Doosan Fanuc G76 thread start angle

[caesarspalace]

I am looking for info on how to control the G76 thread start angle (clocking) on Doosan-Fanuc.

I have been machining threads for 30 years on Haas machines but relatively new to Doosan-Fanuc.

On Haas machines and some Fanuc with the single line G76, the Q is used for thread start angle or clocking of the thread.
On my new machine with a Doosan-Fanuc control with dual line G76, the Q in the first line is used for minimum depth of cut, and the Q on the second line is used for depth of first cut. According to my programming manual, it doesn't list any value that controls the start angle.

Can anyone help me here?

 

[ewlsey]

You can change the start angle by changing the Z axis start point of the canned cycle. I'm assuming this is a multi-start thread?

 

[angelw]

I am looking for info on how to control the G76 thread start angle (clocking) on Doosan-Fanuc.

I have been machining threads for 30 years on Haas machines but relatively new to Doosan-Fanuc.

On Haas machines and some Fanuc with the single line G76, the Q is used for thread start angle or clocking of the thread.
On my new machine with a Doosan-Fanuc control with dual line G76, the Q in the first line is used for minimum depth of cut, and the Q on the second line is used for depth of first cut. According to my programming manual, it doesn't list any value that controls the start angle.

Can anyone help me here?

Hello caesarspalace,
The "Q" address for indexing the Start of the Thread is not available with the Two Block Format G76 Cycle (FS16 Standard Format). It is available with the Single Block Format (FS15 Format) and is specified in the same way as you're familiar with using the HAAS control. FS15 or FS16 Format is selected with parameter bit 0001.1. Setting the parameter bit to "1" will select FS15 Format.

Failing that, the only way to index the Start of the Thread with the Two Block Format is as ewlsey suggests. The Z Start Point is moved by the Thread Lead/Number of Starts (Thread Pitch) for each new Thread Start.

The "Q" address can be used to index the Thread Start with G92 and G32 Threading processes when the control is set to FS15, or FS16 Format (Two Block G76 Threading Cycle).

Regards

Bill

 

[sinha]

... and F is lead, not pitch.

 

[caesarspalace]

No, it's not a multi-start thread, I have an irregular shaped workpiece and I want the thread to start at the 9:00 O'clock position (180 deg).
I will try the G92 method, even though my programming manual doesn't list 'Q' as an option in the G92 example.

 

[yardbird]

No, it's not a multi-start thread, I have an irregular shaped workpiece and I want the thread to start at the 9:00 O'clock position (180 deg).
I will try the G92 method, even though my programming manual doesn't list 'Q' as an option in the G92 example.

Very Interesting!

I know of no way to locate the start point on a thread on a radius value. As other have stated typically you start the first thread and any variant there after is either variable in the cycle or shift in the start position? I kinda always thought the start orientation point of the thread weather it be G76 G32 G92 had something to do with M19?

I'm thinking a custom macro and not a Fanuc canned cycle but still wouldn't know how to do it?

Got a sketch of the part you could post for us to see?



Brent

 

[caesarspalace]

Very Interesting!

I know of no way to locate the start point on a thread on a radius value. As other have stated typically you start the first thread and any variant there after is either variable in the cycle or shift in the start position? I kinda always thought the start orientation point of the thread weather it be G76 G32 G92 had something to do with M19?

I'm thinking a custom macro and not a Fanuc canned cycle but still wouldn't know how to do it?

Got a sketch of the part you could post for us to see?



Brent

Don't have a scetch, it's a single start thread as I've already stated, not a multi start. With the single line G76, the 'Q' indicates the start position or clocking, with that you can start the thread at any given degrees, eg. Q180.00 would be 180 degrees. I have an offset fixture in the 3-jaw and I need to start the thread in the 9:00 O'clock position, the 12:00 O'clock position of my fixture is lined up with jaw #1. The OD of my part is wobbling by the amount of offset built into my fixture, the ID is running true with machine centerline (obviously) as I just bored it out. The 12;00 position of the fixture that's lined up with jaw # 1, is the largest part of my eccentric, the 6:00 O'clock position is the thinnest which lies half way between jaws 2 & 3. The mid points of my eccentric are at the 3:00 O'clock and 9:00 O'cock positions. Now I want to thread the ID starting at the 9:00 O'clock position. It's imperative that the thread starts here.
I hope you can picture in you mind what I'm tryin to do.
The lathe doesn't have live tooling or C axis, so I cant mill it.
The encoders CNC lathes use which start the thread in the same place each pass also are able to start at a commanded position.

 

[angelw]

The encoders CNC lathes use which start the thread in the same place each pass also are able to start at a commanded position.

Hello caesarspalace,
The Start Position (index wise) of the Thread will be affected by the Tool Start distance in Z from the Workpiece. Accordingly, any randomly selected Start Distance from the Start of the Thread in the Workpiece will be less than one Thread Lead from the correct position to give you the Index Location you desire. Moving the Tool Z Start Position by a whole Lead will Index the Thread 360deg. Therefore, after taking a light test threading pass, if you determine that the Thread Index is incorrect by 10deg, for example, you only have to move the Tool Start position by:
L/36
Where L is the Lead of the Thread.

Because your part is being held in a fixture, the determined correct Tool Start Position will give the same correct result when the job is run again in the future (providing the Z Offset of the Tool is set correctly).

Regards,

Bill

 

[Vancbiker]

^ this is what you have to do.

@ OP:
Keep in mind that there is no relationship set by the machine builder as to which jaw on the chuck equates to the one revolution mark on the spindle encoder. You have to find the timing of your part on your fixture as Bill describes above. Once you have established that then your remaining parts will be the same. Move the process to an different, but identical machine and you will have to find the correct start position for that machine. They will not be the same.

This will be true whether or not you have the one line G76 or two line G76. In simple terms, the Q value in the one line G76 just tells the control to wait X number of encoder counts after the one revolution mark before starting the threading pass.

 

[caesarspalace]

^ this is what you have to do.

@ OP:
Keep in mind that there is no relationship set by the machine builder as to which jaw on the chuck equates to the one revolution mark on the spindle encoder. You have to find the timing of your part on your fixture as Bill describes above. Once you have established that then your remaining parts will be the same. Move the process to an different, but identical machine and you will have to find the correct start position for that machine. They will not be the same.

This will be true whether or not you have the one line G76 or two line G76. In simple terms, the Q value in the one line G76 just tells the control to wait X number of encoder counts after the one revolution mark before starting the threading pass.

Yes, I understand that. thanks guys.