-
Welcome back Guest! Did you know you can mentor other members here at H-M? If not, please check out our Relaunch of Hobby Machinist Mentoring Program!
Cnc Course in hobby machinist
- Thread starter Syaminab
- Start date
- Joined
- Jan 21, 2013
- Messages
- 871
All I can find for Cimco Edit is links to their product description and trial download, but no prices, even at the re seller web sites, so I must be missing something. NCPlot is $300 and is way outside my budget right now. Not complaining, just providing feedback. If I have to follow along with the software, that's what I'll do! 
)
)Ok, to me $300 seems to high for student also. Let`s find out if Cimco Edit is under US$150.00 I would recommend it if it was. The thing here is that I will start posting programs in the near future, probably a week or less from now and this software have the feature of giving examples, and posting the code and line in red if something is wrong or missing. They help you a lot to learn and work faster. Without a simulating software, The student abandones because he can`t see what the programs do, and having a CNC is way more expensive than a software. Also this software is an investment, because it will let you program in the near future a lot faster and without mistakes, also will help you to quote, estimate materials, hours of work and the list of tooling needed.All I can find for Cimco Edit is links to their product description and trial download, but no prices, even at the re seller web sites, so I must be missing something. NCPlot is $300 and is way outside my budget right now. Not complaining, just providing feedback. If I have to follow along with the software, that's what I'll do!
I highly recommend their use. I do not recommend scaling to Softwares like MasterCam, SurfCam and so on, because they will not be helpful for learning and understanding the Code. Something I see here, among hobbiest, is that they like to control the machine and make the parts, Not program a software to do the parts for them. It is the closest to have the real satisfaction feeling of doing the parts on conventional for yourself, with a CNC.
Chapter Three, GCodes G50-G59, Cycles will be skipped for the moment to grant a program G90-G99
G50 (Scaling Cancellation)
G51 (Scaling, Requires a Center in I, J, K and P as the Scaling Factor) It should be written like this
G51 I0.0 J0.0 K0.5 P1.05 (In here we are leaving 0.050" oversize for a final pass for finish, It can also be negative, for fitting and assembly purposes)
G54 through G59 (Workpiece Set point or 0 point, also called UCS, If you are working on several pieces on the table of the machine, you may use several ucs)
G90 (Absolute mode command, This orders the machine to move considering the complete UCS, counting as 0 the G54-G59 Chosen)
G91 (Relative or increment mode command, This orders the machine to count starting where it is standing, let`s say you have a UCS at the top of the lower corner of a part, then you find the center of that plate and want to move from there only one inch, if you turn to G91 then, instead of adding the distance from the corner to the center plus the inch, you just write the inch)
G94 (Feed per minute)
G95 (Feed per rotation, I advise to use this one a lot, specially on drilling because they last longer as they are always biting the same amount of metal, problem is that once starting to run they will be tied to the spindle rotation as if you where tapping, so the feed rate can not be slowed, only the RPMs.
G98 (Return to initial point in a canned Cycle)
G99 (Return to R given point in Canned Cycle, Will explain these on drilling cycles)
Well, Now we are set with G`s, let me teach some M so we can start writing our first program for understanding.
G50 (Scaling Cancellation)
G51 (Scaling, Requires a Center in I, J, K and P as the Scaling Factor) It should be written like this
G51 I0.0 J0.0 K0.5 P1.05 (In here we are leaving 0.050" oversize for a final pass for finish, It can also be negative, for fitting and assembly purposes)
G54 through G59 (Workpiece Set point or 0 point, also called UCS, If you are working on several pieces on the table of the machine, you may use several ucs)
G90 (Absolute mode command, This orders the machine to move considering the complete UCS, counting as 0 the G54-G59 Chosen)
G91 (Relative or increment mode command, This orders the machine to count starting where it is standing, let`s say you have a UCS at the top of the lower corner of a part, then you find the center of that plate and want to move from there only one inch, if you turn to G91 then, instead of adding the distance from the corner to the center plus the inch, you just write the inch)
G94 (Feed per minute)
G95 (Feed per rotation, I advise to use this one a lot, specially on drilling because they last longer as they are always biting the same amount of metal, problem is that once starting to run they will be tied to the spindle rotation as if you where tapping, so the feed rate can not be slowed, only the RPMs.
G98 (Return to initial point in a canned Cycle)
G99 (Return to R given point in Canned Cycle, Will explain these on drilling cycles)
Well, Now we are set with G`s, let me teach some M so we can start writing our first program for understanding.
Chapter Four, The M codes
M00 (Program Stop, used at the middle of programs to test a Thread or add a component that must be machined)
M01 (When the Optional Switch on the machine is on, The program stops as M00. Used on the cycles where an optional stop is needed, to check for wear of a tool or measure the part only every so many parts in production runs)
M02 (End of program)
M03(Spindle rotation Clock Wise seen from behind the spindle)
M04(Spindle rotation CCW) Both are used as: M04 S1300, that is spindle CCW at 1300rpms.
M05 (Spindle rotation stop)
M06 (Tool Call, written as M06 T7, To load Tool 7 on the spindle)
M08 (Coolant on)
M09 (Coolant off)
M19 (Spindle orientation, it orients the spindle in preparation to a tool change, or if you are using a probe, to always use the same side)
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)
M54 (I should say part count, but indeed is cycles run counter)
M98 (Subprogram Call)
M99 (Subprogram End, this last two are used often on programs that may use different subprograms to do family parts)
I know they are more than Five, but we are now ready to Start a program....)
M00 (Program Stop, used at the middle of programs to test a Thread or add a component that must be machined)
M01 (When the Optional Switch on the machine is on, The program stops as M00. Used on the cycles where an optional stop is needed, to check for wear of a tool or measure the part only every so many parts in production runs)
M02 (End of program)
M03(Spindle rotation Clock Wise seen from behind the spindle)
M04(Spindle rotation CCW) Both are used as: M04 S1300, that is spindle CCW at 1300rpms.
M05 (Spindle rotation stop)
M06 (Tool Call, written as M06 T7, To load Tool 7 on the spindle)
M08 (Coolant on)
M09 (Coolant off)
M19 (Spindle orientation, it orients the spindle in preparation to a tool change, or if you are using a probe, to always use the same side)
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)
M54 (I should say part count, but indeed is cycles run counter)
M98 (Subprogram Call)
M99 (Subprogram End, this last two are used often on programs that may use different subprograms to do family parts)
I know they are more than Five, but we are now ready to Start a program....
)Our First Program, Explaining a Heading with preparatory commands, Body and end of program.
Well, Finally, let`s see our first easy program, Just making a Slot. First we are to write a heading that will assure several things, that the machine is safe to use, that we are planning different planes and commands on machine, That automatic cycles that could have been left running are cancelled, That we are in Cartesian Coordinates, etc. let`s write the first part of the heading.
O2455 (The O, not a cero, but an o followed by the four digits denotes program number for controll in the memory of the control)
% (Tells the control a program fallows)
G15 G17 G40 G49 G80; ( We cancell polar coordinates, We choose the XY Plane, We cancell any lenght and radious compensation and We cancell any Automatic Cycle left with G80, which we have not seen yet until we see cycles)
G20 G54;(We set Inches in the machine units mode and set the G54 NCS (Part Coordinate System)
G91 G28 X0.0 Y0.0 Z0.0; (Sends the machine to the initial Reference point To clear the table in preparation to load a tool)
M06 T8; (Loads the tool number 8 in the spindle)
M03 S1200; (Start the spindle spinning CW at 1200 rpms)
G90 G00 X0.0 Y0.0; ( We set absolut command mode and send the spindle in rapid mode to the NCS in X and Y only, Not in Z to avoid wrecking )
G43 Z10.0 H8 (While moving the Z axe to 10.0 we compensate the difference in lenght between our tool probe and the tool in use)
G00 Z0.5; ( We then move in rapids half an inch above the part NCS)
G42 X2.5 Y2.5 D8 F25; (We compensate the Radius of Tool 8 and move to X2.5 Y2.5)
G01 Z-0.5 F20 M08( We start our cut by penetrating the part down to Z-0.5 at a feed rate of 20 inches per minute with coolant)
G01 X5.0 Y5.0 F40; (We start our cut going to a point X5 Y5 at a feed rate of 40 IPM)
G01 Z0.5; (After making a slot at the right of an invisible line that runs from X2.5 Y2.5 to X5.0 Y5.0, the spindle exits the part at a feed rate of 40IPM)
G04 X10.; (Washes the part during 10 seconds to eliminate swarf)
G00 Z10. G40 G49 M09; (We send the spindle to Z10 in rapid mode while cancelling the compensation for lenght and radius of tool, and shuts off the coolant after having washed a little the part )
G28 Z0.0 M05; (Sends the spindle as high as possible and stops the spindle)
G28 Y0.0; (Moves the part close to us and the door for inspection)
M01; (If optional stop Switch on, waits for us to inspect the part, when we finish the inspection we must press start again in the panel board)
M30; (End of program, Rewind and open the door)
%
This is more less a program first debug. If you find problems, let us know.
Well, Finally, let`s see our first easy program, Just making a Slot. First we are to write a heading that will assure several things, that the machine is safe to use, that we are planning different planes and commands on machine, That automatic cycles that could have been left running are cancelled, That we are in Cartesian Coordinates, etc. let`s write the first part of the heading.
O2455 (The O, not a cero, but an o followed by the four digits denotes program number for controll in the memory of the control)
% (Tells the control a program fallows)
G15 G17 G40 G49 G80; ( We cancell polar coordinates, We choose the XY Plane, We cancell any lenght and radious compensation and We cancell any Automatic Cycle left with G80, which we have not seen yet until we see cycles)
G20 G54;(We set Inches in the machine units mode and set the G54 NCS (Part Coordinate System)
G91 G28 X0.0 Y0.0 Z0.0; (Sends the machine to the initial Reference point To clear the table in preparation to load a tool)
M06 T8; (Loads the tool number 8 in the spindle)
M03 S1200; (Start the spindle spinning CW at 1200 rpms)
G90 G00 X0.0 Y0.0; ( We set absolut command mode and send the spindle in rapid mode to the NCS in X and Y only, Not in Z to avoid wrecking )
G43 Z10.0 H8 (While moving the Z axe to 10.0 we compensate the difference in lenght between our tool probe and the tool in use)
G00 Z0.5; ( We then move in rapids half an inch above the part NCS)
G42 X2.5 Y2.5 D8 F25; (We compensate the Radius of Tool 8 and move to X2.5 Y2.5)
G01 Z-0.5 F20 M08( We start our cut by penetrating the part down to Z-0.5 at a feed rate of 20 inches per minute with coolant)
G01 X5.0 Y5.0 F40; (We start our cut going to a point X5 Y5 at a feed rate of 40 IPM)
G01 Z0.5; (After making a slot at the right of an invisible line that runs from X2.5 Y2.5 to X5.0 Y5.0, the spindle exits the part at a feed rate of 40IPM)
G04 X10.; (Washes the part during 10 seconds to eliminate swarf)
G00 Z10. G40 G49 M09; (We send the spindle to Z10 in rapid mode while cancelling the compensation for lenght and radius of tool, and shuts off the coolant after having washed a little the part )
G28 Z0.0 M05; (Sends the spindle as high as possible and stops the spindle)
G28 Y0.0; (Moves the part close to us and the door for inspection)
M01; (If optional stop Switch on, waits for us to inspect the part, when we finish the inspection we must press start again in the panel board)
M30; (End of program, Rewind and open the door)
%
This is more less a program first debug. If you find problems, let us know.
Last edited:
- Joined
- Jan 21, 2013
- Messages
- 871
Re: Find the Errors in the first program
Some things aren't clear to me. is 0.0 the maximum height above the table? Z10 appears to lower the end of the endmill to 10 inches from that point, but then we move to .5 to go above that point? If positive descends, wouldn't another positive lower an additional .5? You then move -.5 so in any case, we're back to the starting point from that h10 move, not below the surface of the work, or, we descended .5 into the work and then returned above it before cutting the slot.
Also, how does this work? are all movement commands relative to the last position? :think1:
Some things aren't clear to me. is 0.0 the maximum height above the table? Z10 appears to lower the end of the endmill to 10 inches from that point, but then we move to .5 to go above that point? If positive descends, wouldn't another positive lower an additional .5? You then move -.5 so in any case, we're back to the starting point from that h10 move, not below the surface of the work, or, we descended .5 into the work and then returned above it before cutting the slot.
Also, how does this work? are all movement commands relative to the last position? :think1:
Re: Find the Errors in the first program
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.
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.
- Joined
- Jan 22, 2011
- Messages
- 8,031
Rapid Output markets an old standard package that's been around quite a while called G-Zero. Nothing fancy, at least back when I was using it. I just looked and they have a Student version with a 90 day free trial on their mill package. Probably lathe package as well.
http://www.g-zero.com/1157/index.html
Glad you guys are enjoying this. And I'm glad you've got an instructor willing to share what he knows. Just be sure and ask questions as you go along rather than wait and bombard him at the end. And he's right.....take notes.
The G-Zero is an industrial grade program, but it will generate code and plot tool paths that help prevent crash moves. Have fun with it.
http://www.g-zero.com/1157/index.html
Glad you guys are enjoying this. And I'm glad you've got an instructor willing to share what he knows. Just be sure and ask questions as you go along rather than wait and bombard him at the end. And he's right.....take notes.
The G-Zero is an industrial grade program, but it will generate code and plot tool paths that help prevent crash moves. Have fun with it.