Need Help!- programing tool length offset in a 3axis mill

[bert4255]

programing tool length offset in a 3axis mill/. it is vickers acramatic pc2100. does this code look right for tool changes with offsets. i was told to use H code but my manual which is useless says use a O code. i've tried for several days and still cant figure out my tool offsets. i've set all tools offsets in the control, does it have to be in the code as well? does anyone have some code i can see to compare mine with? i'm using bobcam v23. the mill is a tree journeyman 250. it i set up one tool the machine is great. i just have to figure out the tool change codes and offsets.
please help. mschrowang@nycap.rr.com

:100

N01 G17 G40 G70 G80 G90 G94 G97

N02 M06 T2
N03 O2
N04 G00 G90 X3. Y0. S201 M03
N05 Z.1 M08
N06 G81 X3. Y0. Z-.08 R.1 F.4034
N07 X0. Y3.
N08 X-3. Y0.
N09 X0. Y-3.
N10 Z.1
N11 G80
N12 M09
N13 M05

N14 M06 T3
N15 O3
N16 G00 G90 X3. Y0. S323 M03
N17 Z.1 M08
N18 G83 X3. Y0. Z-1.5381 R.1 Q.2715 F.9708
N19 X0. Y3.
N20 X-3. Y0.
N21 X0. Y-3.
N22 G00 Z.1
N23 G80
N24 M09
N25 M05


N26 M06 T4
N27 O4
N28 G00 G90 X3. Y0. S238 M03
N29 Z.1 M08
N30 G84 X3. Y0. Z-1.3636 R.1 F.0909
N31 X0. Y3.
N32 X-3. Y0.
N33 X0. Y-3.
N34 G00 Z.1
N35 G80
N36 M09
N37 M05


N38 G00 Z.5
N39 X0. Y6.
N40 M02

[sti2011]

Not familiar with your type of machine at all but using O instead of zero on a Fanuc is all wrong. A Fanuc would require:G43 H2. G43 turning on length comp and H as the tool length offset. If this works you may need to use G49 before sending the tool home to turn off length comp. I would put it in your first z posit move.(this may or may not work on your mach)

[sti2011]

Put the G43 H? on you first Z move and put the G49 on your last Z move home. I re-read what I wrote and it could be confusing. There is most likely a G code list in your manual look for one that turns on length comp.

[1234567]

try this
%
O100


N01 G17 G40 G70 G80 G90 G94 G97

N02 M06 T2
N04 G00 G90 X3. Y0. S201 M03
N05 G43 H2 Z.1 M08( PICK UP TOOL OFFSET)
N06 G81 X3. Y0. Z-.08 R.1 F.4034
N07 X0. Y3.
N08 X-3. Y0.
N09 X0. Y-3.
N10 Z.1
N11 G80
N12 M09
N13 M05
M14 G49

N14 M06 T3
N16 G00 G90 X3. Y0. S323 M03
N17 G43 H3 Z.1 M08
N18 G83 X3. Y0. Z-1.5381 R.1 Q.2715 F.9708
N19 X0. Y3.
N20 X-3. Y0.
N21 X0. Y-3.
N22 G00 Z.1
N23 G80
N24 M09
N25 M05
N25 G49


N26 M06 T4
N28 G00 G90 X3. Y0. S238 M03
N29 G43 H4 Z.1 M08
N30 G84 X3. Y0. Z-1.3636 R.1 F.0909
N31 X0. Y3.
N32 X-3. Y0.
N33 X0. Y-3.
N34 G00 Z.1
N35 G80
N36 M09
N37 M05
N37 G49
N37 G28 91 Z0.
N27 G28 G91 X0. Y0.
N40 M30
%

[christinandavid]

Hi,

Have run this control. It is very confusing with many levels of tables of offsets for tools, fixtures, tram lengths and god knows what else. Pretty sure that it all depends which table you use. We kept it simple. As I recall, the way we ran it I am pretty sure we had to put the Tool DIAMETER into the tool table we used (which may have been called automatically, or with O, can't remember). I am also pretty sure that H and D offsets were extra offsets in a different table that you could use if required. Its been a few years so its all a little bit hazy...

Also recall this control being a pain in the ass if you defined the tool form as it would then only run certain cycles - and it had dozens of cycles, for every conceivable strategy (most of which were impractical to use). If I ever had to do circular pockets on it I always programmed it long hand so I could get it up and running with the minimum of fuss.

It has got a funky windows like touch screen control though and the mc we had a remote pendant that you virtually had to strap to your arm, it had thousands of buttons all over it.

DP

[bert4255]

Originally Posted by christinandavid Hi, Have run this control. It is very confusing with many levels of tables of offsets for tools, fixtures, tram lengths and god knows what else. Pretty sure that it all depends which table you use. We kept it simple. As I recall, the way we ran it I am pretty sure we had to put the Tool DIAMETER into the tool table we used (which may have been called automatically, or with O, can't remember). I am also pretty sure that H and D offsets were extra offsets in a different table that you could use if required. Its been a few years so its all a little bit hazy... Also recall this control being a pain in the ass if you defined the tool form as it would then only run certain cycles - and it had dozens of cycles, for every conceivable strategy (most of which were impractical to use). If I ever had to do circular pockets on it I always programmed it long hand so I could get it up and running with the minimum of fuss. It has got a funky windows like touch screen control though and the mc we had a remote pendant that you virtually had to strap to your arm, it had thousands of buttons all over it. DP

my machine does not like g43? what do i use?

[mactec54]

Hi bert4255
Try parts of this as it should work, This is not your program ,but you could put yours together like this.

:G90
M6 G40 T1
S484 M3
G0 X9.888 Y9.777 Z1.
G0 X0.573 Y1.95
Z0.1
G1 Z-0.122 F5.
G41 T1
X0.575 F10.
G3 X0.875 Y2.25 P0.3
G1 Y3.
G2 X1. Y3.125 P0.125
G1 X1.3584
G2 X1.6038 Y2.9228 P0.25
G3 X2. Y2.5964 P0.4036
X2.3962 Y2.9228 P0.4036
G2 X2.6416 Y3.125 P0.25
G1 X3.
G2 X3.125 Y3. P0.125
G1 Y1.5
G2 X2.5 Y0.875 P0.625
G1 X1.5
G2 X0.875 Y1.5 P0.625
G1 Y2.25
G3 X0.575 Y2.55 P0.3
G40 T
G1 X0.573
G0 Z0.1
Z1. M5
M6 G40 T3
S765 M3
G0 X9.888 Y9.777 Z1.
G0 X2.5 Y1.5
G81 Z0.1 P Q-0.122 E0.1 F12.
X1.5
X2. Y2.
G80
M6 G40 T4
S888 M3
G0 X9.888 Y9.777 Z1.
G0 X2.5 Y1.5
G83 Z0.1 P Q-0.122 F14.
X1.5
X2. Y2.
G80
Z1.
M2

[christinandavid]

Your machine may not even need G43. Seem to recall that tool length offset was loaded automatically even when calling tool with a Tn M6 in MDI (Z coordinate displayed would alter to suit tool in spindle as soon as M6 was complete).

DP

[tobyaxis]

Siemens Vickers Acromatic 2100 does not use a G43 or a Height Offset.

Set your tools to a Known Height then Touch one tool to the top of the work.

In your program all you need is T1M6 and the Set-Up information does the rest. I have to double check a few things but this is how most 2100 controls work.

BTW: Arcs are programmed with a "P" Designation not "R". You can use "I" and "J" as well.

[bert4255]

Toby, how do u input tool lengths? do u calculate the lengths by using the digital z readouts and entering the numbers manually in the tool manager or do you use the fetch option or mdi t1,t2? every time i do it either way i get different numbers? what is the proper way?
thanks
Marc

[christinandavid]

Hi,

Believe that Length Offset is loaded automatically on M6 command (even in MDI) so you can't go by what the Z-axis co-ordinates are, as that figure will be relative to the length currently in the table. The only way you could do it this way is to reset all lengths in your tool table to zero (along with your work offset Z values) and measure new tool by touching on your 'Tram position'. I suggest you use 'Fetch' (sounds familiar).

I assume you have set a 'Tram Length' to the spindle-nose (I ran ours for 6-months before someone pointed this out to me and from then everything started making sense)?

DP

[tobyaxis]

Originally Posted by bert4255 Toby, how do u input tool lengths? do u calculate the lengths by using the digital z readouts and entering the numbers manually in the tool manager or do you use the fetch option or mdi t1,t2? every time i do it either way i get different numbers? what is the proper way? thanks Marc

Be in MDI MODE
Call the tool on the Key Board : T1 M6
Cycle Syart
Hit the SET UP Button on the Handle
Bring you tool down to Zero (top of the work if your programming Z- in the program for depth )

Then Hit Tool Set on the Handle.

This should be it. I have not worked on one of these in a while, and even then it was very brief.

Do you have a Manual for this Machine??