[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.

[sanisz]

Hi,

I was wondering if it was possible wit G83 peck drilling (or something else to do canned cycles) that the tool retract position isn't the surface position Z.
It would be better if it would do just the feed rate stop at Q interval or just a minimum of 0.2mm retract distance.
(Linuxcnc)

Thanks in advance.

[handlewanker]

Hi.....as I'm very new to CNC and learning G code, I have to wonder what happens during a peck cycle when a small piece of swarf stays in the bottom of the hole and with a peck cycle, where the drill is lifted fully out of the hole, you then get a situation where the next drill down feed just hits down on it and prevents the drill from cutting despite a feed rate.

I came across this frequently when manual drilling and lifting the drill bit to break the swarf and clear the drill, but a small piece of swarf frequently got left in the hole and I had to blow it out with a jet of air.

I cured this by just pausing the down feed to break the swarf without actually lifting the drill bit.

Would it be better in a peck cycle to just stop the down feed and dwell for a second and then down feed again etc?

Any swarf not pushing out of the hole with the cut, which usually produces a string or short chips (leaded or freecutting steel) wit be ejected on the next down feed but won't get trapped under the drill point provided the drill point is not lifted.
Ian.

[sinha_nsit]

I do not think this is possible with the regular G83.
You will have to design such a sequence yourself. There are several ways. If you do not want to use macro programming, G82 may be used repeatedly, to simulate pecking. G82 is a continuous drilling cycle with dwell.

[handlewanker]

Hi, I'm still learning G code, but the possibility of a piece of steel swarf under the drill point bothers me.

So, without using the G83 command, does the P dwell command have a time factor that causes the program to resume after a second or two?.....that would suit me fine........lifting the drill out of the hole is something I want to avoid at all costs even if it's the established method.

Not sure of the "amended" peck sequence I want, but as the P part is the dwell time........would I have to write something like G01 Z3 F100 and add a P .02 to get .2 seconds dwell then Z5 to get 2mm more depth at the same feed rate and another P .02 dwell etc etc..... without lifting the drill out until the full depth is obtained.........I'm not sure of the sequence to achieve that

I've found this to be highly successful for manual drilling deepish holes in steel.....at least holes that are 3D or more.

Soft materials like aluminium tend to weld the chips to the flutes of the drill if not lifted out completely, but the drill can cut into any loose chips that get under the drill point, so no problem.

I've come to the conclusion that writing G code is like writing a book......with a book you can leave out all the punctuation and still be able to read the contents......I think G code is a bit like this too, but not so forgiving.

For instance, you could leave out the G20 and still run the program if you set up your machine to Metric measurements, but not to give the program to someone else with Imperial settings.

I've seen different G code sequences for the same function and this makes tutorials confusing.
Ian.

[sinha_nsit]

G04 P1000 would dwell for 1 second.
G04 X1 also would dwell for 1 second.
P does not take decimal values.

There is no default for G20/21. The mode used in the previous machining session is used by the machine, unless it is changed.

[angelw]

Hello handlewanker,
If I understand your problem correctly, you can use the High Speed Drill Cycle G73 to achieve your required result. G73 is a Peck Drilling Cycle that does NOT retract to the "R" plane after each Peck, it only retracts a small distance that can be set via parameter. You could set the parameter to an infinitesimally small value so that there was practically no lift off, but enough hesitation to break the chip.

G20/G21 is recorded in parameter when its executed and therefore will default to that setting when power to the control is cycled. It is good practice to include G20/G21 in a first block safety line, one that sets the desired default status of the control for the program being run. Doing so will ensure that the control will correctly interpret the Imperial/Metric units of the program that is being executed.

Regards,

Bill

[sinha_nsit]

He wants a dwell also at the end of each peck, if I understand it correctly.

[angelw]

He wants a dwell also at the end of each peck, if I understand it correctly.

Hi Sinha,
Yes, I see that from his Post #13. I believe that G73 with a very small retract, say 0.02mm, would have the desired result of breaking the swarf. Dwelling at the end of each peck could only be for the purpose of breaking the swarf.

Regards,

Bill

[handlewanker]

Hi......thanks....that's what I want, only a dwell not a retract, just to break the swarf string.........having had the experience of an 8mm drill trying to overcome a chip at the bottom of a deep hole.........600mm .....I kid thee not........it was for a lubrication gallery on a 100mm diam shaft, the outcome was that to get the loose pieces of swarf out I used a magnet on a piece of steel rod.

That was for a manual drilling operation, and as it might impact on a CNC situation, even for a relatively shallow hole where you have no indication of a chip left in the bottom of the hole, I decided to investigate the peck cycle to see if it could be "improved"........for my use etc.

BTW.......the guy on day shift who worked on that same drilling job broke the drill bit off half way down the shaft......4 times.........so they welded plugs in the top of the blocked holes and I got to finish the job.......my secret method stayed with me because they were a bunch of arseholes.....LOL.

I'll investigate G73 as I don't know how it's used in a G code sequence......learning learning.

I have a job I'm working up to do when I get the G code sequence in order......it entails drilling four 5mm diam holes in 8 pieces of work.....32 holes in all....approx. 10 mm deep, so that'll be a good start to my CNC escapade.......the mill I have, a Skyfire SVM-0 build, is still in it's virginal pristine condition, so it's getting near the time to create a bit of swarf.
Ian.