Haas Lathe Programmers

I was wondering if there are any Haas Lathe programmers here who use the G71 Stock Removal Cycle. I am having problems with a program I am trying to do with it. I have never really used these cycles as I generally use the cam system but wanted to try it and it keeps saying the program is non monotonic. I would like someone to look at what I have and tell me what I am doing wrong.

Thanks

I use these cycles all the time on my Haas, and have had the same problem. Post your code and I am sure we can figure it out.

Below is the code. It says it is non-monotonous. I am not sure but maybe it has to do with the 2 radius continuing in to each other. I appreciate any help.

%
O02001
( TOOL 9 )
T9 G54
N100 G97 S700 M03
N101 T909
N102 G00 X0. Z0.1 M08
N103 G01 Z-0.64 F0.006
N104 G00 Z0.1
N105 M09
N106 G00 X8. Z8.
N107 T606
N110 G50 S2800
N111 G97 S1910 M03
N115 G54 G00 X0.6 Z0.2 M08
N120 G96 S450
N125 G71 P130 Q165 U-0.01 W0.005 D0.1 F0.012
N130 G41 G01 F0.005 X2.91
N135 G01 Z0. F0.005
N140 F0.005 X2.905
N145 G02 X2.875 Z-0.03 R0.03
N150 G01 Z-0.0927
N155 G03 X2.6809 Z-0.3364 R0.25
N160 G03 X0.1 Z-0.6396 R11.9876
N165 G01 G40 X0.05 M9
N170 G70 P130 Q165
N175 G97 S1910 M5
N180 G28
N185 M30
%


[This message has been edited by Traceman (edited 07-29-2003).]

Your starting "X" and "Z" need to be the same place to complete the loop.

Try this. make changes shown on lines with *** .

O02001
( TOOL 9 )
T9 G54
N100 G97 S700 M03
N101 T909
N102 G00 X0. Z0.1 M08
N103 G01 Z-0.64 F0.006
N104 G00 Z0.1
N105 M09
N106 G00 X8. Z8.
N107 T606
N110 G50 S2800
N111 G97 S1910 M03
N115 G54 G00 X3.0 Z0.2 M08 ***
N120 G96 S450
N125 G71 P130 Q165 U-0.01 W0.005 D0.1 F0.012
N130 G41 G01 F0.005 X2.91
N135 G01 Z0. F0.005
N140 F0.005 X2.905
N145 G02 X2.875 Z-0.03 R0.03
N150 G01 Z-0.0927
N155 G03 X2.6809 Z-0.3364 R0.25
N160 G03 X0.1 Z-0.6396 R11.9876
N1625 G01 G40 X3. M9 ****
N165 G00 Z.2 ******
N170 G70 P130 Q165
N175 G97 S1910 M5
N180 G28
N185 M30

GOD!!! the Non monotonic alarm!!! It took me a while to understand that damn alarm, and what it means.... The BLANKING manual does not do a great job explaining it.
What it means is, your program is going back and forth along the same axis ... You can not do that in a type 1 program. If you want to remove stock say on an OD you would start your tool somewhere on the clearance plane. (assume a 2" dia. stock.) So your clearance plane is around 2.1" Your first move in your P,Q block will probably be a rapid move. Say... n1g0x1.48g42, after that you will FEED in towards Z0... n3go1z0.
From there on out in the rest of your P,Q block, you can only go BIGGER on diameter. The same goes for Z axis moves. Once you start on a path, say... z-.75 you can no longer go anywhere but further along the Z- direction.

Now type 2 programs...
If you want to go back and forth along a given axis while in a P,Q block you must use a type 2. Think of a larger diameter in the middle of the part. ( a shoulder, that you want to machine on either side of) You will have to use a type 2 for that.
That is not a big deal. All you have to do is put the X, and Z, positions on your starting N line. (Ex. N1g0x1.48z.1)
From then on out the machine will know it is a type two program.
The PROBLEM with a type 2 is that while it is very versitile, it will NOT leave any finsh stock either in X, or Z for a g70 clean pass.
This is where you might have a tool in tool position #1, with a given tool offset(t101), then copy that same offset to position 2, and use the tool wear to enter in a bigger dia. on tool offset #2 (t102)(ruffly the amount of cleanup pass that you want)
THere are different things you can do to get by this, buit I am probably not the man to teach you.


[This message has been edited by doug925 (edited 07-29-2003).]

[This message has been edited by doug925 (edited 07-29-2003).]

Thanks,
I will try the edits tonight and see if it will make it through the graph.

I will let you know tomorrow.

Bingo doug925,
Hey Traceman I use the g71 all the time over the cam output it gives me better controll on chip load. I hate it when you have to keep going back to the computer to repost a program. I usually start out aggressivly and sometimes have to cut back on the depth of cut with g71 you simply change one number and your on your way again.
Jeff.

Hey Traceman I use the g71 all the time over the cam output it gives me better controll on chip load. I hate it when you have to keep going back to the computer to repost a program. I usually start out aggressivly and sometimes have to cut back on the depth of cut with g71 you simply change one number and your on your way again.

Click to expand...

yeah, I really didn't like the way the Cam system was turning this and thought the G71 would work beter for my needs. We'll see tonight.

Well,
It didn't work. It kept giving me the same errors. I really don't see what it could be.

Try this change.
N115 G54 G00 X3.0 Z0.2 M08

Vortech,
That appears to be the same edit Cogsman gave me to make.

I am going to double check the radius points again to make sure I am not off there or something.

Well if that didn't work you are dealing with a differant level of g codes and you CANNOT go to a smaller dia. than the one you are at. You are at 2.6809 and then tell it to go down to .1, This level of G code will not let you do that. You will have to stop at the big dia and then do a grooving cycle "G75" or buy a higher level for your machine. You seem to have TypeI and you would need TypeII.
Goodluck

Traceman, Could line 140 be the culprit? it reads n140f0.005x2.905
Then you are trying a rad. of .03 from 2.905 to 2.875 diametricly... Should you not start your rad. from 2.935 IE. .06 diametricly from 2.875??? That alone could generate a non-monotonic alarm...
Also, it has been my experience that the Haas likes a rad. + -.0001 from what you would normally put. Not that I do that every time... just sometimes it likes it more than the nominal dimension.
One other thing... (yes I know you gave up on the part but,) Is you tool tip set to 2? I know this may be overly obvious... but I have overlooked that from time to time...



[This message has been edited by doug925 (edited 08-01-2003).]

Trace,
It's been awhile since I have run into that type of problem. I was running ball ends and I had to call the Haas tec guy's. At that time they said there was a software glich and I had to rough the front of the ball then the back of the ball then use a g73 for a finish pass. The tec department at Haas is pretty good. I would think they would have tackled that glich by know but it's worth a call. I know what you mean by that problem driving you crazy.
Jeff

I coppied the code and ploted it to see what's going on. In seconds you can see that transition from strait Z move to .25 R is generating undercut, transition from .25 R to large arc is too sharp and it seems that it's not blending at proper tangency point.
Second problem is the fact that even if it was on target , you would still get an alarm.
In G71 (and G72) undercuting is not allowed.
If you go from smaller dia to bigger dia in ID cycle, that is undercuting.
I used incremental move for that purpose in all my (one line) G71 type of cycles, in essence if you are going from X1.Z-.05 to X1.03Z-.2 in an ID cycle you will get an alarm, but if you go from X1.Z-.05 to Z-.2U.03 it will work,this is the same but incrimental command will cheat the cycle.

Another way to do this is by roughing majority of stock by G71 and then using G73 to do pattern shifting passes and profile the feature of any configuration tool can clear, use G70 to repeat G73 profile and you are done.
You can make that lathe dance without ever touching Type II G71 cycle.
Get the software here:
http://www.CNCEdit.com
set graphics plotting for lathe and see for yourself.
I always use I and K to define arcs, mush more acurate especially when doing arcs that cross one quadrant.


[This message has been edited by Vic (edited 08-16-2003).]

not a haas man but haas claims to use the same codes as fanuc and i use fanuc daily.
on the fanuc you can not use tool nose comp (g41)in a g71 cycle on 6ta or b controls. just my 2cents.