[jabbo]

Hey we got this old school and rebel AC2100 Milling machine-Vickers Acramatic CNC MC Control, and we are planning to machine four parts that are exactly the same. The thing is that we are having a hard time to know how to machine them in such efficient way using one tool at a time to machine all 4 of them, and the next tool do the same thing. TOOL EFFICIENCY is what I mean. Thanks a lot!

Sincerely,

A young CNC programmer.

[fordav11]

if you are mounting 4 parts on the table just do each operation with the current tool on each part in order. use G54 G55 G56 G57 to shift the workshift to the X0 Y0 of each part then run the program again. You can do that with a main and sub program.

%
O1000 (MAIN PROGRAM)
G54 (workshift X0 Y0 for 1st part)
M98 P1001
G55 (workshift X0 Y0 for 2nd part)
M98 P1001
G56 (workshift X0 Y0 for 3rd part)
M98 P1001
G57 (workshift X0 Y0 for 4th part)
M98 P1001
G54
M30
%

%
O1001 (SUB PROGRAM)
(put here all of the program to machine the part)
...
.....
........
...........
G91 G28 X0 Y0 Z0
G90
M99
%


if you don't have multiple workshifts (G54-G59) you can use G92 X... Y.... instead

[jabbo]

Hey thanx a lot for taking time and reply to my question!

I'll try what you said right know and let you know if it works. I thought that G54...G59 were not supported by this machine since when we generate the CNC code in FeatureCam it replaces such G to an H letter.

Whatever happens I'll let you know.

-Jabbo

[jabbo]

Man it did not work, the machine has: Vickers Acramatic 2100 CNC MC Control.
And also, can you explain me how is that Main program and Sub program works?

The way we programmed was via the machines multisetup screen. we did not do it thru FeatureCam. I do not know if that is a problem. How the machine works is like this:

the program has only two tools.
it machines on "piece" using the two tools
then, M2
and starts over but with the next set ups [2,3,4]

[chucker]

Use one setup then use H2 ,H3 ,H4 instead of the G55,G56,G57 push the offset key on the right side of the screen the 1st table will be your setup numbers the lower left one is fixture offsets here is where you you would put your shift from the orignal setup that would be your H offsets the table on the right I never use I think it is for pallet offset if you have more than one pallet.
Hope this put you on the right track
Sorry if my explaination is a little off I dont run the 2100 every day any more.

[jabbo]

If I post the code would it be helpful?
thanks for the help! I just wonder if I have to do a main program and a subprogram. I could not find the key on the screen. you mean the offsets button? hey man thanks! I tried G codes but did not work, do I have to copy each tool block cycle? arghhh I am all frustrated, but we will win this u.u

[fordav11]

post your program and we'll try to see what's going on. for main/sub you need to have 2 programs in memory. on your old piece of crap you can have 2 programs in memory, right?

[John_B]

I do run one of a machine with an A2100, and Chucker has it right basically. On the Set-up screen you want to create one set-up (doesn't matter if it has an offset in it or not), then create a fixture for each workpiece position. Each fixture will be use a workshift starting with H1, then H2, and so on...

Then when you're programming, you make one paragraph for each tool that moves it between each fixture:

:T1M6
G0G90H1X0Y0S500M3
Z.25M8
G1Z-1.F5.
X5.F20.
...
G28 (GOTO TOOLCHANGE HEIGHT)
G0G90H2X0Y0
Z.25
G1Z-1.F5.
X5.F20.
...
G28 (GOTO TOOLCHANGE HEIGHT)
M01
:T2M6
G0G90H1X0Y0S500M3
Z.25M8
G1Z-1.F5.
X5.F20.
...
G28 (GOTO TOOLCHANGE HEIGHT)
G0G90H2X0Y0
Z.25
G1Z-1.F5.
X5.F20.
...
G28 (GOTO TOOLCHANGE HEIGHT)


(ETC.....)

This is a simplistic example, but it should get you started.

Rgds,
John B

[fordav11]

Ah yes. Years ago I worked an old Toshiba mill with Tosnuc 600 control that used H for fixture offsets.
It's all coming back now.... (the nightmares)