A572 Grade 50 Steel...!!!

[Delw]

if you have that many parts you would increase your speeds and feeds production a ton for a few hundred bucks with inserted carbide drills Like the iscar or sanvik I like sandvik cause I can run a few sizes with the same inserts.
they work good in the mill and lathe. that flat out haul butt. when I first bought one years ago I was unsure bigtime and didnt want to waste the money, now if theres a hole I have to drill and these drills can do it I am buying the drill or I already own it.
I have the sandviks down to 1/2 and up to 1 1/4 not only do they feed fast the bore is even and smooth, I dont have to worry about stringy chips plus in a lathe I can use them as a roughing boring bar if needed.
I have has some of them that I use weekly from 1997 including my 1/2" dia one that is around 2.5" long flute length.

Talk to your tooling salesman it may be very benificial.

Delw

[cterry352]

On the 3/4 endmill im going full depth of part .775, (<---plunge depth) Then just using a simple G13 with I K Q...

I being .4605 ( radius of hole already there)
K being .725 ( radius of 1.45 hole, leaving .05 to finish)
Q being .0625 which would be the (Radial DOC???)

On your end mills, what are you running for axle DOC and radial DOC?

[cterry352]

Here is the program that is running now.. This is what feature cam post.. I would like to make different drilling cycles.


%
O1504
( FEATURE CAM - HAAS VF )

( SPOT DRILL POCKET1 )
G00 G17 G20 G40
T1 M06 ( #8 COATED CENTER DRILL 0.3125 DIA. )
G54 G90 X0. Y0. S1100 M03
G43 H01 Z0.125 M08
G81 G98 Z-0.6914 R0.125 F5.5
G00 G80 Z0.125

( SPOT & CHAMFER HOLE1 )
G00 G54 G90 X0. Y2. Z0.125 S565
G81 G99 Z-0.55 R0.125 F5.5
X-1.732 Y-1.
G98 X1.7321
G00 G80 Z0.125
G53 G49 Z0. M09
M01

( DRILL HOLE1 )
G00 G17 G40
T20 M06 ( 13MM TWIST DRILL )
G54 G90 X1.7321 Y-1. S858 M03
G43 H20 Z0.125 M08
G83 G99 Z-0.9752 R0.125 Q0.200 F6.86
X-1.732
G98 X0. Y2.
G00 G80 Z0.125
G53 G49 Z0. M09
M01

( DRILL POCKET1 )
G00 G17 G40
T19 M06 ( 59/64 TWIST DRILL )
G54 G90 X0. Y0. S456 M03
G43 H19 Z0.125 M08
G83 G99 Z-1.125 R.125 Q.275 F4.56
G00 G80 Z0.125
G53 G49 Z0. M09
M01

( MILL POCKET )
G00 G17 G40
T18 M06 ( 3/4 ENDMILL )
G54 G00 G90 X0 Y0
M03 S1910
G43 Z0.125 H18 M08
G13 I0.46 K0.7375 Q0.0625 F22. Z-0.775 D18
G00 G90 Z1. M09
G53 G49 Z0. M09

( CHAMFER POCKET POCKET1 )
G00 G17 G40
T17 M06 ( 45 DEGREE CUTTER 1.0 DIA. )
G54 G90 X0. Y0. S1600 M03
G43 H17 Z0.125 M08
Z-0.305 F15.
G00 Z1.

( MILL POCKET FINISH )
G00 G17 G40
T16 M06 ( 1/2 ENDMILL )
G54 G00 G90 X0 Y0
M03 S1528
G43 Z0.125 H16 M08
G13 I0.75 F27. Z-0.825 D16
G00 G90 Z1. M09
G53 G49 Z0. M09
G53 Y0.
M30
%

[txcncman]

Let me find a Haas manual and I will look at this.

[txcncman]

Partly to refresh my memory and partly so that we are both on the same page, from the Haas mill manual:

G73 High-Speed Peck Drilling Canned Cycle (Group 09)
F Feedrate in inches (mm) per minute
I First cut depth
J Amount to reduce cutting depth for pass
K Minimum depth of cut (The control will calculate the number of
pecks)
L Number of repeats (Number of holes to drill) if G91 (Incremental
Mode) is used
P Pause at the bottom of the hole (in seconds)
Q Cut Depth (always incremental)
R Position of the R pla ne (Distance above part surface)
X X-axis location of hole
Y Y-axis location of hole
Z Position of the Z-axis at the bottom of hole
I, J, K, and Q are always positive numbers.
There are two methods to program a G73; first using the I, J, K addresses and
the second using the K and Q addresses.
If I, J, and K are specified, The first pass will cut in by the value I, each
succeeding cut will be reduced by the value of J, and the minimum cutting
depth is K. If P is specified, the tool will pause at the bottom of the hole for that
amount of time.
If K and Q are both specified, a different operating mode is selected for this
canned cycle. In this mode, the tool is returned to the R plane after the number
of passes totals up to the K amount.

G81 Drill Canned Cycle (Group 09)
F Feedrate in inches (or mm) per minute
L Number of holes to drill if G91 (Incremental Mode) is used
R Position of the R plane (position above the part)
X X-axis motion command
Y Y-axis motion command
Z Position of the Z-axis at the bottom of hole

G83 Normal Peck Drilling Canned Cycle (Group 09)
F Feedrate in inches (or mm) per minute
I Size of first cutting depth
J Amount to reduce cutting depth each pass
K Minimum depth of cut
L Number of holes if G91 (Incremental Mode) is used
P Pause at end of last peck, in seconds (Dwell)
Q Cut depth, always incremental
R Position of the R plane (position above the part)
X X-axis location of hole
Y Y-axis location of hole
Z Position of the Z-axis at the bottom of hole
If I, J, and K are specified, the first pass will cut in by the amount of I, each
succeeding cut will be reduced by amount J, and the minimum cutting depth is
K. Do not use a Q value when programming with I,J,K.
If P is specified, the tool will pause at the bottom of the hole for that amount of
time.
Setting 52 changes the way G83 works when it returns to the R plane. Usually
the R plane is set well above the cut to ensure that the peck motion allows
the chips to get out of the hole. This wastes time as the drill starts by drilling
“empty” space. If Setting 52 is set to the distance required to clear chips, the R
plane can be put much closer to the part being drilled. When the chip-clearing
move to R occurs, the Z axis distance above R is determined by this setting.

[txcncman]

G12 Circular Pocket Milling CW / G13 Circular Pocket Milling CCW
(Group 00)
These two G codes are used to mill circular shapes. They are different only in
which direction of rotation is used. Both G codes use the default XY circular
plane (G17) and imply the use of G42 (cutter compensation) for G12 and G41
for G13. These two G-codes are non-modal.
*D Tool radius or diameter selection
I Radius of first circle (or finish if no K). I value must be greater than
Tool Radius, but less than K value.
K Radius of finished circle (if specified)
L Loop count for repeating deeper cuts
Q Radius increment, or stepover (must be used with K)
F Feedrate in inches (mm) per minute
Z Depth of cut or increment
*In order to get the programmed circle diameter, the control uses the selected
D code tool size. To program tool centerline select D0.
NOTE: Specify D00 if no cutter compensation is desired. If no D is specified
in the G12/G13 block, the last commanded D value will be used, even
if it was previously canceled with a G40.
The tool must be positioned at the center of the circle using X and Y. To remove
all the material within the circle, use I and Q values less than the tool diameter
and a K value equal to the circle radius. To cut a circle radius only, use an I
value set to the radius and no K or Q value.
These G codes assume the use of cutter compensation, so a G41 or G42 is
not required in the program line. However, a D offset number, for cutter radius
or diameter, is required to adjust the circle diameter.
The following programming examples show the G12 and G13 format, as well
as the different ways these programs can be written.
Single Pass: Use I only.
Applications: One-pass counter boring; rough and finish pocketing of smaller
holes, ID cutting of O-ring grooves.
Multiple Pass: Use I, K, and Q.
Applications: Multiple-pass counter boring; rough and finish pocketing of large
holes with cutter overlap.
Multiple Z-Depth Pass: Using I only, or I, K, and Q (G91 and L may also be
used).

[cterry352]

Yes all that is correct..

[txcncman]

Now let's look at how to improve the first drilling cycle:

( DRILL HOLE1 )
G00 G17 G40
T20 M06 ( 13MM TWIST DRILL )
G54 G90 X1.7321 Y-1. S858 M03
G43 H20 Z0.125 M08
G83 G99 Z-0.9752 R0.125 Q0.200 F6.86
X-1.732
G98 X0. Y2. <<<<<<<<<Why switch to G98???
G00 G80 Z0.125
G53 G49 Z0. M09
M01

Let's try:

G73 G99 Z-0.625 R0.1 I0.25 J0.05 K0.2 F9.85
X-1.732
X0. Y2.
G80
G83 G99 Z-0.9752 R0.1 I0.775 J0.711 K0.064 F9.85
X-1.732
X1.7321 Y-1.
G80

What do you make of this?

[txcncman]

Now, let's work on the second hole:

( DRILL POCKET1 )
G00 G17 G40
T19 M06 ( 59/64 TWIST DRILL )
G54 G90 X0. Y0. S456 M03
G43 H19 Z0.125 M08
G83 G99 Z-1.125 R.125 Q.275 F4.56
G00 G80 Z0.125
G53 G49 Z0. M09
M01

Almost the same thing here:

G73 G99 Z-0.625 R0.1 I0.275 J0.05 K0.2 F6.38
G80
G83 G99 Z-1.125 R0.1 I0.825 J0.71 K0.115 F6.38
G80

Are you with me so far?

[cterry352]

Looks like a plan, i will change the program up, and run it.. But it will be about 1 to 2 hrs.. my boss just pulled me off of this job for a min.. have to run do another order of parts then switch back...

[txcncman]

Now let's look at rough milling the pocket:

( MILL POCKET )
G00 G17 G40
T18 M06 ( 3/4 ENDMILL )
G54 G00 G90 X0 Y0
M03 S1910
G43 Z0.125 H18 M08
G13 I0.46 K0.7375 Q0.0625 F22. Z-0.775 D18
G00 G90 Z1. M09
G53 G49 Z0. M09 <<<<<<Don't need M09 twice

Let's try:

G13 I0.4 K0.7375 Q0.275 F15.8 Z-0.412 L2 D18

See if you understand the changes here.

[cterry352]

And the G99 is in there because of feature cam i think... It gives you the option to rapid to the R-Plane or Z-Axis clearance. If the R-Plane is selected it puts the G99 in to Rapid to the R-Plane..

No really sure why feature cam post like that, its always adding codes, or not letting me do the right code.. Like adding a "D" to use with CC even if the CC mode is selected in the software it still does add it to the program...

And cant seem to get help from anyone or feature cam for why it post like that.. they just want more money to give you more post..