Peck Drill Cycle G83

[Sam A]

I have a Practical CNC with a WinCNC controller. I use BobCad for creating g-code files.

I am adding a Peck Drill Cycle to my machining tools.

Simple questions;

1. Do I have to have G83 on each line of code?

2. How do I set the Rapid movement Z in the code?

Thanks

Sam

[TOTALLYRC]

I have a Practical CNC with a WinCNC controller. I use BobCad for creating g-code files.

I am adding a Peck Drill Cycle to my machining tools.

Simple questions;

1. Do I have to have G83 on each line of code?

2. How do I set the Rapid movement Z in the code?

Thanks

Sam

Hi Sam, G83 is a canned cycle designed to make it easier to drill multiple holes. While I don't have either of the mentioned programs, here is how it works on Mach3 and Deskcnc.

1. No. the code looks like this,
G83 x0 y0 z-1 r.1 q .050
x1 y1
x0 y2
x4
y4
G00 z2 (to clear the tool and cancel the G81)
X0 Y0
The second line and the rest just have x and y coordinates.
The tool does the following. It will rapid to the X0 Y0 Z.1 position, then it will drill in increments of .050 (the Q value) retracting to .1 above the surface (the R value) until it gets to -1(the Z value).
All of the retracts and the return to drilling are done at the machines rapid speed. The cycle stops the return rapid just short of the last depth, then goes to the feed rate to drill the next increment. It makes coding this much easier than hand coding it. It is also cool to watch.

Be careful about setting R to 0 as it will rapid right to the surface of the part, depending on where your Z0 is set. IIRC

You may have to add code to clear obstacles, so in my example above you might put in a G00 Z4, then on the next line a X0 Y0 to get around something and put the tool above the hole before starting the g83.

It will then move to all the other X,Y values untill the G83 is cancelled by another G-code such as G00. You can even have just the X value or the Y value on a line and it is still valid.

I would try some air cutting the first time to make sure it will work with your program and that I have not left out anything.

Mike

[stevo1]

A very important step is your first Z move before your G83 line entering into canned cycle mode. This sets and will be your initial plane. If your first move before the G83 line is G0Z3. This is the distance that the tool will retract above the part before moving to the next X,Y location. This can be specified by using a G98 in the G83 line of code. Most machines by default use G98. However if the 3” clearance from hole to hole is not needed then you can put a G99 which will use the R value as your clearance plane from hole to hole. In TotallyRC’s example it would be .1”

Stevo

[Rich Kay]

A very important step is your first Z move before your G83 line entering into canned cycle mode. This sets and will be your initial plane. If your first move before the G83 line is G0Z3. This is the distance that the tool will retract above the part before moving to the next X,Y location. This can be specified by using a G98 in the G83 line of code. Most machines by default use G98. However if the 3” clearance from hole to hole is not needed then you can put a G99 which will use the R value as your clearance plane from hole to hole. In TotallyRC’s example it would be .1”

Stevo

Great comment! I am avid user of structuring rapid movements well above the surface of machining. I always add a G98 Z4 (by default) to all my programs ensure I don't rapid tools into hold down straps, clamps, or higher than Z0 machined fits... it's awesome insurance... IMO the G99 is extremely risky, (at least for what my machining consists of)

[mactec54]

Hi sam A

Stevo1 has the best & correct way to do it you also need to cancel with a G80 at the end of the canned cycle

G90G17
S2850M3
G43Z2.H1
G83G98X0Y0Z-.250R.1Q.030F12
G80G0Z2.
M9
M5
M30

As Stevo1 has said if your tool is clear of the part & you don't have to clear anything then you can use a G99 were the G98 is This piece of Gcode is just a small sample of what you need to do for a canned cycle the beginning of the Gcode sample is not complete

[menkay]

I have a peck drilling problem (G83) while operating my Cincinnati Milacron Sabre 750 with 2100 Acrimatic controller;
Below are the lines of codes I ran on the VMC, the G83 code went rapid to the clearance plane, then stopped there. It did not go further to drill the programmed hole.
:100 T15 M6; HSS-Cobalt I (0.272inch diameter drill, 135o point angle)

N10: G0 z1.0 M08

N20: G83 X3 Y0.3189 R0Z-1.6563 K0.125 J11 F0.7 S350 M03 W1

Please any help regarding this will be appreciated.

[angelw]

I have a peck drilling problem (G83) while operating my Cincinnati Milacron Sabre 750 with 2100 Acrimatic controller;
Below are the lines of codes I ran on the VMC, the G83 code went rapid to the clearance plane, then stopped there. It did not go further to drill the programmed hole.
:100 T15 M6; HSS-Cobalt I (0.272inch diameter drill, 135o point angle)

N10: G0 z1.0 M08

N20: G83 X3 Y0.3189 R0Z-1.6563 K0.125 J11 F0.7 S350 M03 W1

Please any help regarding this will be appreciated.

Basically, the block looks OK, except for the Spindle Speed and Start, I'm unsure if they're allowed in the canned cycle block. I would put them on a separate block after the tool change.

What value do you have for the Gauge Height Parameter?

Regards,

Bill

[dwood]

I have a Practical CNC with a WinCNC controller. I use BobCad for creating g-code files.

I am adding a Peck Drill Cycle to my machining tools.

Simple questions;

1. Do I have to have G83 on each line of code?

2. How do I set the Rapid movement Z in the code?

Thanks

Sam

Sam
if you will post this in the bobcad forum,under bobcad-cam, i will help you
along with others, i use wincnc everyday, your post may need some adjusting
and will need to know how your router is setup
DW

[menkay]

Basically, the block looks OK, except for the Spindle Speed and Start, I'm unsure if they're allowed in the canned cycle block. I would put them on a separate block after the tool change.

What value do you have for the Gauge Height Parameter?

Regards,

Bill

Thank you Bill for responding to my question,
I just tried it exactly the way you suggested and I still experienced the same problem. My Gauge Height Parameter I used a 6 inches aluminum block to set the surface length offset using TRAM, that was basically my reference point (ie 6 inches) before I then used a drill bit to set the Tool Length Offset from the 6" reference position. All codes worked perfect apart from the G83 'peck drilling' code....please any further suggestion or help will surely be appreciated

[angelw]

Thank you Bill for responding to my question,
I just tried it exactly the way you suggested and I still experienced the same problem. My Gauge Height Parameter I used a 6 inches aluminum block to set the surface length offset using TRAM, that was basically my reference point (ie 6 inches) before I then used a drill bit to set the Tool Length Offset from the 6" reference position. All codes worked perfect apart from the G83 'peck drilling' code....please any further suggestion or help will surely be appreciated

I'm not sure if we're talking about the same Gauge Height Parameter. The Gauge Height Parameter for drill cycles is the distance above the R plane that the tool returns to at the end of the drilling operation. This position is R+Gauge Height Parameter setting+ W (if used - its optional)

Has the G83 cycle ever worked? Does the G82 cycle work?

Regards,

Bill

[menkay]

I'm not sure if we're talking about the same Gauge Height Parameter. The Gauge Height Parameter for drill cycles is the distance above the R plane that the tool returns to at the end of the drilling operation. This position is R+Gauge Height Parameter setting+ W (if used - its optional)

Has the G83 cycle ever worked? Does the G82 cycle work?

Regards,

Bill

In that case, the Gauge Height Parameter is W1 in the line of G83 code;
The G83 has always worked and G82 works very well...That's why I know what what could be wrong with the code or if there's anything extra I should do that I haven't done.