Drilling in X axis with live-tool

[philrace34]

Hello ., I own a daewoo puma 230 msb with controller fanuc 18i, is there any G code for drilling in X axis with the live tooling or I have to program it in G01 ? I am looking for a G code like G81 or G83 but for the X axis , I have been trying G87 but I have an alarm G-code error Okk thank

[dcoupar]

G87 is X-axis drilling, G88 is X-axis tapping.

Please post the section of your program where the alarm occurs and the alarm number.

[CNCRim]

what is your control? Daewoo has it own control I don't think it has Fanuc..... I had never worked with Daewoo before, but one time I read their program manual and from what I remember, can cycle for Daewoo is difference then Fanuc, so check your manual.

[dcoupar]

According to his post, it's an 18i. Daewoo currently uses Fanuc controls, they used to put Mitsubishi on some of the machines. AFAIK, they never had their own control.

[philrace34]

hi thanks for the help , Yes my controller is a FANUC 18i-t year around 2001
I have try G87 and dont work ,

my featurecam program the block like that

M33S2000G0G54G98:
G0X2.0Z-1.0:
G87U-0.200R0F5.0
G28U0W0

I have try change the U-0.200 by X-.200 and X .200 but always the same result , it says Improper G-code 010 , even when I just type G87 in mdi mode I end up with this I think its maybe a parameter that is wrong or this fanuc dont have the option of drilling in the X axis ,
ok if someone have an idea let me know thanks !

[dcoupar]

You might need a C-axis command in the G87 line. Also, a G00 in the G28 line.

[g-codeguy]

This is a sample that came in the Daewoo MS200 we bought.

:3456 (RADIAL DRILL)

G0G40G80
G50S1500
M35
G0T0606
G97S500M33
G54Z.1C0.
Z-.5
X6.0
G98G87X3.5Q2500F20.H45.K8M89
G0G80X6.0
Z.1M35
G28U0.
G28W0.
M30

Another drilling example in the control upon purchase.


:2345 (SAMPLE AXIAL DRILL)

G0G40G80
G50S1500
M35
G0T0404
G97S500M33
G54Z.1C0.
X3.0
G98G83Z-1.0Q2500F20.H90.K4M89
G0G80Z.1
G99
G28U0.M35
G28W0.H0.
M30


How I program an axial drill.


N1000G54M91 (LIVE SPOT DRILL)
M35
T1010M8
S300M33
G98X1.874Z.5C0
Z-.425S5000
G83Z-.55Q3000F20.H90.K4M88
G0Z.5M35
M90
M91
M1


Not sure if I have a sample of the G87 used in one of my programs. I normaly use G1 as I seldom use a spot drill unless also tapping. Thus I feed very slowly until the drill point is into the material before kicking up the feedrate. Can't do that with a G87 cycle unless you want to run it twice.

M88= low pressure clamp, M89= high pressure clamp, M90 cancel clamp pressure on our lathes. Don't know if the M35s are necessary. I do know that we have to start the live tooling at S300, make a move & then kick RPM to desired level as the tool doesn't always catch and alarms out if started much faster.

EDIT: Not sure if the samples that were in the control upon purchase are 100% correct. I don't see an M90 to cancel the high pressure clamp.

[dcoupar]

What is the serial number of your machine?

[phx]

hi philrace

can u try this?

T202
G97 ;U/min
G98 ;Feed per min
M33 S2000
G28 H0
G0 x30 Z20
Z-10
G87 X0 F100 Q2000 R0
G0 X50
Z20
X200 Z200
M30

@dcoupar
can it be that G87 ist an Option and he do not have it?

[dcoupar]

That's why I asked for the serial number. AFAIK, if you get milling on a Puma, you get canned cycles.