The Collected Wisdom
of the Haas Answer Man

Haas Rotary Products

(Fall ’04
vol 8 # 31)

Dear Applications:

Dear Ken: 

With a full 4th axis and semi 5th axis setup, 4th-axis positioning is done with a standard A address code. There are two ways to “position” the 5th axis. One method, as you suggested, is by assigning it an M code from the spare M-function user interfaces. An alternative method, which adds a lot more functionality, is to use Setting 38, Auxiliary Axis Number. This setting is used to select the number of external auxiliary axes added to the system. (Up to four may be added: C is a rotary axis, and U, V and W are linear.) When you use Setting 38, the auxiliary axes must be connected through the CNC mill’s second RS-232 port (the bottom one) to the rotary servo control unit.

If Setting 38 is set to 1, a C axis is assumed, so you can control the 5th axis by using C address codes in your program. In addition, using Setting 38 allows you to move the C axis with the jog handle on the mill control, and the mill Position display will show the current position of the C axis.

Please consult your VF Operator’s manual for more detailed information about auxiliary axes.

Sincerely,

Haas Applications

(Summer ’04
vol 8 # 30)

Dear Applications:
      On the VF-0, I can zero the A (rotary) axis and it will zero out in less than one revolution. This is useful for a restart after doing multiple rotations in one direction. When I attempt the same thing on the Super Mini Mill, it seems to go all the way through several revolutions. Can the Super Mini Mill Zero Single Axis perform the same function as on the VF-0?
      Gil Stein

Dear Gil:
      Sure it can. Your Super Mini Mill probably does not have Setting 108 (Quick Rotary G28) turned on. With this setting on, the G28 command (Zero Return thru Ref Point) will cause the machine to unwind from 361 degrees to 0 degrees by unwinding 1 degree. Note that if the rotary is at less than 360 degrees, it will unwind the entire amount – if it’s at 359 degrees, it will unwind 359 degrees to go to A0. Also, if the rotary is at 630 degrees, it will zero out by unwinding 270 degrees, not by moving forward 90 degrees. This feature eliminates the need to unwind more than 1 revolution.
      Finally, with Haas mill software versions 12.03 and later, turning on Setting 108 also requires a parameter change. Most parameters can only be changed by Haas Service personnel, but you should be able to turn on Parameter 43, bit 11, Circ Wrap, by changing its value from 0 to 1. Call your local dealer or the Haas Service department if you need help with this.
      Sincerely,
      Haas Applications

• • •

Dear Applications:

When I power up my older VF-0 , my 5C Haas rotary only goes about 7 degrees to find home. I have a new HA5C that always goes to home, no matter where it had stopped. What is the difference?

Rick Connelly
 

Dear Rick:

Older 5C rotary products did not have a home switch; they only used the “per rev” signal from the motor (about 5 degrees, actually). New HA5Cs and other rotary products all have a home switch.

Sincerely,
Haas Applications

(Summer ’03
vol 7 # 26)

Dear Applications:

If I hook up an auxiliary axis on my Haas VF-3, can I use it like a full 4th axis, or just as an indexer? My VF-3 does not have a 4th-axis option. The auxiliary axis is an HRT160 Haas indexer with the red control box.
    Jose Garcia

Dear Jose:

When you connect a rotary product, such as the HRT160, as an auxiliary axis without the 4th-axis control option, you will not have 4th-axis interpolation – that is, the 4th-axis motion will not occur simultaneously with movement of the other 3 axes.

Still, using your HRT160 for indexing can save you a lot of setup time. For example, you could machine four sides of a block with one setup. You can also program the auxiliary axis (C axis) through your VF-3 control, either in a program or in MDI. You could, for example, mill a slot around the circumference of a bar by programming a C-axis move with a feedrate.

If you need to do true 4-axis machining, you will need to have the 4th-axis option installed on your machine.
    Sincerely,
    Haas Applications

(Spring ’03
vol 7 # 25)

Dear Applications:

I have a VF-3 with a 4th axis (an HRT model). I want to rotate the A axis 1,088 degrees, while feeding the Z axis -0.50” and the X axis 0.25” for each 360 degrees of A-axis movement. Can you help me program this?
     Dave Coffey

Dear Dave:

Here’s how it works:
1088 ÷ 360 = 3.0222
0.5 x 3.0222 = 1.5111                           (distance move in Z = -1.5111)
0.25 x 3.0222 = 0.7556                         (distance move in X = 0.7556)

So you would write the program as follows:

G01 X0.7556 Z-1.5111 A1088.0 F20.0

although the feedrate, of course, will depend on the diameter of the part
(Setting 34), the material you’re cutting and the tool(s) you’re using.

     Sincerely,
     Haas Applications

(Spring ’02)
vol 6 # 21)

Dear Applications:

I have a Haas indexer semi-permanently installed on my VF-2 mill. When removing or re-installing the indexer, I have to change Setting 30. Can I avoid changing this setting if I’m always using the same indexer?

     Joe Coehlo

Dear Joe:

The reason you have to change Setting 30 each time you connect your indexer is because it turns off the logic connection to the amplifier. If you leave the setting on, turn off the power and physically disconnect the table from the machine, then turn the power back on, the machine won’t run correctly. It will alarm out and remain in the alarmed state until the setting is turned off.

When Setting 30 is on (set to the rotary product you’re using), the machine is looking for feedback – a status report – from the table or indexer.

The machine parameters change automatically according to the model number given in Setting 30. Every Haas rotary product has a specific set of parameters that need to be loaded for it to work correctly. Setting 30 needs to be set to the appropriate model for this to occur.      Sincerely,      Haas Applications

(Spring ’02)
vol 6 # 21)

Dear Applications:

A job that I am doing requires engraving around the circumference of the work using a Haas HRT 210 rotary table on a Haas VF-2. Can this be done using a G107 command along with a G47? If so, is there anything else needed in the program?

     Mark Mensch

Dear Mark,

G107 will work for this. You can find a detailed explanation of the use of this command in the G code section of your user’s manual (we’ve listed the main points below). All you need to do is set up the G107 first, and then call G47 for engraving.

G107 (CYLINDRICAL MAPPING) translates all programmed motion occurring in a specified linear axis into the equivalent motion along the surface of a cylinder (attached to a rotary axis). Its default operation is subject to Setting 56 (M30 RESTORE DEFAULT G). The G107 command is used to either activate or deactivate cylindrical mapping. Remember to turn it off at the end of the program, unless you want to keep using it.

• Any linear-axis program can be cylindrically mapped to any rotary axis (one at a time).

• An existing linear-axis G-code program can be cylindrically mapped without modification by inserting a G107 command at the beginning of the program.

• The radius (or diameter) of the cylindrical surface can be redefined, allowing cylindrical mapping to occur along surfaces of different diameters without having to change the program.

• The radius (or diameter) of the cylindrical surface can either be synchronized with or be independent of the rotary axis diameter(s) specified in the Settings page.

     Sincerely,
     Haas Applications