Helical spiral groove onto curved surface?

[Doug Overkill]

I have a job where I would like to cut a helix along a curved surface. This is on my Hardinge T51SP with Fanuc 18T control. I was hoping to be able to use a threading routine (G76) similar to how I would cut a tapered thread, but instead of cutting the thread along a straight taper, cut it along a defined arc.

Does anyone think this is possible? Any ideas as to how?

Thanks in Advance,
Doug

[Doug Overkill]

I have created a picture of something similar to what I am trying to do.

[angelw]

Originally Posted by Doug Overkill

I have a job where I would like to cut a helix along a curved surface. This is on my Hardinge T51SP with Fanuc 18T control. I was hoping to be able to use a threading routine (G76) similar to how I would cut a tapered thread, but instead of cutting the thread along a straight taper, cut it along a defined arc.

Does anyone think this is possible? Any ideas as to how?

Thanks in Advance,
Doug

Hi Doug,
Its not possible with a threading cycle. Your only hope would be if your machine has a "C" axis. If so, Post back and I, or someone from the Forum will be able to help.

Regards,

Bill

[Doug Overkill]

Hi Bill,
This lathe does not have a C axis. I was hoping for a macro or something which would allow me to run a profile that started at a prescribed moment in the lead similar to how the threading routines start.
Is there anyway to command a "wait until index pulse" or something?
Doug

[angelw]

Originally Posted by Doug Overkill

Hi Bill,
This lathe does not have a C axis. I was hoping for a macro or something which would allow me to run a profile that started at a prescribed moment in the lead similar to how the threading routines start.
Is there anyway to command a "wait until index pulse" or something?
Doug

Hi Doug,
Unfortunately, physics gets in the way. Everything that changes direction must stop, albeit for a very brief moment. Further, to stop, deceleration is involved, and to go from stop to programmed speed, acceleration is involved.

Special software functions (see link below) are available that may be able to do what you want to do, but if your machine does not have a "C" axis, it would be certain that the control would not have the smarts required.

None of what you suggested in your last Post is possible.


http://www.youtube.com/watch?v=XSIcV710ACk

Regards,

Bill

[Doug Overkill]

Hi Bill,
As much as I would like to, this is not one of the times I am trying to break the laws of physics.

The G76 threading routine does what I am trying to do. It gets to the starting point of a threading cycle and locks the z axis to the spindle timing and cuts a straight or tapered thread in multiple passes. Each pass or restart of the program re-engages the same pitch and will cut a deeper thread. So the machine does have the ability to do what I am trying to do.
I am trying to the same thing as a thread cycle just along an arc. Something within the threading cycle which I think is the Q parameter (default to zero) says start threading a 3 o'clock. If the Q is set to 180 then it starts the thread lead at 9 o'clock and this way you can make a multi-lead screw.
My point (without trying to sound argumentative) is that somewhere in the logic of the G76 cycle it waits for a signal to go at the start of each pass timed to the spindle. I was hoping to find out what the signal or wait is and program a toolpath (non linear) to travel such that it starts to move at the signal. I am not trying to start and stop within the workpiece.

Anyway, I appreciate your help and just want to make sure my problem was clear.

[angelw]

Originally Posted by Doug Overkill

Hi Bill,
As much as I would like to, this is not one of the times I am trying to break the laws of physics.

The G76 threading routine does what I am trying to do. It gets to the starting point of a threading cycle and locks the z axis to the spindle timing and cuts a straight or tapered thread in multiple passes. Each pass or restart of the program re-engages the same pitch and will cut a deeper thread. So the machine does have the ability to do what I am trying to do.
I am trying to the same thing as a thread cycle just along an arc. Something within the threading cycle which I think is the Q parameter (default to zero) says start threading a 3 o'clock. If the Q is set to 180 then it starts the thread lead at 9 o'clock and this way you can make a multi-lead screw.
My point (without trying to sound argumentative) is that somewhere in the logic of the G76 cycle it waits for a signal to go at the start of each pass timed to the spindle. I was hoping to find out what the signal or wait is and program a toolpath (non linear) to travel such that it starts to move at the signal. I am not trying to start and stop within the workpiece.

Anyway, I appreciate your help and just want to make sure my problem was clear.

Hi Dough,
Yes, I'm aware that the thread can be indexed, and in software its not hard to do. In fact, in software, just simulating the move, I can get the tool to do just about anything I want. What you have left out in your above reasoning, is that the tool is in fresh air when the new index is started. You don't see the effects of acceleration.

Take for example a parallel thread being cut with any of the threading cycles. The tool starts from a stopped position with the spindle revolving at a constant RPM. To track accurately in the thread path, the slide velocity must equal:
SV = RMP * L
Where
SV = Slide Velocity
L = Lead of thread

To get to the calculated SV from stopped, the Slide will touch every linear speed increment between Zero and SV, albeit briefly; that's physics. Given that the RPM don't change during this acceleration period, the following formula would apply for each SV point along the way.

L = SV/RPM

Lets now say that we run the above algorithm every 0.5ms. Can you see that with every execution of this algorithm, SV will be different, and because the RPM stays constant, the resulting Lead will change. This is the reason why, the faster the spindle RPM used in threading, the further away from the start end of the thread the threading tool started. This is to avoid applying the erroneous Lead to the physical thread being cut. Most programmers just take a guess at this distance based on experience, but a formula can be applied to determine what the minimum length of the erroneous Thread Lead will be. Thread Lead error also occurs at the finish end of the thread, but a different formula is used.

None of the threading cycles are able to cut a thread on a circular path. G32 could be used to cut a thread that had more than one taper angle, but you would be dealing with Acceleration/Deceleration at every change in direction, and the resulting Lead errors.


Regards,

Bill

[Doug Overkill]

Hi Bill
Again thank you for working thru this with me. I understand what you are saying about slide velocity and such but in my case a constant pitch is less important.

Similar to threading I can start an inch or more away from my work piece and run of off the back side such that the tool has ample time to accel and decel without being engaged in the workpiece. I also am not totally concerned with holding a set pitch thru out the toolpath.

Example: 3" dia material which has a flat face (Z zero). The profile of the piece is created along this toolpath:
G1X0Y0
X1.0
G3X3.0Z-1.0R1.0
G1 Z-2.0

So now If my spiral grooving tool ran a toolpath that was some thing like this:

Z1.0 X1.0 S50
G?? (special command to wait for spindle index pulse, which probably doesn't exist)
G1 X1.0 Z0 F.200
G3X3.0Z-1.0R1.0
G1 X5.0 Z-2.0

Then I adjust the X offset in a few thou for this tool and rerun it. In theory (and I know what they say about theories), Each time along the path I can deepen this spiral which follows a nominal 5 TPI path along the arc. Each time I rerun the program it would end up back into the same groove. Without the ability to rerun the toolpath deeper I would need to run the above at the final depth once and hope the tool survives.
The whole toolpath is 3" or so long and at 10 IPM (.2/rev) will go pretty fast. It is done in 15 revs of the spindle at 50 RPM. If it takes more than 1" to accelerate than I can start further away from the workpiece.

Does this make sense? Is it the same as you thought before this example? My reading of your response makes me believe you were worried about different things than I.

[angelw]

Originally Posted by Doug Overkill

Hi Bill
Again thank you for working thru this with me. I understand what you are saying about slide velocity and such but in my case a constant pitch is less important.

Similar to threading I can start an inch or more away from my work piece and run of off the back side such that the tool has ample time to accel and decel without being engaged in the workpiece. I also am not totally concerned with holding a set pitch thru out the toolpath.

Example: 3" dia material which has a flat face (Z zero). The profile of the piece is created along this toolpath:
G1X0Y0
X1.0
G3X3.0Z-1.0R1.0
G1 Z-2.0

So now If my spiral grooving tool ran a toolpath that was some thing like this:

Z1.0 X1.0 S50
G?? (special command to wait for spindle index pulse, which probably doesn't exist)
G1 X1.0 Z0 F.200
G3X3.0Z-1.0R1.0
G1 X5.0 Z-2.0

Then I adjust the X offset in a few thou for this tool and rerun it. In theory (and I know what they say about theories), Each time along the path I can deepen this spiral which follows a nominal 5 TPI path along the arc. Each time I rerun the program it would end up back into the same groove. Without the ability to rerun the toolpath deeper I would need to run the above at the final depth once and hope the tool survives.
The whole toolpath is 3" or so long and at 10 IPM (.2/rev) will go pretty fast. It is done in 15 revs of the spindle at 50 RPM. If it takes more than 1" to accelerate than I can start further away from the workpiece.

Does this make sense? Is it the same as you thought before this example? My reading of your response makes me believe you were worried about different things than I.

Hi Doug,
I understand what you mean, but you have to use one of the threading G codes to obtain synchronization with the Spindle and Slides. Because of this, you will have to virtually generate the curved surface with short G32 X_Z_ moves, and because of Acceleration/Deceleration, this will end in tears. What you want to do is possible with software, but not with what you have with your control.

I do a lot of this special type of work for clients with machines that can't do what they want. I can think of a way to do what you want to do, but its with some extra hardware. Basically a another short stroke, small slide way set as a tool in the tool turret. You would really need to be doing quite a bit of the focus work to warrant the effort.

The best way to do this job would be on a lathe with live tooling and "C" axis, or a 4 axis machining centre.

Regards,

Bill