 (Set tool offset)
G54 G00 X0. Y0. Z1. (move to your starting position with a bit of Z clearance)
Z0. (move Z to top of stock)
G91 G01 Z-0.25 F20. M97 P1000 L4 (increment Z and go to subroutine)
G53 G00 Z0. (retract Z)
G28 (home)
M30
----
N1000
G90 (set absolute positioning)
This is the facing sequence
M99

This sequence simply increments Z four times and calls the subroutine each time.

I just noticed dcoupar's program; the only real difference between his and mine is that I use the incremental Z and the L count on the subroutine call.

[vtecyoyo1a]

Thank you all for the replies it helps to know people care enough to stop and help, many thanks to you all

Here's the program that I am using to profile these parts:
%
O00601
N1 GOO G17 G40 G49 G80;
N2 G00 G49 G53 Z0;
N3 T10 MO6;
N4 G00 G90 G54 X6.5 Y-2.1246 A0.;
N5 S874 M03;
N6 G00 G43 H10 Z1. M88;
N7 G01 Z0. F50.;
N8 G01 G42 D10 X6.0772 F20.;
N9 G02 X4.0772 I-1. J0.;
N10 G03 X0.1985 Y4.5937 I-8.2452 J-0.2814;
N11 G03 X-0.1985 I-0.1985 J-0.3181;
N12 G03 X-4.0772 Y-2.1246 I4.3665 J-6.9997 F20.;
N13 G03 X-3.8787 Y-2.4683 I0.3749 J-0.0128 F20.;
N14 G03 X3.8787 I3.8787 J7.2813 F20.;
N15 G03 X4.0772 Y-2.1246 I-0.1763 J0.331 F20.;
N16 G02 X6.0772 I1. J0. F20.;
N17 G40 X6.5;
N18 G00 Z6. M89;
N19 M30;
%
This program is cutting into the parts at a width of .430" and each pass is .250"...into steel. Aggressive is an understatement. Today I put the wrong offset into the TLO and tried to take a .750" deep pass. By all the wincing and or giggling you all just did...I don't have to tell you a scraped the part, tool needed some clean up but its still alive (people, it was glowing red when I hit the stop button).
Which is why I want to run this program without having to tell the machine the cutter is .250" shorter on each pass. I figure the less input from me, the better things will run..
Now that you all can see the program where would the sub-routine stuff fit in. and if you could explain each block of info you are adding, I don't just want the "how" I want the "why" so I can take this lesson on to other parts.
Thanks again, John

[Geof]

This should do it. Run it in Graphics and/or with your Tool Offset raised a couple of inches above the part.

Refer to my other post for explanations.

What size is your cutter? F20. seems a bit aggresive for only 874 rpm.


%
O00601
N1 GOO G17 G40 G49 G80;
N2 G00 G49 G53 Z0;
N3 T10 MO6;
N4 G00 G90 G54 X6.5 Y-2.1246 A0.;
N5 S874 M03;
N6 G00 G43 H10 Z1. M88;
N7 G00 Z0.;
N8 G91 G01 Z-0.25 F50. M97 P1000 L4
N9 G00 Z6. M89;
N10 M30;
(------)
N1000 G90 G01 G42 D10 X6.0772 F20.;
N1001 G02 X4.0772 I-1. J0.;
N1002 G03 X0.1985 Y4.5937 I-8.2452 J-0.2814;
N1003 G03 X-0.1985 I-0.1985 J-0.3181;
N1004 G03 X-4.0772 Y-2.1246 I4.3665 J-6.9997 F20.;
N1005 G03 X-3.8787 Y-2.4683 I0.3749 J-0.0128 F20.;
N1006 G03 X3.8787 I3.8787 J7.2813 F20.;
N1007 G03 X4.0772 Y-2.1246 I-0.1763 J0.331 F20.;
N1008 G02 X6.0772 I1. J0. F20.;
N1009 G40 X6.5;
N1010 M99
%