Rigid tapping with OTC

[bob1112]

I did visit the offset page and there is no macro softkey at the bottom. There is a macro button on the key pad which brings up a mostly blank screen. I tried to enter the above code in MDI but MDI will not even allow character inputs, only numbers and select letters.

I will have to do some checking on parameters. I am hoping this is an easy bit change. Since the machine is pretty basic, I really need to add a few things to it.

[underthetire]

Well, almost 20 years working on/for mori, I can guarantee the old sl you have won't ridged tap without live tool. A few of the newer triple digit sl's could as a special order option, and usually only on the sl153/154 models. Im sure its available on the newer nl's as well. Those were integral spindles. Now, it's not to say you couldn't turn on the fanuc option and tweak parameters to make it work for a particular part weight. Mori sold it with the full c axis contour control, and by the time you paid for that, it wasn't much different in price to buy the live tool option.

[bob1112]

Normally, if the control does not have rigid tapping on the main spindle, then M19 is not possible. What do you mean "then times out"? With rigid tapping, M19 will orientate the spindle and hold it there until the spindle is started in program or MDI by M03/M04, or manually.

The P/S 10 alarm mentioned in your earlier Post mean improper "G" code, meaning that the control does not have that tapping cycle. parameter to call. On the machine I installed recently, Rigid Tapping was invoked in the same way it is on a machining centre. With a machining centre, there is a parameter to invoke Rigid Tapping with G84 or M29. When invoked with M29, the tapping cycle is still called with G84.

Regards,

Bill

I think M19 might be for what you mentioned which is to stop and "ready" the spindle for tapping as it seems to hold for about 10sec, then just says "time elapsed" or something indicating there is no alarm, it was just executed for a length of time.

Since it did not go to a fixed position, I wonder if peck tapping is even possible with this control. Might be handy for bigger taps, should I need it.

My code included an M29 line and G84. I single blocked through it and it errored only when G84 was invoked.

[bob1112]

Well, almost 20 years working on/for mori, I can guarantee the old sl you have won't ridged tap without live tool. A few of the newer triple digit sl's could as a special order option, and usually only on the sl153/154 models. Im sure its available on the newer nl's as well. Those were integral spindles. Now, it's not to say you couldn't turn on the fanuc option and tweak parameters to make it work for a particular part weight. Mori sold it with the full c axis contour control, and by the time you paid for that, it wasn't much different in price to buy the live tool option.

Could you answer questions regarding how to program around this issue, what the encoder ability truly is, and if a custom macro can help here?

I am just not sure why tapping was not in the big scene years ago. The machine is very capable otherwise. Rigid tap every day in VMCs without issue, even with gear backlash comps. The lathe does not have lash in the spindle and should be highly accurate. I can only imagine that the "canned cycle" operations are slightly tweaked to provide reduced decel rates to a target stop, and reversal of the feeds at spindle stop/reverse.

[underthetire]

Well, yes back then r tap on mori mills was standard. Not on lathes. The encoder is there only for feed per rev and single point threading. The 0 control was the base model, so everything was a purchase option from fanuc. Macro b was common on the mills, not on the lathes. The 0 would have had the s series spindle drive, without the orientation/c axis control card option. The upgrade control back then would have been the 15, and it was a few grand more. I know you don't want to hear the answer, but floating holders are really the only option, there is no simple programming around it. You could re configure the control, buy the rigid tap option parameter from fanuc, and tune the axis good enough to work, but you will have lots of time and money in it. This is one if not the main reason mori developed the mapps control, so they could add memory, USB, networking, and other options without forking over mass amounts to fanuc, and even run other controls behind the mapps like Mitsubishi and be transparent to the operator/programmer.

[bob1112]

OK, I do know the drive is S series without the feedback card on it. If I understand you right, there needs to be very tight control from spindle amp to spindle through the feedback (C axis) card? IE rigid tap is likely on possible with C axis on the spindle which is mostly pointless without live tool?

So when we lock up feed/rev and feed in/out, will a simple axial float holder get it done or do you need some auto reverse head and all that?

[angelw]

I did visit the offset page and there is no macro softkey at the bottom. There is a macro button on the key pad which brings up a mostly blank screen. I tried to enter the above code in MDI but MDI will not even allow character inputs, only numbers and select letters.

I will have to do some checking on parameters. I am hoping this is an easy bit change. Since the machine is pretty basic, I really need to add a few things to it.

Its unlikely that your control has the User Macro option. There are two types available, A and B. Type B is far more user, and has a syntax similar to Basic and Pascal. With either type, a Macro variable page will be in existence. Accordingly, if you can't find a Macro variable page, the control does not have that option.

The fact that you get the P/S alarm means that the G84 tapping cycle does not exist on your control. Its often that an error will not be raised with an "M" function that doesn't exist. Accordingly, don't get too excited that the control seems to accept M29. Any M code error messages are normally generated by the PMC (PLC) program, and is MTB specified.

Many machining centres use a Custom Macro program for execute a tool change. Not so with a conventional CNC Turning Centre with a tool turret. However, notwithstanding that the machining centre uses a Custom Macro program for the tool change, often the keypad supplied does not support inputting Macro statement. When this is the case, the work around is to write the program including Macro statements using a PC, then upload it to the control.

Regards,

Bill

[bob1112]

OK Bill, your Macro, info went over da head a bit. When hitting the macro button, a screen pops up but I cannot input anything, nor are there any variables there and if I understand you right, that page should contain variables?

Are you further saying that if we cannot enable the macro options in the machine, you can otherwise upload macro routines within a part program?

I can tell you a couple things that REALLY frustrate me with this machine is the lack of an unloader and no way to check to check tool breakage or cutoff. I need to be able to walk away from the machine but with cutoff concerns, I can't. Ran 500 parts one time. Finally walked away on the last 10 parts and wouldn't you know it.... Luckily minimal damage.

[underthetire]

All you need is a simple float holder also know as a compression tap holder. No auto reversing head is required. If you found one that only had .5 or less in/ out float you'd be fine.

[bob1112]

Can you offer sample code for this operation? All my CAM programs will want to output G84 so I might need to adjust my post for this machine.

[underthetire]

I always just did a g1 in reverse and g1 out. In inch per rev mode. There may have been a float tap cycle, I don't remember. The extent of my programing now days is setting up lasers and ballbars for the most part.

[angelw]

So when we lock up feed/rev and feed in/out, will a simple axial float holder get it done or do you need some auto reverse head and all that?

Bob,
Yes, a simple axial (Compression/Extension) holder will work.

On blind holes, when tapping close to the bottom of the hole, and where the tapping depth needs to be consistently controlled, a tap holder that has a freewheeling area is available. When consistency of depth is required with this type of holder, a dwell with G04 is programmed after the block containing the Z depth move, and before the spindle rotation is reversed. Most of these holders work via the process of the tap continuing to feed whilst the Z slide remains stationary due to the dwell.
1. The spindle of the holder extends until its drive pin inside the holder, finds an annular groove which allows the tap holder spindle to rotate freely with the machine spindle and workpiece.
2. When the spindle direction is reversed, the tap holder continues to rotate with the work until the drive pin engages in a drive slot on the Z minus side of the annular groove as the Z axis feeds in a plus direction away from the workpiece.

Are you further saying that if we cannot enable the macro options in the machine, you can otherwise upload macro routines within a part program?

No, the machine must have the User Macro executable available. It just may not have been supplied as an Option ordered by the customer. It may be available in the control for use by the MTB (for tool change Macro etc), but because the machine is basically being supplied without the Option, the User Macro inputs via the keypad are not supported. In this case you can write a Macro program via a PC. But if you control doesn't have a Macro variable page where values can be registered, then your control effectively does not have the option. In this case a Macro program will be rejected by the control, even though the syntax may have been correctly written using a PC.

Following is an example of coding the tapping process in the CNC program. Depending on the MTB, the spindle reverse may have to be programmed as in Example 2. Write a sample program and observe the operation with the program cycling in fresh air.

Use G32(G code system A), G33(G code system B) instead of G01 to inhibit Feed Rate and Spindle Speed Override.

(Metric Example 1)
T0101
G97 S600 M03
G00 X0.0 Z5.0
G32 Z-20.0 F1.5
Z5.0 M04
G28 U0.0 W0.0
M01

(Metric Example 2)
T0101
G97 S600 M03
G00 X0.0 Z5.0
G32 Z-20.0 F1.5
M04
Z5.0
G28 U0.0 W0.0
M01

Regards,

Bill