|
|
|
|
|
 |
The Collected Wisdom
of the Haas
Answer Man |
| |
|
|
Haas Rotary
Products |
|
|
|
Semi
5th-Axis Positioning
(Fall
’04
vol 8 #
31) |
 |
|
Dear Applications:
|
We recently purchased
a VF-5 and a TRT-210 two-axis tilting rotary table. This option required
the additional purchase of a 4th-axis drive,
|
 |
|
and included the separate servo unit that can also be used
on non-Haas machines.
|
 |
|
I have been assigned
to do the programming for this, and would like an example of how to
program the 4th and 5th axes. Since we do not have true 5th-axis
capabilities with this configuration, is the 5th axis controlled by M code
in the program, with a separate sub-program?
Ken Miller
|
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
|
• • •
|
4th
Axis at Home
(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
|
|
Indexing vs Full 4th Axis
(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
|
• • •
|
4th-Axis Feeds
(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
|
• • •
|
Setting 30
(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 |
 |
|
• • •
Cylindrical Mapping
/
Engraving
with a Rotary Table
(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
|
• • •
[ Home ] [ MachineCare ] [ Communicate ] [ FeaturesOptions ] [ MiniMachines ] [ MiscTopics ] [ Offsets ] [ Productivity ] [ Programming ] [ Rotary ] [ Thread/Tap ]
Search CNC Machining On-line!
|
|