HAAS DS30 SubSpindle Machining Help

Hello all,

We have a new DS30 here at our shop, and I'm trying to run half of my part in the main spindle, and the second half on my secondary spindle. I got the main spindle down, I'm having an issue trying to machine on the secondary spindle.
I have read in the manual that we can use the G14 Spindle Swap code to make all of the main spindle codes applicable on the secondary spindle. This G14 also activates Z axis mirroring. Is there any way to use the G14 without the mirroring feature?
I have tried to machine on my secondary spindle without using the G14 and just turning on the spindle with it's own appropriate G code. The spindle starts up and the tool will position (G00) correctly, but at reading it's first feed (G01) command, the machine gives a "spindle not turning" alarm, when it actually is. Does anybody have any feedback on this?

I'm sure I can get it to work with the mirror feature, but the big boss doesn't really like the idea. We are not using mirror on any of our Mori machines, so we'd like to keep it the same across the board. That's the only reason I'm looking into this.

Thanks

I take it that you are programmed in IPR?

There has to be a code that tells the control to read the rpm from the sub instead of the main. "Spindle Swap" sure sounds like the right description for that, but I don't run HAAS, nor know their codes.

No idea about the "mirroring".


Unless your threading - I would trhink that you could feed in IPM and git your parts running.


-----------------

Think Snow Eh!
Ox

RE: Subspindle

Have you considered turning on the main spindle also?

I have tried programming both IPM(G98) and IPR(G99) to see if I would have different results, but to no avail.

The thought of turning both spindles has crossed my mind, but I really wouldn't want to turn it for nothing.

I came across something in the book today that I'm going to try. It says:

"The G14 command will automatically activate Z-axis mirroring. If the Z-axis is
already mirrored (Setting 47 or G101) the mirror function will be canceled."

I'm going to try and turn on the mirror function with the G101, and then try the G14 and see if the mirror turns off.

I appreciate your joint input, and I'll let you all know what comes of it.

Thanks again.

I think I'd call Haas by now.

Our ideas were only to git you rolling for the night or weekend or ???

For longterm fix - find out from HAAS how it's sposed to be done.


----------------

Think Snow Eh!
Ox

You do not need to mirror anything, you can run the secondary spindle independently. Send me a backup of this machine and I can tell you the problem. [email protected]

To backup machine:
LIST PROG
USB
F4
Save All

Gravedigging here, but this is what popped up when I searched for this problem.

To cut on the sub spindle on a Haas you need to commmand G14 to let sub spindle take control. But doing so also mirrors your program in Z. This is so you can program as though you are machining on the main spindle.

If you program like everyone else for the last 30 years and have all your cuts going in the positive direction. You need to command G101 Z0 to Mirror the program a second time to get it to cut the way it should.

Why Haas had to be different if beyond me. It just adds to the long list of why Haas' are not good machines.

Example:
(FINISH FACE)
N3 T0315
G14 <--- Spindle swap to Sub Spindle, mirrors current program.
G101 Z0 <--- Mirrors the program in Z to put it back to the correct direction.
G55
G18 G99
G97 S1063 M04 <--- Command Spindle as if you're running the main spindle.
G0 X1.2579 Y0. Z0. B0. M8
G50 S2000
G96 S350
G1 X-.0313 F.0035
G0 Z-.1
(FINISH OD)
X1.0697
Z-.0173
G1 X1.0897 Z0.
X1.0956
G2 X1.1248 Z.006 I0. K.0206 F.0005
G1 X1.2379 Z.0626 F.0035
G2 X1.25 Z.0772 I-.0146 K.0146 F.0005
G1 Z1.7941 F.0035
G2 X1.2379 Z1.8086 I-.0206 K0. F.0005
G1 X1.1394 Z1.8579 F.0035
G3 X1.131 Z1.868 I.0102 K.0102
G1 Z2.0506
G3 X1.1598 Z2.065 I.0144 K0.
G1 X1.2127
G2 X1.254 Z2.0856 I0. K.0206 F.0005
G1 X1.2886 Z2.0956 F.0035
M9
G97 S1037
T0300
G0 G59 X0. Y0. Z0.

NINE year old post.

machineit2 said:

NINE year old post.

Click to expand...

So? I had this same problem and wanted to share my solution for fixing it. Did you even read the first line of my post?

Metzenw said:

Gravedigging here, but this is what popped up when I searched for this problem.

Click to expand...

To me, that means I was well aware of the age of this post. Also indicated that I used the search function and discovered this post that didn't have a clear answer. I than provided a solution to the problem that I'm sure other people have experienced.

If I had said something to the effect of "Did you solve this yet?" or "I have the same problem, Help!" Then your comment would have been warranted.

At least I made a contribution with my post. Where's yours?

Metzenw said:

At least I made a contribution with my post. Where's yours?

Click to expand...

Oh Oh, newbie mad at me, I better quit the forum.

Just so you know, it is much better to state a problem and then post the solutions you have for it. It is much better than resurrecting an old post,(some of which can be many multiple pages long)and thus requires the reader to read pages of comments to catch up to your answer.

Just saying, but I stand chewed out.