G73 G83

[Ajit]

Hi friends

G73 - High Speed Peck Drilling Cycle

G83 - Deep Hole Drilling Cycle

What is differnce between G73 and G83 canned cycles. When we use this cycles? Or this are Controller dependent.

 

Also I found some CNC code containing G codes Like

G92.5 R0.

G71.1

What is the above G Codes means.

 

Thanks in advance.

Ajit

[Henk]

G83 the drill rapid each peck out to "R", rapid down and drill the next peck.

G73 the drill retact for 0.5mm then drill the next peck

[Marty A]

g73 and g83 are identical except in g83 the

tool retracts all the way out of the hole

between pecks. hth

 

 

marty

[LNDCAD]

Additional info -

G73 - High Speed Peck Drill Cycle (Also called chip break cycle) will only retract a set amount between pecks (usually set up on the parameter page of the controller, and not on the G73 code line). Used where the flutes of the tool are not buried, allowing the chips to flow out of the hole while drilling. This is a very fast cycle and can save a lot of time / machine motion when used properly.

G83 - Deep Hole Peck Drill Cycle is used where the flutes of the tool would be buried in the workpiece during drilling. This cycle retracts all the way back to the Z height specified as "R". This cycle is slower but will clear the chips better on a deep hole. HTH.

[chris m]

I notice that you have the lathe icon displayed for this topic; if you are in a lathe the G73 and G83 may not perform these functions at all. In many lathes the cycle used as a peck-drill cycle is often defined as a face-grooving cycle which has programmable peck depth, retract amount, etc.

 

The general description of the differences between these cycles [in a milling machine] above are absolutely correct except for that the retract amount for G73 can often be specified in a parameter [edit LNDCAD you're too fast /edit] so it may not be [probably isn't, actually] .5mm in your particular case. A thorough read of the machine tool's manuals is necessary to understand cycles and settings available in your case.

[Ajit]

Thanks to all

I asked G83 and G73 for Milling Machine only.

I select lathe Icon by misstake only.

Can any body explain about my second question. ie G92.5 and G71.1

What is mean by this G code.

 

Thaks

Ajit

[Rob B]

In my Mazak Parameter book, it listed G71.1 as a fixed cycle chamfer (CW). G72.1 as fixed cycle chamfer (CCW).

 

I have never seen these used in prgramming. But the example that it shows a line of program that looks like this: [Xx Yy] Rr Zz Qqo [Ppo Ddo] Ffo

qo: Radius

po: Overlap amount

do: Distance from point R

fo: Feddrate

 

I don't know if this helps.

It appears that this is a canned cycle for chamfering. Does anyone know if MC can output this type of cycle & has anyone ever seen this used.

 

My parameter book has a lot of this type of "G" code. Some I have never seen used.

[heeler]

quote:

---

Additional info -

G73 - High Speed Peck Drill Cycle (Also called chip break cycle) will only retract a set amount between pecks (usually set up on the parameter page of the controller, and not on the G73 code line). Used where the flutes of the tool are not buried, allowing the chips to flow out of the hole while drilling. This is a very fast cycle and can save a lot of time / machine motion when used properly.

G83 - Deep Hole Peck Drill Cycle is used where the flutes of the tool would be buried in the workpiece during drilling. This cycle retracts all the way back to the Z height specified as "R". This cycle is slower but will clear the chips better on a deep hole. HTH.

---

While this is true for our fanuc controls, In our Vickers controle the has something to do with setting a Probe Stylus and Tip Dimension. We must know what control this machine is to really be able to anser the question correctly.

 

I learned about this when someone was trying to run a G73 on our Vickers control. kept throwing alarms for not having the proper data on the line.

 

HTH

 

Glenn