I have 395 holes to tap, I have a reversing tapping head, the reverse speed is twice as fast as the spindle rpm.

I can very closely match the z feed to the 10-24 pitch tap needed to feed down into the hole, but I need to retract at twice the infeed rate.

All the drilling cycles rapid back. The drag boring cycle will only feed back out at the infeed rate.

Is there an easy way to create a macro or subroutine call I can place in my Mach2 post  proccesor that I use through VisualCam to give me twice the feed rate out over the infeed rate?

Thanks for the insight

jh

Hi JH,

are all the holes in the same part?

are the holes in a regular pattern?

if so you could use a sub program

let me have more detail about the hole pattern and pitches and I will look at it for you.

Graham.

Graham and I are about the same on this one

This is how I would do it....

S300 M3
M8
G00 G43 H3 Z1.00
G00 X1.0 Y2.0
M98 P1000
X2
M98 P1000
X3
M98P1000
M30


O1000
G01 F40 Z-.5
G01 F80 Z1.00
G04 P1.0
G00
M99

they are all 10-24's on .5" centers.   31 collums   20 rows

I'm wondering how to get my VisualMill 5 program to insert the P1000 line of code after every x-y move, or which wizard to use I guess?

it looks like the subroutine takes over between x-y moves?

S300 M3                      spindle 300 prm rotate cw
M8                              flood on
G00 G43 H3 Z1.00         rapid move, apply tool offset, tool offset index, +z 1.0" from work
G00 X1.0 Y2.0               rapid move, to x1" and y2"
M98 P1000                   call subroutine P1000
X2                               move to x2" i think
M98 P1000                   call subroutine P1000
X3                               move to x3" i think
M98P1000                    call subroutine P1000
M30                            program end and rewind


O1000                         subroutine name "where should this be text located, at the top or bottom of the main program string "
G01 F40 Z-.5                lineriar interpolation, feedrate 40"per min, to Z -.5" this sends the tap in at a matching thread per rev basicaly
G01 F80 Z1.00               lineriar interpolation, feedrate 80"per min, to Z 1" this sends the tap out at twice thread per rev basicaly to _ __ __                               match  the double reverse gearing speed of the tap head
G04 P1.0                      dwell time of 1 second at the 300 rpm to give the tap head a chance to completely withdraw
G00                             set to rapid travel
M99                            return from subroutine back to main program giving up machine control to main program which begins the next _           _                               move command

does this explain the situation? My minimum rpm is 351 so 351/24=14.625 imp feed rate to match 24tpi, how does this all sound.


jh

Sounds to me like you are ready to make some chips

Put the sub at the end of the program...

Good luck.

I think so, but,

now the next hurdle is to get the CAM software to write all the sub calls in the right place 390+ times

any clues here?  thanks for the advice so far, I feel I'm about ready to make tapping chips.

jh

Hi JH,

this is how I would do a rectangular pattern of holes. By changing the "L" numbers any number of rows can be done.

I hope this is what you want, no charge ;-)

Graham.


G20 G40 (standard setup lines)
S300 M3
M8
G00 G43 H3 Z1.00
G00 X0 Y0    (set position of first hole as X0 Y0)
M98 P1000 L19 (repeat 19 times)
M30

O1000
(this bit moves Y axis)
M98 P1001 L30 (repeat 30 times)
G91 (set to move incremental)
G00 Y-.5 (do move of .5 inch)
G90 X0 (set to absolute and go back to start of line)
M99

O1001
(this bit moves X axis)
M98 P1002 (tap hole)
G91 (set to incremental)
G00 X-.5 (do move of .5 inch)
G90 (back to absolute)
M99

O1002
(this bit taps hole)
G01 Z-.25 F14.625
Z1. F29.25 (remove this line to drill holes and change feed and depth)
M99

Thanks Graham,

I dug into the post generator in VisualMill 5 for the Mach2 controler.

under the cycles tab it lists the variables associated with tapping in this case. As such I'm able to deleate the vairables associated with tappnig leaving the x-y move calls. Then I just added the M98 P1000 text

Now when i post using the tap tool, it generates all the x & y's with the M09 P1000 call under each! great, but it still is leaving the G84 call which right now I'm just doing a search and replace in notepad to elliminate this code. I works great.

But, I put the sub routine at the end as suggested just before the M05 and M30 and it works fine until after the last x-y tapped hole is done, then the controller reads the sub as another line and exicutes it one last time in the same/last x-y position. I can't see where to put the sub without it running one last time. Any where else it doesn't work properly with the rest of the code. i thought the sub would not be read unless there was a M98 call?

this is what I have been testing

G20
G0 G17 G40 G49   G90
G61(CONSTANT CONTOUR OFF OR TURN ON W/G64)
(Clockwise tap operation)
M08
T7 M988 M6
G43 0
S+351 M03
G00 Z+.5000
X+4.0000 Y-2.0000
m98 p1000
G00 Z+.5000
X+4.5000 Y-2.0000
m98 p1000
G00 Z+.5000
X+5.0000 Y-2.0000
m98 p1000
G00 Z+.5000
X+5.5000 Y-2.0000
m98 p1000
G00 Z+.5000
X+6.0000 Y-2.0000
m98 p1000
G00 Z+.5000
X+6.5000 Y-2.0000
m98 p1000
G00 Z+.5000


O1000
G01 F14.60 Z-.5
G01 F29.2 Z1.00
G04 P2.0
G00
M99

M05
M30

Hi JH,

try it like this

Graham

G20
G0 G17 G40 G49   G90
G61(CONSTANT CONTOUR OFF OR TURN ON W/G64)
(Clockwise tap operation)
M08
T7 M988 M6
G43 0
S+351 M03
G00 Z+.5000
X+4.0000 Y-2.0000
m98 p1000
G00 Z+.5000
X+4.5000 Y-2.0000
m98 p1000
G00 Z+.5000
X+5.0000 Y-2.0000
m98 p1000
G00 Z+.5000
X+5.5000 Y-2.0000
m98 p1000
G00 Z+.5000
X+6.0000 Y-2.0000
m98 p1000
G00 Z+.5000
X+6.5000 Y-2.0000
m98 p1000
G00 Z+.5000
M05
M30

O1000
G01 F14.60 Z-.5
G01 F29.2 Z1.00
G04 P2.0
G00
M99

Graham that was an excellant example of the L par use. I had to look it up again myself. Peter Smid (CNC programming Handbook) wrote of it, using only 25 lines of code to drill 100,000,000 holes.  Thanks For the reminder  Terry