[1ctoolfool]

using visual quick code, when I try to run the G71 that is generated I get the following error "non monotonous PQ blocks in Z"

what is the problem?

thanks,
joev

[SeymourDumore]

Joe

Can you post a snippet of your code starting a block before the G71 call to a block after the Q block?
There are a few little things that can be wrong, and I think quick code can make a mistake ( though I have never used it)

[Geof]

It means somewhere within the P-Q block you have the Z backing up or your first Z position is ahead of your start position that is set before the G71 command.

Either post your code or a picture of what you are doing. I use G71/72/70 a lot on my TL1 and may be able to give some hints.

[1ctoolfool]

Below is the code
I used the VQC number 8, just a simple OD turn with 2 outside radius blends. Same tool for rough and finish.
.5" OD to .75" OD each .5" long.
VQC generates a G72 face rough, a G71 OD rough and G70 finish
Alarm is at the G71
thanks


%
O00300
(G71 OD W/Rounding 8)
(RghToolN = 1)
(MaxRpm = 1000)
(SpdleRpm = 1000)
(SurfSpd = 300)
(RghFeed = 0.01)
(FinToolN = 1)
(FinFeed = 0.002)
(DIA1 = 0.5)
(DIA2 = 0.75)
(Z1 = 0.5)
(Z2 = 0.5)
(R1 = 0.1)
(R2 = 0.1)
(FaceStk = 0.05)
(StkDia = 1.)
(G71 OD DOC = 0.025)
(G72 FACE DOC = 0.025)

T1
G50 S1000
G97 S1000 M03
G96 S300 M08
G00 Z2.05
G00 X1.1 Z0.07
G72 P101 Q102 D0.025 U0.02 W0.004 F0.01
N101 G00 Z0
G01 X-0.07
N102 G00 W0.1
G71 P103 Q104 D0.025 U0.02 W0.004 F0.01
N103 G00 X0.2
G01 G42 Z0
G01 X0.3
G03 X0.5 Z-0.1 R0.1
G01 Z-0.5
G01 X0.55
G03 X0.75 Z-0.6 R0.1
G01 Z-0.5
G01 X1.1
N104 G40 X1.2
G97 S1000 M09
G28
M01

T1
G50 S1000
G97 S1000 M03
G96 S300 M08
G00 Z2.05
G00 X0.6 Z0.15
G01 Z0 F0.05
X-0.07 F0.005
G00 X1.1 W0.1
G70 P103 Q104 F0.002
G97 S1000 M09
G00 G28

[Geof]

Just a quick glance and I have not put it in a machine but your problem could be here.

Notice on the second line down Z-0.5 then further down Z-0.6 followed by Z-0.5 meaning it is trying to back up.

Make this Z -0.6 or -0.7 and see what happens.

G03 X0.5 Z-0.1 R0.1
G01 Z-0.5
G01 X0.55
G03 X0.75 Z-0.6 R0.1
G01 Z-0.5
G01 X1.1

[1ctoolfool]

yes, z should be -1.0 after the 2nd G03 inside the G71, but why is it doing this?

runs fine when I manually change this in the program

do i have something set wrong somewhere or is this a VQC glitch?

thanks
joev

[Geof]

... but why is it doing this?....
do i have something set wrong somewhere or is this a VQC glitch?

thanks
joev

These questions I cannot answer. I took one look at VQC, came to the conclusion it was a lot of gobbledy-gook I did not need to know and went straight to G-code. I just have what I call template programs that have the G71 blocks numbered and all I need to do is enter the coordinates for what I am doing. Very quick, simple and I know what I am telling the machine to do and if there is an error I know it is in my entry not coming from someplace that I cannot control.

[SeymourDumore]

Yup, that Z-move appears bogus.
I'd say it looks to be a simple enough path to draw it in CAD and then pick the dims off of it, so Geof is right on with VQC being a little hokey.
Specially when you're using G42 in the G71 block, you can get exact results every time.
The only thing I'd add though is whenever I use comp inside the rough cycle, I prefer to put it in before the cycle starts and get out of it after. This way I seem to get better tool control in tight spaces such as neck-downs behind threads and such.

[Geof]

Regarding the G42 inside the G71 block you should check your manual. I know my TL1 ignores tool comp inside the G71 but reads it at the final pass using G70. It is necessary to make the U and W values large enough to cover the tool comp difference.

I found it very handy to sit down at the machine and play with different values and commands in graphics and see what is happening. Because the Haas editor is so easy to use you can write a program then duplicate an entire section below itself. In the duplicated section you do the changes you want to look at and then single block through in graphics. This way you can follow the trace when it is running through the duplicated but altered version of the program and see what is going on and how it differs from the unaltered version. Very useful for getting a handle on tool comp and tool vectors.

[SeymourDumore]

Geof

I have and SL10 and a MiniLathe. They both work with comp inside the canned cycle, and do so as intended.
One word of caution though, if you're programming realt part dims, and you're working both sides of the tool (such as in the case of the aforementioned neck-down) you do not want to specify a W. It causes overcut in the direction it was specified in. Absolutely fine with front and back tapers, just need to be careful with faces and walls.
But the short story is: G41/42 is functional withing G71 cycles.

[1ctoolfool]

my entry caused the problem, absolute vs. relative Z depth
I agree quick code is pretty plain,
thanks
joev