Rigid tapping with OTC

[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