Mach3 end movement G81 or G1 with external input Signal

Hello,

we have two machines to drill counterbores in sheet metal. One of them has Mach3 as CNC controller.
Due to warping of the sheetmetal wie have a drillhead with down hold funktion via gas springs.
On the other machine we have a sensor on the drill head and a digital input to end a custom G81 cycle bevor it reaches the programmed depth if the counterbore is deep enough.
The Z-Axis stops and returs to the SafeZ Position. Controller on this machine is Tekna OEM software.The concept works really fine (tollerances +-0,1mm), that is why I want to stay with this solution.

Now i need a methode to do this on the Mach3 software.
Can you give me some advice how to archive this?
It doesn't have to be a solution with G81, i want to use a macro with the parameters for the holes.


Info:
Mach3 R3.043.066
IO: CSMIO_IP

Best regards

Quote:

---

Originally Posted by lootspastille

Hello,

we have two machines to drill counterbores in sheet metal. One of them has Mach3 as CNC controller.
Due to warping of the sheetmetal wie have a drillhead with down hold funktion via gas springs.
On the other machine we have a sensor on the drill head and a digital input to end a custom G81 cycle bevor it reaches the programmed depth if the counterbore is deep enough.
The Z-Axis stops and returs to the SafeZ Position. Controller on this machine is Tekna OEM software.The concept works really fine (tollerances +-0,1mm), that is why I want to stay with this solution.

Now i need a methode to do this on the Mach3 software.
Can you give me some advice how to archive this?
It doesn't have to be a solution with G81, i want to use a macro with the parameters for the holes.


Info:
Mach3 R3.043.066
IO: CSMIO_IP

Best regards

---

A G81 is a standard drilling cycle and Mach3 can use / do the same process, this is a feed in and rapid out operation

Thank you for answering.
The Mach3 G81 cylcle does not react to a external input to stop overdrilling. How can i archive this?
My problem is that i drill into the sheet metal without knowing the exact Z position of the sheet. I cant measure the position first because it depends on warp and cuting pressure.
I thinking of using G31 as a drill cycle to archive stopping by external input but i dont know if it works with active M3.

Best regards

Quote:

---

Originally Posted by lootspastille

Thank you for answering.
The Mach3 G81 cylcle does not react to a external input to stop overdrilling. How can i archive this?
My problem is that i drill into the sheet metal without knowing the exact Z position of the sheet. I cant measure the position first because it depends on warp and cuting pressure.
I thinking of using G31 as a drill cycle to archive stopping by external input but i dont know if it works with active M3.

Best regards

---

It's very simple

G90G0X0Y0.
G43Z.1
G81G98X----Y-----Z-.1F8. the Z depth is completely controllable by whatever number you use for the Z- Depth what I show here is it will go from .1 above the part to .1 through the part, this number can be anything you want it to be.

A G31 is not anything to do with a drill cycle, it is for a probing cycle

Hello,

I know about the normal use of G81 and G31. The problem is that the final Z depth is not known at the cycle start. I can give the cycle the theoretival z depth but if the sheet is warped this leads to overdrilling the counterbore and the workpiece is scrap metal.
To prevent this i have a drillhead that has a adjustable sensor who tells via a 24V Signal when the correct Z depth is reached.
When the controller get the input signal, no matter programmed z depht is reached, the the z axis must reverse feed.
I search for a solution to this problem.

The probing cycle has somewhat of this behavior. But i dont know if this works with M3 or M4 und with a drill as tool in mach3.

A probing command for drilling will work just fine. It will not check or interfere with M3/M4. Naturally, you would have to program all the movements manually without the convenience of a canned cycle.

Something like this:

Code:

---

G90 (make sure we are in absolute mode)
G0 Z5 (go to safe height Z=5)
G0 X10 Y20 (go to the hole coordinates X=10 Y=20)
M3 (start spindle)
G0 Z1 (fast plunge to Z=1)
G31 Z-2 F100 (drill to Z=-2 or until probe input activates)
G0 Z1 (fast retract to Z=1)
M5 (stop spindle)

---

Quote:

---

Originally Posted by CitizenOfDreams

A probing command for drilling will work just fine. It will not check or interfere with M3/M4. Naturally, you would have to program all the movements manually without the convenience of a canned cycle.

Something like this:

Code:

---

G90 (make sure we are in absolute mode)
G0 Z5 (go to safe height Z=5)
G0 X10 Y20 (go to the hole coordinates X=10 Y=20)
M3 (start spindle)
G0 Z1 (fast plunge to Z=1)
G31 Z-2 F100 (drill to Z=-2 or until probe input activates)
G0 Z1 (fast retract to Z=1)
M5 (stop spindle)

---

---

The G31 will cause a retract as soon as the drill touches the work so this will not work

G31 will move an axis until the probe is triggered (Drill), or as soon as it makes contact with something then it will retract.

A G31 uses an electrical signal for the input to the control when it makes contact, which it would need for it to work, (the drill and the work) would make the circuit, so as soon as it touched it would retract

There may be a trick that can be used but not like you have posted

Quote:

---

Originally Posted by lootspastille

Hello,

I know about the normal use of G81 and G31. The problem is that the final Z depth is not known at the cycle start. I can give the cycle the theoretival z depth but if the sheet is warped this leads to overdrilling the counterbore and the workpiece is scrap metal.
To prevent this i have a drillhead that has a adjustable sensor who tells via a 24V Signal when the correct Z depth is reached.
When the controller get the input signal, no matter programmed z depht is reached, the the z axis must reverse feed.
I search for a solution to this problem.

The probing cycle has somewhat of this behavior. But i dont know if this works with M3 or M4 und with a drill as tool in mach3.

---

So, you may be able to use this trick if you can maintain the electrical signal, through the work and the Drill

Too use the G31 and get the exact depth each time, once the signal is made from the Drill touching the work, the Z axis would then continue to move down to a set depth and then retract

You would have to write this in a Probing Macro routine this is the only way a G31 could work for what you want to do.

The signal will be the deciding factor between the drill and the work and how reliable that signal will be