Cnc Course in hobby machinist

[MikeWi]

Re: Find the Errors in the first program

This is because there are two zeros, one for the machine and one for the part, G28 will be zero machine that is Z all way up and table to the left all thw way and as close to the door, this is the reference point of the machine.
the G54 through G59 are zeros of each part, or NCS. But also if you use G91 where you are standing at the time of execution becomes a zero relative to that precise standing point. If not clear let me know.

What is NCS? This term is used a lot, but I'm afraid I don't understand what it is.

Re: your original question about bugs: You are loading tool number 8 into the spindle without ensuring that the spindle is empty. I don't see any command to do this though.

You ask about already compensating for height, but up until the tool is loaded and the G43 command is given, the tool is set all the way up, so I'm not seeing a way to crash, but does this then affect the actual position of the G91 G28 call? that could offset the actual location by the height of the tool, and then we do it again with the G43 command, compounding the error EXCEPT you already cleared everything with G15 G17 G40 G80;, so once again, the only trouble seems to be if the spindle is not empty.

 

[Syaminab]

Re: Find the Errors in the first program

What is NCS? This term is used a lot, but I'm afraid I don't understand what it is.



Re: your original question about bugs: You are loading tool number 8 into the spindle without ensuring that the spindle is empty. I don't see any command to do this though.

You ask about already compensating for height, but up until the tool is loaded and the G43 command is given, the tool is set all the way up, so I'm not seeing a way to crash, but does this then affect the actual position of the G91 G28 call? that could offset the actual location by the height of the tool, and then we do it again with the G43 command, compounding the error EXCEPT you already cleared everything with G15 G17 G40 G80;, so once again, the only trouble seems to be if the spindle is not empty.

NCS is the Zero of the parts on the table, WCS is the world cordinate system or machine coordinate system or zero of the machine.
Good try, your problem is that you give for granted we cleared everything....Review those codes, I`m missing maybe a G49? So if the tool is loaded on the spindle and compensated and you did not cancel the lenght compensation and compensate again with G43, the machine will wreck the tool against the part, ruining the part and tool.....This is serious:angry:. So be very careful with standardizing a good heading that will cover you for that. And a good end that will cancel compensations used by you. One more error to clear....

 

[Hawkeye]

Re: Find the Errors in the first program

One more error to clear....

Are you referring to the G04 line? It shows X10. Dwell time would be more like P10000, wouldn't it?

 

[MikeWi]

Re: Our First Program, Explaining a Heading with preparatory commands, Body and end of program.

G15 G17 G40 G80; ( We cancell polar coordinates, We choose the XY Plane, We cancell any lenght compensation and We cancell any Automatic Cycle left with G80, which we have not seen yet until we see cycles)

What I took for granted is that your description was accurate! LOL Looks like this should have read "radius compensation" instead of length. Sneaky.

 

[Syaminab]

Re: Our First Program, Explaining a Heading with preparatory commands, Body and end of program.

What I took for granted is that your description was accurate! LOL Looks like this should have read "radius compensation" instead of length. Sneaky.

Right my friend, review programs, dont rely on previous written programs no matter who wrote them...machines are not to blame because of wrong edited old programs, rivalry among operators or tools changed on the magazine and not eliminated or edited on the program left on the memory. All previous major forms of wrecks.

Fellow Machinists, please dont take it wrong, anyone can learn the codes and programming from a book, but experience on common accidents with CNC....good value!

 

[angelfj1]

[FONT=&amp]"M30; (End of program, Rewind and open the door)[/FONT]" per previous, isn't "M02", end of program and not "M30"?

you keep referring to "the door", as in the following:

[FONT=&amp] G28 Y0.0 (sends the part near the door)

[/FONT] [FONT=&amp]M30 (Program end, Rewind or go to the beginning of the program again, and open the door, is used always at the end of programs for production)[/FONT]


[FONT=&amp]G28 Y0.0; (Moves the part close to us and the door for inspection)[/FONT]


[FONT=&amp]M30; (End of program, Rewind and open the door)
[/FONT]
[FONT=&amp]Please explain.

Thank you,

Frank

[/FONT]

 

[Syaminab]

[FONT=&amp]"M30; (End of program, Rewind and open the door)[/FONT]" per previous, isn't "M02", end of program and not "M30"?

you keep referring to "the door", as in the following:

[FONT=&amp] G28 Y0.0 (sends the part near the door)

[/FONT] [FONT=&amp]M30 (Program end, Rewind or go to the beginning of the program again, and open the door, is used always at the end of programs for production)[/FONT]


[FONT=&amp]G28 Y0.0; (Moves the part close to us and the door for inspection)[/FONT]


[FONT=&amp]M30; (End of program, Rewind and open the door)
[/FONT]
[FONT=&amp]Please explain.

Thank you,

Frank

[/FONT]

Dear Frank, M30 does three things at the same time, it ends the program by stoping the spindle, it sends the cursor to the beginning of the program to start again, and opens the door lock for you. CNC machines have an enclosure and a door with a lock. To open this lock certain conditions or permisive must all occur, the door will not open if the spindle is running, the machine wont start if the door is open, etc.

 

[Syaminab]

Review, How a heading and End of program should be...Recipee.

From the past Chapters, here is a recipee on how the heading and end of a program should be, Please write the next in your hardcover notebook:
Warning: This heading and end considers you set the NCS at the highest point of the block, in forthcomming programs we will learn that if the NCS will disappear when machinning it is better to set the NCS at the bottom, then the Z0.5 to begin machinning and end should be according to the size of block.
Program Heading
O####
%
G15 G17 G40 G49 G80;
G20 G54;
G91 G28 X0.0 Y0.0 Z0.0;
M06 T#;
M03 S####;
G90 G00 X0.0 Y0.0;
G43 Z10.0 H#; (Calculate that the difference between the tool lenght and the tool probe is less than 10 inches)
G00 Z0.5 M08;

Body of program goes here, in other words, the actual cutting of the part or Trajectories.

Program End
G01 Z0.5;
G04 X10.;
G00 Z10. G40 G49 M09;
G91 G28 Z0.0 M05;
G28 Y0.0;
M01;
M30;
%
:whistle:

 

[Syaminab]

Fellow Friends, shall we stop to resolve doubts here, or can I continue with Cycles.

This is the time for questions, If you do not have any I would like to continue with Drilling Cycles, Tapping etc.:whiteflag:
sorry to speed up, but if works comes to the shop, I will be tied...

 

[Syaminab]

Drilling Cycles

As told before, A Simple Gcode can have a lot behind...Let`s learn How to automate drilling on the CNC.
G80, used briefly on our last program, before seeing its meaning, It is used to Cancel any left cycles on the heading, Here we use it to cancel the cycles we will be running.

The First Drilling is a Simple Drilling with a G81 Code, the program line should be written like this:

G98 G81 X#.# Y#.# R# Z-#.# F#

G98 ( The retraction point will be the last Z the spindle was before initiating the Cycle, If I Had the Z10.0 we have been using, it will go up there after drilling. Instead if I write G99, the retraction will be to point R described below.

X, Y (are the coordinates of where you need the hole).
R ( Written as R0.3, is the height above the block at which we can move Safe but close to drill several holes, ahead it will be useful to determine when Pecking the height we need to widraw the drill bit to clean).
Z-1.345 (The total depht of the hole, take into account the 118º angle of the point of the drill, if you want to go through, and where you are supporting the part...Dont drill the bedways of your press)
Feed at which you need to drill, too much brakes the drill, to few burns or dulls the bit edges...How to know:

In Inches:

Rpms of the Drill = (Cs * 4)/D; With a CS for Steel = 60 Ft per minute, Cs for Aluminium = 60, Cs for Castings =40
Feed in Inches per minute: RPMs * Number of flutes * Feed per flute;
Feed per flute as follows:
Small Drill bits: .001 to .004 per flute
from 1/4 to 1/2: .004 to .007
From 1/2 to 1": .007 to .015"

If the Swarf is Black, you are spinning too fast, If is Golden, you are just right. If it curls instead of breaking, more feed, so go from low to high.
Example:

Want to drill a 3/16 hole, on Carbon 1020 steel to 1/2" depth with a HSS drill bit at three different places.
Rpms are : (60* 4)/0.1875=1,280 rpms Feed: 1280*2*0.003=7.6" per minute.

So we write the program:
M06 T12;
M03 S1280;
G00 X 4.5 Y6.7;
G43 Z10.0 H12 M08;
G99 G81 X4.5 Y6.7 R0.5 Z-0.5 F7.6;
Y8.2;
Y9.5;
G00 Z10.;
M09;
M05;
G80;
M30;


G81 Takes care of everything almost... Great help no?:thinking: