drill without spotting

[APC]

I want to create a bunch of holes in mild steel using a .108 dia. carbide drill 1/2 through. In order to prevent the drill from walking  id like to start the hole  .02 or so deep at a reduced fee to insure the drill doesn't walk ,  then drill using a method (i.j.k) or something like that.

Is there a way to force mastercam to output a drill cycle using a sub program (or routine)  long hand as we old school programmers would have done?

 

I could use something like this:

G81 G98 Z-0.02 R.O2 F2.

PATTERN

G80

G83 Z-.5 R0.02 I0.35 J0.2 K0.05 F40.

REPEAT

G80

 

BTW: (I do not have an open pot for a spotting tool)

-Thanks

[Guest]

140° Drill, self centering, thru 1 shot and done

[jeff]

If the surface is machined flat, I'd just blast the drill thru the part.  Carbide drills typically don't need spotting. 

[Guess_who]

1 hour ago, APC said:

I want to create a bunch of holes in mild steel using a .108 dia. carbide drill 1/2 through. In order to prevent the drill from walking  id like to start the hole  .02 or so deep at a reduced fee to insure the drill doesn't walk ,  then drill using a method (i.j.k) or something like that.

Is there a way to force mastercam to output a drill cycle using a sub program (or routine)  long hand as we old school programmers would have done?

 

I could use something like this:

G81 G98 Z-0.02 R.O2 F2.

PATTERN

G80

G83 Z-.5 R0.02 I0.35 J0.2 K0.05 F40.

REPEAT

G80

 

BTW: (I do not have an open pot for a spotting tool)

-Thanks

 

I usually just copy the hole pattern and paste it below the M30. Then I use a M98 Q????, which will call an N block then once it hits the M99 it will return to the line it was called from.  You'll need to make sure parameter 6005 bit 1 is enabled to use program jumps.

So my code would look like this;

O01 (PART ABC)

…usual header stuff..

G54 (RUN 1^ST )

M98 Q100

G55 (RUN 2ND )

M98 Q100

M30

 

N100 (ACTUAL PART CODE)

T1

M6

......

M99

That all being said I agree with the other posters, you probably can just get rid of the spotting.

 

[APC]

thanks for the tips! the face is not machined and flatness has been an ongoing issue thats why i was considering the subprogram

[Guess_who]

3 minutes ago, APC said:

thanks for the tips! the face is not machined and flatness has been an ongoing issue thats why i was considering the subprogram

There is a subprogram button at the bottom of the parameter - linking page

 

[APC]

i never noticed that. i dont see that as being a help. I was thinking the  actual drilling would be done in the subprogram:

Eg:

o1000 (main prog)

G0G90G54X0Y0

G43ZH1S9000M3

M98P1

X1.

M98P1

X2.

M98P1

M30

 

01

GOZ.02

G1Z-.02F2.

Z0.55F40.

G0Z.5

M99

 

[Guess_who]

Create the first OP with subprogram button selected, then copy/paste and change the tool #, parameters, etc. I think it will post what you want.

I just tried and I got this;

 

N1 T1 M6
T2
( T1 =  .125 DIA. CENTER DRILL )
( 1 )
S1000 M3
G00 G90 G53 Z26.
M11
G0 G90 G54 B-3.
B0.
M10
X-2.4591 Y.9531
G43 H1 D2 Z.1 M9
G99 G81 X-2.4591 Y.9531 Z-.02 R.1 F5.
M98 P1001
G80
M98 P8888
M01
 
N2 T2 M6
T1
( T2 =  .29 DIA. X 118. DEG DRILL )
( 2 )
S922 M3
G00 G90 G53 Z26.
M11
G0 G90 G54 B-3.
B0.
M10
X-2.4591 Y.9531
G43 H1 D2 Z.1 M9
G99 G83 X-2.4591 Y.9531 Z-1. R.1 Q.087 F4.13
M98 P1001
G80
M98 P8888
M01
M30
 
 
O1001
G91
X1.5285 Y-.036
X2.1849 Y.0899
X.3956 Y-1.9511
X-2.4906 Y-.0359
X-1.6184 Y-.09
M99
%