[gapy88]

Hi
needsome help. Im runing Hartford matrix VMC-560. I got this problem:
i would like to write a gcode, to make 3 identical electrodes. When i generate my gcode in solidacm, it is in position g45(default). How to change code, so that when electrode on g54 is complete the machine contntinues milling same electrode on g55 and g56 position.
This ismy code :

[mactec54]

Hi
needsome help. Im runing Hartford matrix VMC-560. I got this problem:
i would like to write a gcode, to make 3 identical electrodes. When i generate my gcode in solidacm, it is in position g45(default). How to change code, so that when electrode on g54 is complete the machine contntinues milling same electrode on g55 and g56 position.
This ismy code :

You may not even need to use a different offset, where ever you want it to start the next part you can just do a G0 Y0.X100 or what ever the spacing is, if you want to use G55 and G56 then you have to set that in the machine offset page where you want each offset to start, just like when you setup for your G54, work X0Y0 then you do the same for any other offset you want to use

[chuckorlando]

How exactly would that single line of code move the whole prog to a new origin?

I would have modeled it with 3 and prog it like one part. "Nesting"

Like mentioned, you need to pick up the origin for the G55 and G56 just like you do for G54. Then just replace the G54 with the G56

[rcs60]

i would write it as a subroutine
this is from a haas control similar to fanuc(may have to be writen as a seperate program then called up )(O1011 instead of N1011)


N1
( 3/8 FLAT ENDMILL DIA. - .375 )
T1 M06

S6100 M03 T2
G00 G90 G54 X-0.156 Y-0.4 A0.
G43 H01 Z1.
M08
M97 P1011


G55 X-0.156 Y-0.4
M97 P1011

G56 X-0.156 Y-0.4
M97 P1011

G57 X-0.156 Y-0.4
M97 P1011

N100
G00 Z1. M09
G91 G28 Z0. M05
M30

N1011
G00 Z0.107
G01 Z0. F50.
Y1.3 F72.
X0.156
Y-0.4 F72.
G00 Z1.
M99

[mactec54]

How exactly would that single line of code move the whole prog to a new origin?

He obviously has repeated his same program 3 times but it did not move to another location because he had not set it

The simple line of code works like this instead of having a G55 or a G56 after the first part had cut after Z retract you just use a X Y move to the next position, very simple, and then run the same program again

[chuckorlando]

If he has 3 prog with 3 work off sets they would be identical prog except the g54. So every one would say x1.0 from the origin. So simply moving over would not change the origin for any of them.

So it runs a prog, you tell it to move over x1.0, run the next prog, it will return right to the orig orig and run the orig prog.

Every number in the other codes would also have to reflect that change because they all work off their own origins.

[mactec54]

If he has 3 prog with 3 work off sets they would be identical prog except the g54. So every one would say x1.0 from the origin. So simply moving over would not change the origin for any of them.

So it runs a prog, you tell it to move over x1.0, run the next prog, it will return right to the orig orig and run the orig prog.

Every number in the other codes would also have to reflect that change because they all work off their own origins.

Not at all it would not have the G54 offset in the next program the X Y move take care of that, I do this all the time, it works works well, and is very simple, here is an example, there are other ways to do this same thing as well

%
O1
N1G17G40G80
T4M6
M8
G54
S3450M3
G90G0X-.25Y-.25 ( First Part Start )
G43Z1.H4
G1Z-.5F20.
Y-1.75F60.
G3X.25Y-2.25I.5
G1X1.75
G3X2.25Y-1.75J.5
G1Y-.25
G3X1.75Y.25I-.5
G1X.25
G3X-.25Y-.25J-.5
G0Z.1
G90G0X2.35Y-.25 ( 2nd Part start )
G1Z-.5F20.
Y-1.75F60.
G3X2.85Y-2.25I.5
G1X4.35
G3X4.85Y-1.75J.5
G1Y-.25
G3X4.35Y.25I-.5
G1X2.85
G3X2.35Y-.25J-.5
G0Z.1
G90G0X4.95Y-.25 ( 3rd Part Start )
G1Z-.5F20.
Y-1.75F60.
G3X5.45Y-2.25I.5
G1X6.95
G3X7.45Y-1.75J.5
G1Y-.25
G3X6.95Y.25I-.5
G1X5.45
G3X4.95Y-.25J-.5
G0Z3.
M9
G53Y0.
M5
M30
%

And here is the same program but much shorter
%
O1
M98P2L3
G92X.95
M30
O2
N1G17G40G80
T4M6
M8
G54
S3450M3
G90G0X-.25Y-.25
G43Z1.H4
G1Z-.5F20.
Y-1.75F60.
G3X.25Y-2.25I.5
G1X1.75
G3X2.25Y-1.75J.5
G1Y-.25
G3X1.75Y.25I-.5
G1X.25
G3X-.25Y-.25J-.5
G0Z3.
M9
G53Y0.
M5
G90
G92X-.85
M99
%

[109jb]

The single line move between parts will only work if the rest of the program is written in G91. He has it written in G90, so a single line move like that won't work without G54-G59 offsets.

To use G54-G59 you need to set zero for each one individually. Then when the next work offset is called it will use the defined zero for that one.

[mactec54]

The single line move between parts will only work if the rest of the program is written in G91. He has it written in G90, so a single line move like that won't work without G54-G59 offsets.

To use G54-G59 you need to set zero for each one individually. Then when the next work offset is called it will use the defined zero for that one.

Works perfect no G91 needed in any programing like this

[109jb]

Your program is a total re-write, not a duplicating code for identical parts. Sure that will work, if you have a single fixture that holds the multiple parts, but not so easy if you have separate fixtures, or are using separate vises. Your way would require re-writing the code every time, or careful alignment of the individual fixtures/vises if you wanted to set a job up again. G54-G59 won't care if the individual fixtures aren't perfectly aligned and have perfect offsets since each one has its own zero location.

The guy wanted to know how to use G54-G59 work offsets. The answer to that is not to rewrite the whole program to not use G54-G59. The answer is to tell him how G54-G59 are supposed to work.

[gapy88]

%
O1 (0001)
(KNIFIC 29-AUG-2016)
(----------- ORODJA -----------)

(- T#4 REZ. TOROIDNI D11.8 R0.-)
#4=16 ( --- POZ. ORODJA #4 ----)

(- T#1 REZ. TOROIDNI D11.8 R0.-)
#1=13 ( --- POZ. ORODJA #1 ----)

(- T#3 REZ. TOROIDNI D5.8 R0.5-)
#3=7 ( --- POZ. ORODJA #3 ----)

(- T#2 REZ. TOROIDNI D5.8 R0.5-)
#2=8 ( --- POZ. ORODJA #2 ----)

G40 G49 G80 G90
G54
(- BULL NOSE MILL D11.8 R0.5
T#4 M06
S5000 M13
G49
(- OPER.: HSR-R-CONT-TARGET-1 -)
G05.1Q1
G0 G43 H#4 Z100.
G0 X-10.439 Y28.326
G0 Z10.
G0 Z1.805
G1 X-10.331 Y28.218 Z1.04 F2000
X-10.025 Y27.912 Z0.391
X-9.566 Y27.453 Z-0.043
X-9.025 Y26.912 Z-0.195
X-3.627 Y21.514
G3 X0. Y20.012 I3.627 J3.627
G1 X19.529
X20.554 Y19.976
X21.632 Y19.727
X22.736 Y19.187
G2 X23.653 Y18.406 I-3.415 J-4.939
G2 X23.862 Y18.173 I-4.09 J-3.8
X27.398 Z-66.346
X27.55 Z-65.58
Z10. F6000
G05.1Q0
M5
(- BULL NOSE MILL D11.8 R0.5
T#1 M06
S5000 M13
G49
(- OPER.: HSM-CZ-TARGET -------)
G05.1Q1
G0 G43 H#1 Z100.
G0 X-0.702 Y-5.958
G0 Z10.
G0 Z1.975
G1 X-0.718 Y-5.954 Z1.715 F2000
X-0.768 Y-5.944 Z1.459
X-0.85 Y-5.928 Z1.212
X-0.943 Y-5.903 Z1.012
X-1.057 Y-5.872 Z0.823
X-1.19 Y-5.837 Z0.649
X-1.297 Y-5.802 Z0.532
X-1.412 Y-5.764 Z0.425
X-1.53 Y-5.722 Z0.33
X-1.695 Y-5.654 Z0.22
X-1.87 Y-5.581 Z0.129
X-2.027 Y-5.505 Z0.066
Y3.277 Z-66.619
Y3.193 Z-66.372
Y3.142 Z-66.115
Y3.125 Z-65.854
Z-64.854
Z10. F6000
G05.1Q0
M5
(- BULL NOSE MILL D5.8 R0.5
T#3 M06
S2000 M13
G49
(- OPER.: HSR-RESTR-TARGET-1 --)
G05.1Q1
G0 G43 H#3 Z100.
G0 X12.576 Y8.67
G0 Z10.
G0 Z4.804
G1 X12.544 Y8.688 Z4.422 F1500
X12.448 Y8.739 Z4.055
X12.291 Y8.822 Z3.715
X12.08 Y8.933 Z3.414
X11.823 Y9.07 Z3.165
X11.528 Y9.226 Z2.977
X11.207 Y9.397 Z2.855
X10.871 Y9.575 Z2.805
G3 X7.523 Y7.507 Z2.639 I-1.068 J-2.014
G3 X10.966 Y5.6 Z2.473 I2.279 J0.054
G3 X10.944 Y9.535 Z2.308 I-1.163 J1.961
G3 X7.523 Y7.589 Z2.142 I-1.141 J-1.974
G3 X10.894 Y5.559 Z1.976 I2.28 J-0.029
G3 X11.015 Y9.492 Z1.81 I-1.091 J2.002
G3 X7.525 Y7.672 Z1.644 I-1.212 J-1.931
G3 X10.82 Y5.52 Z1.479 I2.277 J-0.112
G3 X11.084 Y9.447 Z1.313 I-1.017 J2.04
G3 X7.531 Y7.755 Z1.147 I-1.281 J-1.886
G3 X10.745 Y5.485 Z0.981 I2.272 J-0.194
G3 X11.152 Y9.399 Z0.816 I-0.943 J2.076
G3 XX3.527 Y-3.721 Z-15.222
X3.507 Y-3.835 Z-14.987
X3.492 Y-3.917 Z-14.739
X3.483 Y-3.968 Z-14.483
X3.48 Y-3.985 Z-14.222
Z10. F6000
G0 Z100.
G05.1Q0
M5
G0 G90 G53 Z0
M30
%

[gapy88]

is it possible to paste 2 another identical program at the end of first one, but just with diferent position (g55) ?

[rcs60]

gapy88 is this question on how to use G54-G59 or how to get solidacm to do the G54-G59 into the program ?

[chuckorlando]

gaby88 you have 3 totaly different prog for the 3 parts and the second one is a macro. Which is fine.

In this case though if you took just the first part and the code for it, the only change per part would the G54 to a G55 and G55 to a G56

In HSM works for multiple origins you put the number in the "multiple work off sets" box on the set up page. g54=1 g55=2 g56=3

[chuckorlando]

The easiest thing to do if you want to use the offsets....

1)Post code for single part
2)Load material for 3 parts
3)touch off XYZ on part 1 and enter g54
4)Touch off X OR Y (depends which direction you moved the work. Most likely X) for the next part. Enter G55
5)Repeat step 4 as many times as needed for as many parts as needed.
6)Delete the G54 from the orig code, replace it with the correct number for the part. G55, G56, G57, G58

[mactec54]

Your program is a total re-write, not a duplicating code for identical parts. Sure that will work, if you have a single fixture that holds the multiple parts, but not so easy if you have separate fixtures, or are using separate vises. Your way would require re-writing the code every time, or careful alignment of the individual fixtures/vises if you wanted to set a job up again. G54-G59 won't care if the individual fixtures aren't perfectly aligned and have perfect offsets since each one has its own zero location.

The guy wanted to know how to use G54-G59 work offsets. The answer to that is not to rewrite the whole program to not use G54-G59. The answer is to tell him how G54-G59 are supposed to work.

They are 3 identical parts
I gave him 2 Choices how to setup his offsets G55 G56 Etc , and how to do it with X Y moves, if you have ever made EDM electrodes, which is what he was doing, then all you need is X Y moves to the next start point, depending on his software as to which way is the easiest for him to do it

[chuckorlando]

Yes they make identical parts. That does not make the code identical. You have 3 completely different codes written individually.

I dont see any code from you where you simply added a line to move it.

[mactec54]

Yes they make identical parts. That does not make the code identical. You have 3 completely different codes written individually.

I dont see any code from you where you simply added a line to move it.

No one said the code would be identical, the X Y moves are very clear at the start of each part, if you want to use the same program as the first operation then I gave him that choice by setting the work offset G55 and G56

[chuckorlando]

The man asked how to take his code and make 3 parts with that code. You said all he had to do was add one line of code.

So yea, thats kinda what we have been talking about.

Taking a prog from g54 to g56 and g57.... That would be, as I have said, identical prog except the work off set.

[chuckorlando]

" where ever you want it to start the next part you can just do a G0 Y0.X100 or what ever the spacing is"

No you can not.