5 axis positioning question

[kojack]

I normally use g54 and cut with tip for Surfaces on a 5 axis table

I was putting some logos on a part the other day

I figured Id program the logo with 3 axis paths and just position the part

So I positioned the part and set my work offset with G58

Figured every time a part needed a logo

I would just use a G58 in the program and it would rotate the A and B axis

It doesnt work that way Unless I call out a A62 B 180

I thought the G58 would turn the rotary's since my offset table The A and B

axis have been set with Part Zero's


What AM i missing ?

Thanks for the help ...

[makingchips]

Set the A/B the same way you would set the X/Y at the position you need, but there is no way around programming G90 G58 X0. Y0. A0. B0. so in hindsight A62 B 180 is just as easy. You could make a little sub program that can do this with M98 then you only have to program the A62 B 180 program once.You only add the M98 M99 to the program you need logos on.




MC

[kojack]

Originally Posted by makingchips Set the A/B the same way you would set the X/Y at the position you need, but there is no way around programming G90 G58 X0. Y0. A0. B0. so in hindsight A62 B 180 is just as easy. You could make a little sub program that can do this with M98 then you only have to program the A62 B 180 program once.You only add the M98 M99 to the program you need logos on. MC

Thanks for the help ....

I was just confused on why you set A and B in offset table but it doesnt move if you call it out ?


Its not that big a deal I could have programed my part LOL with less typing

so far .. I just figured I was missing something ...

[Caue]

Kojack,

If you loaded A62. B180. into Work Offset Table, as G58 postioning angles, you should only call G0 G58 X## Y## Z## A0 B0 (just as makingchips said) on your code and it should work.
If this is the case, it's programed this way and not working, please post CNC code and we'll analyse it for you.
Cheers!

[kojack]

here are my settings and program

here is a screen shot of the Offset table



here is the code
O0123
(PROGRAM NAME - LOGO )
(DATE=DD-MM-YY - 24-04-09 TIME=HH:MM - 00:02 )
N100 G20
N102 G0 G17 G40 G49 G80 G90
( 1/16 FLAT ENDMILL TOOL - 6 DIA. OFF. - 6 LEN. - 6 DIA. - .0625 )
N104 T6 M6
N106 G0 G90 G58 X.2435 Y-.9587 S12000 M3
N108 G58 H6 Z4.
N112 Z.1
N114 G1 Z-.02 F6.2
N116 X1.7565 F40.
N118 G3 X1.8393 Y-.9387 I-.0065 J.2087
N120 G1 X.1608
N122 G2 X.1271 Y-.9188 I.0893 J.1887
N124 G1 X1.8729
N126 G3 X1.8964 Y-.8988 I-.1229 J.1688
N128 G1 X.1036
N130 G2 X.0858 Y-.8789 I.1464 J.1488
N132 G1 X1.9142
N134 G3 X1.9281 Y-.8589 I-.1642 J.1289
N136 G1 X.0719
N138 G2 X.0612 Y-.839 I.1781 J.1089

[big_mak]

I can't see you calling A or B in your program. Maybe I'm just missing it!

[kojack]

Originally Posted by big_mak I can't see you calling A or B in your program. Maybe I'm just missing it!

no your right ...

But I have a G58 in there and my G58 has the rotory where i need it too go ..

look @ my G58 on the offset table

I run the normal program with g54

I wanted to just place my logo program with a different offset G58

figured it would rotate the tables ...

[big_mak]

G58 will just make that work Coordinate active, it will not reposition until you G00/G01 A## B##

[kojack]

Originally Posted by big_mak G58 will just make that work Coordinate active, it will not reposition until you G00/G01 A## B##

So G58 or G56 wont postion A and B axis unless I call it out

where would you put the B and A move in this Program Can i run it on my
g58 line

I need to go B 208.485 A 62.2

O0123
(PROGRAM NAME - LOGO )
(DATE=DD-MM-YY - 24-04-09 TIME=HH:MM - 00:02 )
N100 G20
N102 G0 G17 G40 G49 G80 G90
( 1/16 FLAT ENDMILL TOOL - 6 DIA. OFF. - 6 LEN. - 6 DIA. - .0625 )
N104 T6 M6
N106 G0 G90 G58 X.2435 Y-.9587 S12000 M3
N108 G58 H6 Z4.
N112 Z.1
N114 G1 Z-.02 F6.2
N116 X1.7565 F40.
N118 G3 X1.8393 Y-.9387 I-.0065 J.2087
N120 G1 X.1608
N122 G2 X.1271 Y-.9188 I.0893 J.1887
N124 G1 X1.8729
N126 G3 X1.8964 Y-.8988 I-.1229 J.1688
N128 G1 X.1036
N130 G2 X.0858 Y-.8789 I.1464 J.1488
N132 G1 X1.9142
N134 G3 X1.9281 Y-.8589 I-.1642 J.1289
N136 G1 X.0719
N138 G2 X.0612 Y-.839 I.1781 J.1089

[big_mak]

Make Line N107 G0 A### B###

[gpcoe]

Originally Posted by kojack So G58 or G56 wont postion A and B axis unless I call it out where would you put the B and A move in this Program Can i run it on my g58 line I need to go B 208.485 A 62.2 O0123 (PROGRAM NAME - LOGO ) (DATE=DD-MM-YY - 24-04-09 TIME=HH:MM - 00:02 ) N100 G20 N102 G0 G17 G40 G49 G80 G90 ( 1/16 FLAT ENDMILL TOOL - 6 DIA. OFF. - 6 LEN. - 6 DIA. - .0625 ) N104 T6 M6 N106 G0 G90 G58 X.2435 Y-.9587 S12000 M3 N108 G58 H6 Z4. N112 Z.1 N114 G1 Z-.02 F6.2 N116 X1.7565 F40. N118 G3 X1.8393 Y-.9387 I-.0065 J.2087 N120 G1 X.1608 N122 G2 X.1271 Y-.9188 I.0893 J.1887 N124 G1 X1.8729 N126 G3 X1.8964 Y-.8988 I-.1229 J.1688 N128 G1 X.1036 N130 G2 X.0858 Y-.8789 I.1464 J.1488 N132 G1 X1.9142 N134 G3 X1.9281 Y-.8589 I-.1642 J.1289 N136 G1 X.0719 N138 G2 X.0612 Y-.839 I.1781 J.1089

This is how I would write it:

N106 G0 G90 G58 X.2435 Y-.9587 B208.485 A62.2 S12000 M3

However on your offset page under G58 I would have the Rotary axis set the same as the other (G54) coordinates. Mine are set to the B axis face (the one you mount to) planer to the machine table. So if I were to do work on the horizontal (A90) in any work coordinate I would always call out A90. in the program. That way anyone else who programs for the machine can program the same and setup is straight forward.

Greg

[Caue]

Alright, now we have your original code, it's quite easy. It's correct that inform G58 only load this information to the machine, but it does NOT command any movement. But, once the coordinates (angles) are informed at Work Offset Screen, you must call A0. (tip: you can type only "A" and the software will complete when you type Write/Enter or Insert) B0. The code will be:

O0123
(PROGRAM NAME - LOGO )
(DATE=DD-MM-YY - 24-04-09 TIME=HH:MM - 00:02 )
N100 G20
N102 G0 G17 G40 G49 G80 G90
( 1/16 FLAT ENDMILL TOOL - 6 DIA. OFF. - 6 LEN. - 6 DIA. - .0625 )
N104 T6 M6
N106 G0 G90 G58 X.2435 Y-.9587 A0. B0. S12000 M3
N108 G43 H6 Z4.
N112 Z.1

My inputs are bold. I use to call all 4 axis positioning at the same block (only exception to Z axis), but you need to check if there's enough space for it at the first time you run the program.
Please, note that I've replaced the second G58 for G43, and this is the most worrying point, cause it may crash the machine.

I hope it can be useful. Once more, thank you all for choosing Haas Automation!!