|
|
 
|
|||||||||||||||
|
|
CNC Machining Magazine | |||||||||||||||
|
|
||||||||||||||||
|
Dear Richard: The Graphics mode is the safest way to check a programmed tool path. You could also try using the handle feed override while in Memory mode; this is useful when setting up a job where the tool comes close to the chuck (within a couple thou’). Single-block through the program and override the feed to a stop if you want, then check your “distance to go” on the Current Commands page. You can feed hold and stop the spindle to make sure the distance to go doesn’t exceed the gap between the tool and the chuck jaws. This method is better than using Dry Run, because you can slow the feed down to 1% (or 0%) and react quicker if it looks like the tool will cut into the face of the jaws. To review: 1) Run the program in Graphics to check the tool path. 2) Run the program in Memory, with rapid override at 5%, and use the jog handle for feedrate override. Use the “distance to go” display on the Current Commands page to compare tool position relative to the workpiece (the spindle may be stopped at any time to check the gap). 3) This is also a good time to make sure other tools and index points clear the workpiece, chuck and tailstock.
Another alternative is to turn on Setting
103, so that the Cycle Start and Feed Hold functions are both controlled
by the CYCLE START button. Hold the button in and the program runs;
release it and the machine stops in a feed hold. This is a very useful
setting, but remember to turn it off when you’re through using it. •••
Is it possible to cut multiple start
threads on an SL-30? If so, how? Dear Carter: Yes, you can cut multiple start threads on an SL-30 – and on every other Haas lathe. Just change the start point of each threading cycle. For example, to cut a two-start 1”-8 thread:
(Note: 0.250" lead ÷ 2 starts = 0.125" Z shift from original start point) Here’s something else to think about: Watch your feedrate! (MMSonline.com says it so well, we’re quoting them almost verbatim.) While the machine’s maximum feedrate is more than adequate for most machining applications, occasionally it can be a limiting factor. When threading on a turning center, for example, it is possible to unwittingly exceed the maximum feedrate. Say a turning center has a max feedrate of 300 ipm (with 600 ipm rapids). If you’re machining fine threads in large diameters, you are not likely to exceed the max feedrate. A 3.0"-16 thread machined at 300 sfm, for example, would require a feedrate of 23.88 (3.82 x 300 [sfm] ÷ 3.0 [dia] x 0.0625 [pitch]). This relatively slow feedrate is allowable on all current CNC turning centers.
On the other hand, when machining coarse threads at high speeds, you do
need to worry about maximum feedrate. And multiple-start threads present
the most problems, since the lead of the thread (not the crest-to-crest
pitch) determines the feedrate. Say you’re machining a four-start 1.25"-4
thread having a lead of 1" (0.25" crest to crest) at 600 sfm. Now, the
required feedrate becomes 1,833.6 ipm (3.82 x 600 [sfm] ÷ 1.25 [diameter]
x 1.0 [lead]). This exceeds the capabilities of even the fastest CNC
turning centers. •••
Dear Gerry:
The B-2.0 in the program examples is to
position the sub-spindle (the B axis). The B command or “address” is where
the sub-spindle will be when you set offsets for the second operation on
the workpiece. Part size is what dictates the B-axis starting point, so
this number will be a constant in programs for similar-size parts, where
you want to start the sub-spindle work at the same point every time. If B
were set to 0 in the program, all of the second-op machining would be done
at the far end of the machine. Moving the second-op starting point closer
to the main spindle (2 inches closer in this example) reduces cycle time
by reducing the distance the turret has to move. ••• I’m wondering if there’s a faster way to do tool changes on my Haas VF-2. Here’s the sequence I’m using:
M05
Is this the best way to do it? Dear Brian: Actually, all you have to do is program an M06, and the Haas control will take care of everything else. When the Haas CNC reads “M06,” it will:
1) retract the Z axis to the tool change
position; Presto change-o! It’s not quite magic, but it is faster.
TIP: For super-fast tool changes on a
VF-2, check out the new Haas VF-2SS, a high-speed machine with a
tool-to-tool change time of 1.6 seconds, a 12,000-rpm spindle and 1400-ipm
rapids (for details, see
www.haascnc.com/news/new_machines.asp). •••
When dealing with arc moves while cutting
circles, is there a minimum straight line move required to have cutter
compensation work? Dear Dan: The short answer is “yes.” Cutter compensation can only be turned on and off in G00 (rapid) or G01 (linear) mode. After you’ve turned it on and before you start cutting, you must make a linear move that is the same or greater than the radial compensation value in your offset. If your radial cutter comp is set at 0.5”, for instance (for a 1” diameter tool), then you must make a linear cut of at least that length before you start cutting. Here’s how the program would look:
Sincerely, •••
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? Dear Dave:
Here’s how it works: 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
Sincerely,
|
||||||||||||||||
On-line!