[69ss396]

we have a new VF-1 and it has the 5c indexer that plugs into the back of the machine. I am having trouble to get it to index with the program. I was trying Saturday to mill 2 wrench flats on a round part and I could not get it to index with the program. I can index it manually or in the MDI page but I can not get it to work in the program does anyone have a program format for a simple program like the one I was just needing.

[makingchips]

I just did somthing quick with the 5 axis post. I have not even run my new Haas yet. I told MC that this was just a 4th axis move and this is what it gave me.


hope it helps.

%
O0000 (HAAS TEST)
(HAAS VF 5AX TABLE)
(OPERATION-1)
(MASTERCAM - X)
(MCX FILE - TEMP)
(MATERIAL - NONE)
(PROGRAM - HAAS TEST.NC)
(DATE - DEC-01-2008)
(TIME - 11:17 AM)
(POST DEV - IN-HOUSE SOLUTIONS)

(T1 - 1/4 BALL ENDMILL - H1 - D1 - D0.2500" - R0.1250")
G00 G17 G20 G40 G49 G80 G90
G54 X-25. Y-9. (TOOLCHANGE POSITION)
(TOOLPLANE NAME - TOP)
T1 M06 ( 1/4 BALL ENDMILL)
M11 (B-AXIS UNLOCK)
M13 (A-AXIS UNLOCK)
G00 G17 G90 G54 A0. B0.
G00 X-.125 Y-2. S2139 M03
G43 H1 Z.75
G94 Z.6
G01 Z.5 F15.
Y-1.9 F25.
Y-1.8
Y-1.7
Y-1.6
Y-1.4999
Y-1.3999
Y-1.3
Y-1.1999
Y-1.0999
Y-1.
Y-.9
Y-.7999
Y-.7
Y-.6
Y-.5
Y-.4
Y-.3
Y-.2
Y-.1
Y-.0001
Y.1
Y.2
Y.3
Y.4
Y.5
Y.6
Y.7
Y.8
Y.9001
Y1.0001
Y1.1001
Y1.2
Y1.3
Y1.4
Y1.5
Y1.6
Y1.7
Y1.8
Y1.9
Y2.
G00 Z.6
Z.75
G91 G00 G28 Z0.
G00 G90 A180. B0.
X-.125 Y-2.
G43 H1 Z.75
Z.6
G01 Z.5 F15.
Y-1.9 F25.
Y-1.8
Y-1.7
Y-1.6
Y-1.4999
Y-1.3999
Y-1.3
Y-1.1999
Y-1.0999
Y-1.
Y-.9
Y-.7999
Y-.7
Y-.6
Y-.5
Y-.4
Y-.3
Y-.2
Y-.1
Y-.0001
Y.1
Y.2
Y.3
Y.4
Y.5
Y.6
Y.7
Y.8
Y.9001
Y1.0001
Y1.1001
Y1.2
Y1.3
Y1.4
Y1.5
Y1.6
Y1.7
Y1.8
Y1.9
Y2.
G00 Z.6
Z.75
M05
G91 G00 G28 Z0.
G90 X-25. Y-9. (TOOLCHANGE POSITION)
M10 (B-AXIS LOCK)
M12 (A-AXIS LOCK)
M30

MC

[HuFlungDung]

Well, you have it plugged in and operational, so I guess that must mean you didn't blow up the drive by plugging it in 'hot'

Here is what I do: ESTOP, go to settings and select the proper indexer from the list, and also input the OD of the part if I think of it at this time.

Then, still in ESTOP, plug the indexer cable in. Remove the ESTOP and clear the alarms. Then go to Zero Return mode, hit A and then zero single axis. This will home the indexer. You might see an alarm sometimes during this initial homing. Just clear it and try again.

After that, make sure that you use G00 mode with your commands

G00 A180.
G00 A0.

If you command in G01 mode, it may not move if no feed was in effect or if the diameter of the part was input as zero.

[Geof]

First question: Is it turned on in the Settings? If the machine does not know the 4th is connected it will not use it.

An easy way to check is go to the Work Offset page and see if there is a column for the A axis, if there is it is turned on, obviously.

Do you need your wrench flats in a specific place? If so you will need to enter a Work Zero for A, which simply means moving the A axis to the correct position and enterning the value the same as for all the other axes.

With or without a work zero entered the command G00 A0.0 will move the A axis to the zero position; this will be machine zero if there is no work offset entered and it will be the G54 zero if there is a value in the G54 line for the A axis.

G00 A180.0 will index the A axis 180 degrees and any other value will index it by that value.

The key sequence SINGL AXIS, A, G28 will home the A axis.

Incidentally when you are just indexing the axis it is not necessary to worry about unlocking the brake or anything like that, actually I think the 5C rotary does not have a brake.

[69ss396]

Thanks that helped a lot. I am used to using a seperate control and using a m code to index. I am not at all used to the Haas mill yet

[littlerob]

I am used to using a seperate control and using a m code to index.

Me too, and I really, really hate it. You will really, really like the A axis.