Fadal riged tapping and the default posts any one using

[Jayson Kramer]

I was wondering if any of you are using the default Fadal format 1 and format 2 posts for your Fadal's and do ridged taping and the cycles seem correct?

 

Thanks

[Colin Gilchrist]

Hi Jay,

 

Have you read through the options in the headers of each post? I have just recently done some rigid tapping on a Fadal. We used Format 2. Did you look in the cycle drop down list and pick the Rigid Tapping cycle, and not just the normal "tap" cycle?

 

Here is code I got for a 1/4-20 tap. It looks pretty good to me...

 

N106 G0 G17 G20 G40 G80 G90
N108 T1 M6
N110 G0 G90 S1000.2 M5 M90 E1 X1.0683 Y-2.852
N112 H1 Z10.
N114 G84.1 G99 X1.0683 Y-2.852 Z-.5 R010. S1000.2 F50.
N116 X3.6283 Y-2.839 S1000
N118 G80
N120 G91 G28 Z0.
N124 G90 X0 Y0 E0
N126 M30

[Colin Gilchrist]

N180 T1 M6
N200 G0 G90 S1000.2 M5 M90 E1 X1.0683 Y-2.852
N210 G84.2
N220 H1 Z10.
N230 G84.1 G99 X1.0683 Y-2.852 Z-.5 R010. F1000. Q.05
N240 X3.6283 Y-2.839
N250 G80
N260 M5
N270 G90 H0 Z0.
N280 E0 X0 Y0
N290 M2

 

That was the same two holes, done with Format 1. I selected the "Rigid Tap" cycle.

[Jayson Kramer]

Thanks Colin. I thought we got G54 on format 2 and E1 on format 1 and this helps on the formats for the rigid taping.

[greenxman]

the second post colin sent is right. run it every day just watch your rpm over 1000 its a fadal no mill tap cnc it will do it but can't say thread will be good.

[BBprecise]

It'll work. We have 2 Fadals left of the 5 that we've had (1 has a Fanuc 18i the others had Fadal CNC controls which we ran in format 1). We only use rigid tapping because we don't use tension/compression holders and we do it all the time. My code is slightly different (I turn the spindle on at the beginning of the tool and I don't output the G84.2) G84.2 is prep cycle and isn't really needed as the machine will sync the spindle before it starts the 1st hole. A "P" in the tap cycle line controls the speed coming out. P100 is 100%, P150 is 150% and so on. We don't tap over 1000 rpm's, but the machine taps fine at 1000.

[Jayson Kramer]

Thanks guys. BB do you a G84 instead of a G84.2?

[BBprecise]

Jay, we use the G84.1 right where it's shown in Colins example. We don't output the G84.2 after the tool change. Our code would look like this except we don't have spaces between values:

 

N180 T1 M6 (TOOL DESCRIPTION)

N200 M3S1000.2

N220 G0 G90 E1 X1.0683 Y-2.852

N220 H1 Z10. M8 (IF COOLANT IS USED IF NOT WE HAVE AN M0 AFTER TOOL CHANGE TELLING OPERATOR TO USE CUTTING OIL)

N230 G84.1 G98 X1.0683 Y-2.852 Z-.5 R010. S100.2 F10.

N240 X3.6283 Y-2.839

N250 G80

N260 M5 M9 (MY POST OUTPUT THIS REGARDLESS IF COOLANT IS ON OR NOT)

N270 G0 G90 H0 Z0.

N280 G0 G90 E0 X0 Y0

N290 M2