[Dragoon2]

I am having problems getting my 1980 Howa Sangyo NC11L with a 5T control to circular interpolate. I have tried to follow the manual as best I can, but every time I try it, I get an error 20 (circular interpolation end point error).

I also have another problem that is more troublesome, I can not rapid traverse more than a half inch without it alarming out in both X and Z axis.

I bought this lathe about four months ago and have been trying to get it going in my spare time. I have found some manuals and have been able to fix most of the problems, I am also trying to get a Cimnet BTR that was installed by the previous owner to communicate with the control using Machine Link. At this point I can send programs from the computer to the BTR and on to the control, also from the BTR back to the computer, but when I try to run the program in auto I get a TH alarm. I think this is a horizontal parity error; what does it mean?

Does anyone out there have any ideas on these issues?

Steve

[bborb]

Please post the G-code that won't run.
Are you using a phase converter to power the machine?

[Dragoon2]

I have 3 phase 480 and a 240 step down transformer, and I have checked the voltages, They seem to be OK.

I have written several programs that I wanted to cut, but so far all have not worked when they get to the G02/03 code, so I wrote a simple one to trouble shoot with. I have tried a few variations, and have tried to the best of my ability to interpret the Fanuc programming manual, here is what I have.

The M26 is a gear range setting for the Howa NC11L.

N001T0600M26;
N002G97S350M04;
N003G50X-102600Z50000;
N004G01X-10000Z0000F5000;
N005G01Z-5000F0100;
N006G02X-20000Z-10000I-5000F0100;
N007G01X-102600Z50000F5000;
N008M30;

First, if I try to use rapid (G00) commands in either axis it alarms out, I need to fix that yet but for now I am just issuing fast feed rates for positioning.

In this program you press cycle start, everything works up to the G02 when it gives an Error 20 and stops, I press the reset button then cycle start, and the program picks back up and finishes. I can do this over and over, just no circular interpolation.

Steve

[bborb]

In the above code, try putting G03 in place of G02 and don't change anything else. See if the error goes away. I'm not familiar programming with - (minus) X values. I can only guess the turret you're using HAS to be programmed with negative X values, or this is the only way you figured out to get things to work. In any case, my NCPlot didn't like your code until I changed the G02 to G03 and then it plotted just like the cut was a G02..... figured G02 becomes G03 on the opposite side of centerline.

[Dragoon2]

Thanks, I have tried that and it does not work in this case either.

I had a gentleman with the same machine as mine try this code and it did not work for him either but he suggested that I use the front turret which would be in the X positive direction. He said the front turret is normally used for OD turning. I was using the rear turret that is normally used for drilling / boring because it can go past center in X, which brings me back to why I used the rear turret in the first place. I was trying to do a contour radius on the ID then around the end to the OD, and then an arc on the OD from there. I have a tool with a 180 degree .094 radius that I am using to do this, I have programmed the cutter center path so I don't need cutter comp. The manual says that I can only do 1 quadrant at a time on the 5T, so I tried aproaching the part near center in Z, then feed out in X, then a G03, another G03, and a G02. It did not work so I have been trying simple one quadrant arc programs without any sucess yet. My next attempt will be using the front turret to see if the machine likes it better for some unknown reason.

Steve

[Dan Fritz]

Some of the early 5T and 5M controls could only circular interpolate one quadrant at a time. I didn't analyze your program, but if you're crossing a quadrant boundary with a G02 or G03 command, that would give an alarm.

The rapid traverse alarm could be almost anything. There are parameters that determine what the rapid traverse rate is, and if the parameter is set too high, your servos can't keep up and you'll get an "excess error" alarm. It would help to know what alarm number you're getting.

The 5T uses the old 3-phase SCR drives, and if they're not tuned up properly, you will have all kinds of trouble. It may be that the servos just need a good tweaking.

[Dragoon2]

Hi Dan,

I have tried to do only one quadrant at a time tool paths, but still no success with circular interpolation.

I know that I can get it to feed as fast as a setting of F5000 @ 350 spindle RPM, I think this is 1/2 inch per revolution, it is fairly fast. Much above that and it alarms out, it will alarm out in about 1/2 inch of rapid G00 or a manual rapid command in either axis which makes it just about impossible to use G28 or manual zero return, in manual I can get within 1/2 inch of the switches and send it home as it rapids then hits the decel switches and slows down until it zeros the axis. Because it does this in both axis I think it is a speed / excess error related issue which could be a parameter setting problem, the power / voltage levels look OK as best as I can tell.

The rapid alarm sets a 1 under "SV", I figured I would have to get someone to look at this thing eventually. I am in the Grand Rapids, Michigan area, do you know of anyone that works on these?

Does anyone have the parameter information for a 1980 vintage Howa Sangyo NC11L with a 5T control? I have some examples, but they are either for another lathe or are incomplete.

Thanks for your input, if you have any ideas I sure would appreciate them.
Fortunately this lathe is a hobby machine for me and is not something I need for a living. It sure is a nice big old piece of iron though (22x60), and I do want to get it running.

Kind Regards,
Steve

[Paul Pippenger]

The values in your I(x) and J are not correct .
Remember these are in relation to where you start the radius.If X0 is the center of the part (spindle) then the arc should have a positive x end point and I is 0
J is the amount the point is away from the tool tip in this case must also be positive.

[Dragoon2]

Paul,

I have worked out the rapid / feed issues as well as the G02/03 problem.
Regarding circular interpolation I found that the positive / negative is very different on this machine. I have to visualize the part from underneath looking up, program it that way and the circular interpolation works fine.

Thanks for the reply!

Steve

[Paul Pippenger]

Thanks for the update ,i know you probably solved this a long time ago but I have just joined this site and I have already found ways to help some others ,Please find my post on the best way to use offsets larger than 9.9999on this control ,it seems not even the tech guys knew of my fix.It may help you also.
Peace
P