Cnc Course in hobby machinist

Hawkeye said:
Good idea. This could accelerate the learning curve. Will it be generic G-code, or have some specifics for commonly used programs such as D2NC?
Click to expand...
We will start easy going with G code, describing first each of the common G's and M's, and an example of how a written program uses that code.
I propose learning 5 codes a day. Then, once the class is mature enough we can complement it with a video of the use.
I HIGHLY RECOMMEND EACH BUYS A TINY SMALL HARD COVER NOTEBOOK. To keep each example of a program for reference.
Lets see how it works during a week, then we can propose improvement upon classroom necessity.

regards
 
Chapter One, a brief description...

A Code is only a way to tell the machine what you need to do, it can be as simple as actuating a solenoid that will turn on a light, pump or mechanism as complex as calling a subprogram that will execute a cycle or subroutine. Lets see the first five:
G00: tells the machine to move in rapids to a position described by X, Y, Z. If you put the three coordinates on the same line, the machine will interpolate to the position, in other words calculate the shortest trayectory to the coordinate given. If you put only one per line, the machine will position one at a time.
G01: will do exacly as the G00, but at the cutting speed or FEED rate.

G02: will order to move on a curve to the right or clockwise.
G03: will order to move on a curve to the left or counterclockwise.
G04: will order the machine to remain on a break for seconds, milliseconds or in other words DWELL. IT is used to finish the bottom of holes, or perform simultaneous tasks that take different time and you want one to wait for the other to finish.
tomorrow we will use all of them on a small program. Meanwhile Memorize them please.

Program example:
(There should be preparatory codes at the heading of the program, now skipped because we have not seen them yet)

G00 X5.263 Y3.236; (I advise all G00 moves are done first X and Y, at the highest Z value, to prevent wrecks)
G00 Z0.25; (positions the spindle 0.25 above the setpoint or reference point on the part)
G01 Z-0.100 F4; (penetrates the part 100 thousands at a feedrate of 4 inches per minute)
G01 X10.0 F40; (cuts in the X direction at 40 Inches per minute)
G03 X12.0 Y-5.0 R2; (cuts from where it is to point X12 Y-5 doing a Clockwise turn of radius 2, if not calculated correctly with other parameters that must also meet, Error alarm will set off, this line can be programmed using I J and K, where you set the arc center, the radius and end point, we will also see polar coordinates later)
G04 X600.0 (The machines remains in the current position for 600 seconds or 10 minutes)
 
Last edited:
Good start. I've learned something new already - same line vs separate lines.

I started a Word document, which I've tagged to the desktop for quick access. I can cut and paste from the lessons and add notes as I learn things.

Thanks for doing this.
 
Hawkeye said:
Good start. I've learned something new already - same line vs separate lines.

I started a Word document, which I've tagged to the desktop for quick access. I can cut and paste from the lessons and add notes as I learn things.

Thanks for doing this.
Click to expand...
Very welcome, other than the word doc. Get you a small notebook, so later, if you are in front of a cnc, and cant recall exact how to make a tap program, you just copy it, same with how to make a subroutine, call a subprogram, etc.
 
Re: Chapter One, a brief description...

Syaminab said:
G02: will order to move on a curve to the right or clockwise.
G03: will order to move on a curve to the left or counterclockwise.
Click to expand...

Hopefully I'm not too late to join in?

I already have a question if I may? What determines the curve (radius?) that it is directed to go to?

Thanks,
Dave
 
Re: Chapter One, a brief description...

fretsman said:
Hopefully I'm not too late to join in?

I already have a question if I may? What determines the curve (radius?) that it is directed to go to?

Thanks,
Dave
Click to expand...
We will see that in the examples. At the end of each 5 codes we will take all questions .
 
dennis98277 said:
I take it that you need a CNC machine to take this class correct?
Click to expand...
No, you will learn how to program Gcode, this has the intention of explaining how its done on CNC So everyone looses up the fear and myths.
Later, if in your job you find a machine you will know what to do. If the scare look of a type board and a screen instead of levers is keeping you from having a cnc, this course will improve those fears.

Once the class is mature enough, I will film some programs on my cnc to complete the teachings. Also Im looking for a software that will emulate a cnc so you all can program in your computers and test run...
 
Chapter two, next five codes

Dear Fellow machinning enthusiasts:
There will be times where I can`t show up here, because of work, travel, etc. So I`m heading on right now to get more advanced...:nuts:

2nd set of five codes:
(Remember, I`m only covering the common in use, I`m not cheating by skipping)
G15 (Cancells the Polar Coordinate Comand, That is if the machine was set in Polar instead of Cartesian)
G16 (Sets the machine in Polar mode, where you put a center, a radius and an angle instead of X,Y...Z remains the same)
G17 (Sets the machine in the X-Y Plane)
G18 (Sets the machine in the Z-X Plane)
G19 (Sets the machine in the Y-Z Plane)...This last three, will be used only when expertise is developed.
G20 (Sets the machine in Inches)
G21 (Sets the machine in mm)
G28 (Orders the machine to return to it`s machine reference point)
G40 (Cancells Cutter compensation in right and left side) and I`m going to run wide open here.:holdphone:..this code is important along with G41 42 for several reasons.
CNC machines have a disability, they are Blind, so you must show them where the part is, and how the tool is. The last codes will assist you on that.
let`s say, you have different drill bits, of course in different lenghts and diameters, well G43 tells the machine this difference in lenght. Now, let`s say you have different diameter endmills, well, if you are running to the left G41 will let you change the cutter diameter and remain on track, or also compensate for minimal differences in between diameters of equal endmills...measure them and they are hardly ever equal plus wear... Remember 3 thousands are enough for part interference and will not assemble right. So if you are one or two thousands off track this codes will help you a lot to run a second pass without rewriting the whole trayectory.

G41 (Cutter path compensation on the Left)
G42 (Cutter path compensation to the Right)
G43 (Cutter compensation in + Lenght)
G44 (Cutter Compensation in - lenght) I never use this one, I avoid it by understanding that my set up probe is 0 in lenght and what ever sign the tool gives I write it on the screen.
G49 (Cutter compensation in lenght Cancellation)

Let`s cut it out for today, I will write the format in which each one is written and explain.
 
Last edited:
i must have missed something. . . i have g01 thru g04 then g15 to g49/ where are g05 thru g14 ?
 
You must log in or register to reply here.
Back
Top