HItachi Seiki CH-250 Polar Coordinate Problems

So we've got a mill turn system at work that I just took over. I'm trying to figure out all its bells and whistles. It didn't have the polar coordinate feature activated until I talked with a tech that did it for me. It'll interpolate correctly in that it will now feed inches/min instead of degrees/min. The problem is that it'll maybe do a few interpolations but as it goes it will move further and further away from the chuck. I assume it's moving in incremental mode, but once I have G121 (polar interpolation) activated it'll throw an error if I put G90 in the code. I've tried quite a few iterations of this, but here's the sample code:


%
O1112 ( .TXT )
(Hitachi_Seiki_Super_HiCell_250_Post)
G170
G28 WB0
G30 U0.
G30 V0.
G30 W0.
M1

N1 T021000
T991500
G40 G80 G17 G54 M43
(---OP1 F-CONTOUR---)
G97 G98 S1000 M13
M8
G121
G0 X5.4162 Z0.4 C-4.6374 F50.
G0 Z0.0393
G1 Z-0.001 F1.32
G42 X5.4154 C-4.6338 F10.
C-55.3662
G3 X2.32 C2.4467 R0.4375
G1 C-115.3662
G3 X-3.0778 C2.2279 R0.4375
G1 C-175.3662
G3 X-5.3983 C-0.2183 R0.4375
G1 C-235.2271
G3 X-2.1936 C-2.4382 R0.4375
G1 X4.646 C-263.3303
G2 X-0.37 C-2.3036 R0.375
G1 X5.358 C-296.3943
G3 X3.2 C-2.1714 R0.428
G1 X4.888 C-325.1599
G2 X4.1817 C-1.3319 R0.125
G1 X5.0508 C-328.5232
G3 X4.8663 C-1.0676 R0.375
G1 X5.4788 C-357.1712
G3 X5.3978 C0.2188 R0.4375
G40G1 X5.4162 C-364.6374
G0 Z0.4 F50.
M15
G120
M9
G30 U0. V0.
G30 W0.
M41
M30
%

I've tried changing X to U and the same thing happens. I've also tried either having no X words, typing in X0, and putting U0 in the code and it still moves away from the spindle. Can anyone help me figure out why this is happening?

Triam said:

I assume it's moving in incremental mode, but once I have G121 (polar interpolation) activated it'll throw an error if I put G90 in the code. I've tried quite a few iterations of this, but here's the sample code:

Click to expand...

Unless the G Code System being used supports G90/G91 for Absolute, Incremental Mode respectively, U and H are used for Incremental moves in the X and C axis respectively. The various G Code Systems can't be mixed, therefore, as you don't make any reference to

G28 WB0
G30 U0.
G30 V0.
G30 W0.

not working correctly, G90/G91 won't be valid for selecting Absolute and Incremental mode.

Triam said:

N1 T021000
T991500
G40 G80 G17 G54 M43
(---OP1 F-CONTOUR---)
G97 G98 S1000 M13
M8
G121
G0 X5.4162 Z0.4 C-4.6374 F50.
G0 Z0.0393
G1 Z-0.001 F1.32
G42 X5.4154 C-4.6338 F10.
C-55.3662
G3 X2.32 C2.4467 R0.4375

Click to expand...

1. The C address when in Polar Interpolation Mode substitutes for Y in an X, Y program.

2. Unless your control is set to consider X as a Radius Value, X will still be programmed in diameter, the same as in a turning operation.

I've only examined the first few Blocks of your program and I can't see how it can work geometrically. Irrespective of how X is interpreted by your control, the distance in Y (C Move) between the Start and End point of the program's first Circular Interpolation is 57.8129, with an R (Radius of the G03 arc) of 0.4375. Geometrically this is not possible. The absolute minimum the R address value could be for these two points is 28.9168.

Post a sketch, with dimension included, of the profile you want to machine.

Regards,

Bill

The way I have it oriented is so that X would be horizontal. Y would be vertical and Z would be coming out of the page. The tool is programmed to start at the point furthest to the left on this drawing and moves counterclockwise around the part (that is to say, the spindle turns clockwise.)

Here's the print:



(I tried to not clutter it with all the dimension so it would be easier to understand. If you need more then let me know)


Here's the three pages in my programming manual that talk about polar coordinates:

Hello Triam,
The following Code is for the profile in the attached drawing of your previous Post with the exception of the detail at 12 and 1 o'clock, where dimensions have not been included; that is, its a 4.646 AF hexagon with 0.313 corner radii. The tool path starts at the 3 o'clock on the profile.

Irrespective of the angle the C axis is indexed to prior to Polar Interpolation being launched, C0.0 is assumed immediately after G121 is executed. Accordingly, if you wish to starts at the 9 o'clock area of the part, as indicated in your last Post, then you would index the C axis to bring the 9 o'clock area of the part to 3 o'clock before launching Polar Interpolation, then program the part starting at 3 o'clock (Zero Degrees) as in my example.

Regards,

Bill

Thanks a ton. That code works. Now I just need to figure out how to make the post processor spit out similar work.