Need Help!- Oriented Thread Cutting on 18i TB

[ecapatto]

Hi,

I'm trying to cut some threads that need to have the start point aligned with one face on the workpiece. I heard about FANUC controls are able to "remachine" threads, just positioning the cutter in the thread and then storing the value on some parameter. But it's one Manual Guide functionality and I have not this option on my control.

So I ask, there is some way to change the thread positioning by changing some parameter? I mean, if the guide do the job done so the parameter must be there somewhere, even without the Guide installed.

I really need to get this job done, if one of you can help me with some tips I'll be glad.

P.S. I already know that if I change the Z entry coordinate I can archieve the entry point position change, but it isn't precise enought to my workpiece, because I need the correct alignment, So I'll need to align the face, read the Spindle position, change the "unknow to me" parameter and then cut the thread.

I also have no idea on how can I see the spindle encoder position.

Thanks,
Eduardo

[dcoupar]

If you're using the G76 threading command, I believe you can specify a start angle with Q. However, you have to change your settings to use the F15 format (one line Multiple Repetitive Cycles)

If you're using G32 or G92, try specifying a Q starting angle... you shouldn't need to change the F15 setting.

180 degrees = Q180000

[sinha_nsit]

While you may adjust the start point/angle in threading cycles, it may not be possible to hold the previously threaded workpiece in exactly the same angular position. So, rework would not be possible, once you unclamp the workpiece.
Manual Guide may have some special feature, as described by you. I am not aware of it, and would like to know more about it.

[dcoupar]

Here's the section of the Manual Guide Lathe Operator's Manual dealing with Rethreading.

[sinha_nsit]

Thanks a lot for the information.
Till now, I was under the impression that Manual Guide is for those who do not have enough knowledge of part programming; Manual Guide prepares machining codes for them in an interactive manner. But, this feature is a unique one, not available otherwise.

I, however, could not find these pages in the 0i manual. Are there different versions of Manual Guide?

[ecapatto]

Thanks for the tips. The Manual Guide manual section really show to me that what I'm thinking about rethreading. Manual Guide does this automaticly, but to who have no Manual Guide the processe is perfectly possible, just by calculating the Q parameter, maybe with one macro or something like that, even the manual shows how to calculate it begining in the page 247.

The entire goal here is to be able to ready, somewhere, the spindle actual position. Maybe must exist some function to transform the Spindle into C axis, just to capture the position. Or some parameter that store that position. Or even an maintenance screen that shows the encoder position.

I'm very happy to see that it's possible, but I can't find where can I see the spindle position.

[dcoupar]

Originally Posted by sinha_nsit Thanks a lot for the information. Till now, I was under the impression that Manual Guide is for those who do not have enough knowledge of part programming; Manual Guide prepares machining codes for them in an interactive manner. But, this feature is a unique one, not available otherwise. I, however, could not find these pages in the 0i manual. Are there different versions of Manual Guide?

Yes. Manual Guide, and Manual Guide-i.

[dcoupar]

Originally Posted by ecapatto Thanks for the tips. The Manual Guide manual section really show to me that what I'm thinking about rethreading. Manual Guide does this automaticly, but to who have no Manual Guide the processe is perfectly possible, just by calculating the Q parameter, maybe with one macro or something like that, even the manual shows how to calculate it begining in the page 247. The entire goal here is to be able to ready, somewhere, the spindle actual position. Maybe must exist some function to transform the Spindle into C axis, just to capture the position. Or some parameter that store that position. Or even an maintenance screen that shows the encoder position. I'm very happy to see that it's possible, but I can't find where can I see the spindle position.

Does your machine have the C-axis option? Can you orient the spindle with M19?

[ecapatto]

It's one Special Machine that we received from UK and then refurbished here in Brazil. The PCL programmer didn't released the M19 or M190 function, but they did one function on PCL called "Spindle Oriente", because we have one mechanism that opens and closes the chuck fisically, so the spindle must be oriented to that specific position to allow this "machanism" to clamp with the chuck.

I know that the spindle doesn't uses one FANUC motor and the Drive is from Telemecanique (Schinneider Electronics).

And there is an Pulse Coder in the spindle. I had worked for this Machine Manufacturer years ago (www.romi.com.br), and I saw many times this kind of configuration in other kind of machines, and I know that M19 function, to work propertly, must be implemented on PLC, but in this case it wasn't.

I just don't know where the spindle position are. Maybe just in the Drive? If it is there so it's possible to see, even in the Drive, will helps anyway, I just asked about this issue to the Drive manufacturer.

But I think that the Pulse Coder position must be monitored by the control.

The Machine Manufacturer just told me that the G33 with Q command will work fine, and they are engaged in find where the spindle angle is. But if anyone knows where it is, please tell me.

Thanks for the advance...

[ecapatto]

The G76, G78 and G33 doesn't work. But the G32 works fine with Q parameter, I did one 4 entry thread on this machine today and all OK.

I did some tests with #4077 - SPINDLE ANGULAR SHIFT. Exactly what I was expecting. There is an Analog Spindle, so Serial Spindle parameters will not work for instance.

Now it's just about to see the Spindle Angle. I'm almost mad, but I'll find this value.