[murrayadams]

hi, im new to this forum but ive had a search and i cant find the specific information i need. ive recently purchased an older hitachi vk45 with a fanuc om-d controller. when i try to run a helical program either milling or threading the controller runs all the z feed first then trys to run the g02. threading causes an alarm and does not feed at all.the manual i have for the om controller says the om-d series-1 controller did not have a helical option, the other 2 series did.the operator manual for the vk45 does not list the series,in fact it is not very specific about which controller its using. it is in fact close to the worst manual ive ever seen. the maintenance manual does not seem to list a parameter for helical motion, but it also does not list any parameters between about 300-500. i notice other people have had similar problems, is there a solution? also where would i find a complete list of parameters? hope some one can help. thanks

[stucapco]

First, contact Fanuc. Is this an option on your controller and machine? Second if it is, are the correct parameters initialized (allowed into play)? I write helical interpolating on my Fanuc all the time.

O0001;
G56 X1.125 Y0 S1250 M3;
G43 H1 Z-.5 M8;
G01 X.5 G42 D1 F5;
M98 P2 L10;
G90 G01 X0 G40;
G0 Z1. M9;
G54 G49 Y0 Z0;
M30;

The sub (P2) looks like this:

O0002;
G91 G03 I-.5 Z.05;
M99;

This assumes a one inch dia, half inch deep, 20 threads per inch and your using cutter comps (height and radius) correctly.
DO NOT USE THIS CODE! I'ts off the top of my head but would work fine in my machines assuming those factors.

I'ts short and simple, all that's needed.

Luck!

PS: right handed thread.

[murrayadams]

thanks Stucapco , ive done a bit more research and contacted fanuc, but as yet im not sure if its an option or not. the controller is actually an om-a and was made in 1986. im assuming the code you posted is for a machine with a helical option. it looks very similar to the code produced by the capsmill program i use with the vk45. the tool paths work fine in the simulator in the program but not on the machine. is it possible to write a subprogram for a machine without a helical option? or are they limited to motion in only 2 planes at a time?

[stucapco]

I see your point and I really don't know on that controller (machine). My advise is to BACKUP the parameter lists before trying anything related to this change. Stand in, my options hang out in the 9000 parameter range. Holy cow look at all the little "goodies" I can turn on. lol

Luck

[Superman]

helical program either milling or threading the controller runs all the z feed first then trys to run the g02. threading causes an alarm

standard threadmilling.... yes ?

Put up the code you are using.
- it could be that you are programming a full arc with a Z pitch......it may think it is already at the finish point and just does a Z move
try breaking the arc into 180° moves

I have worked on a control that could only do 2D arcs,,,,, cannot do a 3D interpolating move

[fordav11]

it might help to know the exact alarm. then we could know if its program error or missing option.

[mactec54]

murrayadams

This is a simple Helical program that might work with your old control, this is using a (.375 EM ) 1.0" hole .5 deep X0 Y0, change speed & feed to suit

%
O3189
N1G17G40G80
T5M6
M8
G54
S2650M3
G90G0X-.2706Y-.1562
G43Z.1H5
G1Z0.F12.
G3X0.Y.3125Z-.02I.2706J.1562F20.
Z-.05J-.3125
Z-.08J-.3125
Z-.11J-.3125
Z-.14J-.3125
Z-.17J-.3125
Z-.2J-.3125
Z-.23J-.3125
Z-.26J-.3125
Z-.29J-.3125
Z-.32J-.3125
Z-.35J-.3125
Z-.38J-.3125
Z-.41J-.3125
Z-.44J-.3125
Z-.47J-.3125
Z-.5J-.3125
J-.3125
X-.02Y.2925J-.02
G0Z3.
M9
M5
M30
%

[adriantom]

I used a program like this and it works well. I found it couple days ago in a programing book :CNC Programming Hanbook by Peter Smid.I modified after my needs and was very good. Good luck!

[murrayadams]

the error code that pops up during the threading cycle are 038 on the controller and 5085 on the screen around the side of the machine. the 038 description says " overcutting will occur in cutter compensation c because arc start point or end point coincides with arc center." 5085 just says NC alarm. i found a list of parameters for options at http://www.gdsk.net/upload/201003/20100309101603704.xls and according to these both helical and 3 axis are turned on.the code i have tried to use but only feeds the z axis looks like this. this is just the first boring pass.
(HELICAL BORING)
G90 G00 G54 X80.000 Y-26.000
G43 H09 Z100.000
G43 H09 Z3.000
F100.1
X84.951 Y-25.639
G02 X85.100 Y-26.000 I-0.361 J-0.361
Z1.881
Z0.762
Z-0.357
Z-1.476
Z-2.595
Z-3.714
Z-4.833
Z-5.952
Z-7.071
Z-8.190
Z-9.309
Z-10.428
Z-11.547
Z-12.666
Z-13.785
Z-14.904
Z-16.023
Z-17.142
Z-18.261
Z-19.380
Z-20.499
Z-21.618
Z-22.737
Z-23.856
Z-24.975
Z-26.094
X76.686 Y-29.876 Z-26.500
I3.314 J3.876
X76.508 Y-29.528 I0.331 J0.388
G00 X80.000 Y-26.000
G43 H09 Z3.000

[mactec54]

murrayadams

Your program is missing the J value for each Z move, it needs it to look like what I posted

[fordav11]

the overcutting alarm means your program is wrong. if it was missing options you would get a different alarm

[stucapco]

mactec54 is correct, that's not helical, it's plunge. I see no circular interpolation here.

[Superman]

mactec54 is correct, that's not helical, it's plunge. I see no circular interpolation here.

Blind ?

What is the last G code before the Z lines ?.......remember it's modal

...so any missing info is carried from the last time it was stated.
---doing full circles may be the exception, it may need to know where it's centre of sweep is ( on each line )

[murrayadams]

the code is as the caps mill programs produced it . maybe the post processing is incorrect for the machine, what is the function of the j term with each z move? could be worth a try but id like to know how the code works when i modify things , the idea that it thinks its already completed the circle sounds possible too

[mactec54]

the code is as the caps mill programs produced it . maybe the post processing is incorrect for the machine, what is the function of the j term with each z move? could be worth a try but id like to know how the code works when i modify things , the idea that it thinks its already completed the circle sounds possible too

What is your cutter size & what is the hole size you are trying to machine, from this we will know what the J value has to be

[murrayadams]

i tried cutting and pasting the j value after each z line and ran it through the machine with no material. sure enough it works . from the look of the position readout its cutting a hole and its certainly running all three axis at once. but im still unsure WHY it works and why the cam program is producing code that doesn't do the job. a helical boring subprogram could be a solution . but these are simple issues. thanks so much everybody for the help. i hope i learn enough to contribute as well one day.

[fordav11]

CAPS? as in conversational programming built into the machine? assuming yes, CAPS has a *lot* of parameters. one of them probably tells it to omit the J value if it is the same as the previous one. that's incorrect, of course. or there could be some other CAPS parameter that is wrong.
In my experience using FAPT and CAPS for 25 years, I've found that CAPS is full of bugs and functions like helical milling were not well tested (and therefore not bug-fixed). unfortunately a lot of the CAPS parameters are undocumented (i.e. secret) so you will probably just have to copy/paste the J value into the program (for the rest of your working life on that machine ;-)