[bob1112]

I understood that our machine could rigid tap. Upon running a test G84 cycle, machine errors with p/s 010 on G84 line. there is also no G84 cycle listed in the manual. Can anyone confirm if the OTC can rigid tap and if so, what are we missing?

If not, how else can we get around this? Machine has encoder on spindle and motor and should have no problem with the feedback part. Tap heads do NOT excite me...

[underthetire]

Sure a OTC can rigid tap, however most lathes will not, unless they have live tooling. Too much mass difference between parts, and collet chucks/ power chucks, so it make them hard to dial in. Maybe post the machine brand, might help.

[bob1112]

Machin is Mor Seiki SL series. Spindle is direct driven with belts to motor and encoder is directly on spindle. Should do it flawlessly I would think.

[underthetire]

Nope. I can say for sure it won't. Not without live tooling.

[cadman@teluspla]

I know you say tap heads do not excite you.
However you can tap very easily on a machine with an OT-C control
but you will need a floating tap holder, not much expense for a lot of work.
If you wish I can post a sample program
Best regards
Chris j.

[bob1112]

I thought there was a way to use feed/rev and lock out feed/speed overrides to repond similar to G84? What would a sample program look like and what will the difference be? I know people say you need a tap head but never say what the machine will do differently than rigid tap in terms of motion.

If the machine runs in feed/rev it is directly synchronizing feed based on the spindle speed. It must have more to do with the stop and reverse because if this sync did not otherwise work perfect, we could not single point threads.

Can you explain the differences in how the machine operates? I assume the tap canned cycle has more to do with the accel/decel? rates which differ from the standard spindle stop commands.

[angelw]

Nope. I can say for sure it won't. Not without live tooling.

Rigid tapping using the main spindle is available on machines without live tooling, as an Option. Roughly 2 months ago I installed a Femco lathe with an 0i control that has Rigid Tapping on the main (and only) spindle. The machine has no live, or "C" axis.

One way of determining if the machine is equipped with Rigid Tapping on the main spindle, is to execute M19 via MDI. In this case the main spindle will orientate to a set position, similar to that of the spindle on a machining centre when M19 is executed.

Regards,

Bill

[bob1112]

Thanks. I did verify that M19, though not listed in the M codes list, does lock the spindle in an orient hold position but does NOT rotate the spindle to and certain angle. It just locks the position for about 10sec, then times out. I know the control is getting good feedback from the encoder of at least 4000pulse per rev. I am sure if there was a way to input a set angular position, it would rotate to that position and hold it.

I guess this might come down to the "canned cycle" in the software or parameters that might need setup. I would CERTAINLY be interested to learn more about this control and things we can tweak on it. It seems pretty stripped down and would really like some extra M codes and such.

[angelw]

I thought there was a way to use feed/rev and lock out feed/speed overrides to repond similar to G84? What would a sample program look like and what will the difference be? I know people say you need a tap head but never say what the machine will do differently than rigid tap in terms of motion.

If the machine runs in feed/rev it is directly synchronizing feed based on the spindle speed. It must have more to do with the stop and reverse because if this sync did not otherwise work perfect, we could not single point threads.

Can you explain the differences in how the machine operates? I assume the tap canned cycle has more to do with the accel/decel? rates which differ from the standard spindle stop commands.

Bob,
You're able to lock the Spindle Speed and Feed Rate by using G32 (G33 in G Code System B) instead of G01. If the control is equipped with User Macro B, Feed Hold can also be disabled before tapping commences and enabled on completion.

With User Macro, you can create your own Custom "G" code to call a Custom Macro program for tapping, and pass arguments, such as Z Depth, Retract Level and Thread Lead, something like the following:

G00 X0.0 Z10.000
G184 Z-25.0 R2.0 F1.5 (metric example)
......
......
Rest of program

The heavy lifting would be done by the Macro program that is called by G184. But you still need the floating holder with Compression and Extension, when the control does not have Rigid Tapping.

If you don't understand how to do this, Post back and I'll give you an example.

Regards,

Bill

[bob1112]

Bill I will have to admit that macros is something I have been itching to get into but never took the time. I also am not sure how to verify if a particular control is capable of macros.
As I understand macros, these are if statements basically added to the ladder in a way? IE I can call an operation G300 if I want and when that G300 is read in the program, it will be found in the macro statements and certain actions will proceed. One issue I do not understand is how you can change things such as spindle decel rates, feed hold bypass, etc.

I am also trying to understand if there is a way to use macros to create new M codes to extra functions. We do not have an unloader on this machine and really need one...

[angelw]

Thanks. I did verify that M19, though not listed in the M codes list, does lock the spindle in an orient hold position but does NOT rotate the spindle to and certain angle. It just locks the position for about 10sec, then times out. I know the control is getting good feedback from the encoder of at least 4000pulse per rev. I am sure if there was a way to input a set angular position, it would rotate to that position and hold it.

I guess this might come down to the "canned cycle" in the software or parameters that might need setup. I would CERTAINLY be interested to learn more about this control and things we can tweak on it. It seems pretty stripped down and would really like some extra M codes and such.

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

[angelw]

Bill I will have to admit that macros is something I have been itching to get into but never took the time. I also am not sure how to verify if a particular control is capable of macros.
As I understand macros, these are if statements basically added to the ladder in a way? IE I can call an operation G300 if I want and when that G300 is read in the program, it will be found in the macro statements and certain actions will proceed. One issue I do not understand is how you can change things such as spindle decel rates, feed hold bypass, etc.

I am also trying to understand if there is a way to use macros to create new M codes to extra functions. We do not have an unloader on this machine and really need one...

Bob,
User Macro executable can be verified via the Offset Button of the control. This will call the Offset page and via the Left/Right Option button at the Left and Right bottom of the monitor, you should see [Macro] as a Soft Key. If you see this then the control has the User Macro option. Another way is to execute the following via MDI:
#1=1
If the control accepts that command without alarm, then the control has the User Macro option.

Yes, you can call Macro Programs using Custom "M" codes. You would then write the function in the Macro program, but there would be some modification of the PMC program for what you want to do.

Confirm if you have User Macro B, before I go creating an example for you.


Regards,

Bill

[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.