Help

[mike cncmachine]

does any one have any info on g71 type II
i us type 1 all the time but can not get type II to cut the correct profile. i think it has to do with the tool tip and offsets i have tred tool tip 0, and 8 with no luck.
it cuts the .755 radius at .850

the program runs with no errows but will not cut the correct porfile
this is on a yang machine and fanuc ot c

any help is much need and appreciated

Mike

:9906( STEEL G71 TYPE II)
N10G00G20G40G80G96G99G50S2500
N20T0303G96S600M13
N30X4.1Z2.15
N40G71U0.025R0.1
N50G71P60Q110U0.01W0.0F0.008
N60G00X4.Z1.953
N70G01X4.Z1.7939F0.005
N80G3X3.8458Z1.6134R0.25
N90G2X3.8458Z0.5226R0.755
N100G3X4.Z0.3421R0.25
N110G01X4.Z0.183
N120G00X4.1Z2.0M09
N130M05
N140M00
N150M08
N160M03
N130G70P60Q110
N120G00X5.0M09
N130Z4.0M05
N140M3

[g-codeguy]

Where's the G41/G42? Also looking at the program I see 2 blocks with the same X value, different arc directions, and a Z value that is way out of wack. The X values could be correct, but I have no way of knowing that. I definitely can say the Z is way off.

EDIT: I also have to ask why do people keep using R.1 with something like U.025 or U.02 values for DOC? Doesn't make sense to me. You are wasting a lot of time cutting air. My standard value is R.01 no matter what the DOC is.

[mike cncmachine]

As far as I have found out g41 and g42 are not efective in a g71,72 cycle it is in g70 though. I think that the tool tip (radius offset) is added in some how my manual says the tool tip 0 and 9 are the only ones though I have tryed both with the wrong results (tool nose radius is .105)and to program cords are pulled rightout of the drawing.

[g-codeguy]

As far as I have found out g41 and g42 are not efective in a g71,72 cycle it is in g70 though. I think that the tool tip (radius offset) is added in some how my manual says the tool tip 0 and 9 are the only ones though I have tryed both with the wrong results (tool nose radius is .105)and to program cords are pulled rightout of the drawing.

I had read that about TNRC in G71/G72, but have no experience with it since I never use TNRC in my programming. Took a second look at the two blocks I said the Z was off on, & realized I must have been dozing the first time. I looked at it like I would for square corners, but it dawned on me this time that it is a more than 90 deg. arc in the part, so naturally the Z-axis move is a lot more than the R value.

You can't have an R.755 for a .755 radius arc using a .105R insert. It must be .755-.105=.65.

so the blocks should read

N80G3X3.8458Z1.6134R0.355
N90G2X3.8458Z0.5226R0.65

I am assuming the G3 radius is .250R on the print. An O.D. radius of .250 with a .105R insert would be .250+.105=.355.

You can't use the radius values from the drawing in the program when not using TNRC. You must add or subtract the tool nose radius from the print value depending on whether it is a fillet or corner radius.

This also will change your starting and ending points. 'Fraid I can't help you with those without a drawing.

Hope this helps you.