Cnc Course in hobby machinist

[Syaminab]

i must have missed something. . . i have g01 thru g04 then g15 to g49/ where are g05 thru g14 ?

Those codes will hardly ever be applied and are specific of peripheal equipment that hardly anyone will use, if you still want them I will send them to you offside.

 

[Ray C]

Re: Chapter One, a brief description...

Question about the 1st lesson... You mention in the 1st line below that Z should be moved high to prevent wrecks. Sounds like good advice. Would it be wise to do this? :

G00 Z(some big number); (lift the head up out of the way)
G00 X5.263 Y3.236;
G00 Z0.25;
.
.

Ray

PS: This is great. Really appreciate the effort you're putting into this.

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 fist 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)

 

[Syaminab]

Re: Chapter One, a brief description...

Question about the 1st lesson... You mention in the 1st line below that Z should be moved high to prevent wrecks. Sounds like good advice. Would it be wise to do this? :

G00 Z(some big number); (lift the head up out of the way)
G00 X5.263 Y3.236;
G00 Z0.25;
.
.

Ray

PS: This is great. Really appreciate the effort you're putting into this.

that is great, but how would you like:
G28 Z0 before anithing, or considering that before moving you changed the tool or loaded one in the spindle....so our effort to move the Z up, was already expected. This is precisely the thinking that make good machinists, they pepare the heading of all their programs with codes that prevent damages to machine. Congratulations Ray, just keep this message, on rapids never put X, Y and Z on the same line.

 

[Syaminab]

Gentleman: We will need a NC plotter very soon, to simulate what you have learned, There are several which I like, but they cost. I recommend Cimco Edit, This software also writes simple codes for you. Also NCPlot is good enough. Im Starting to evaluate Freemill.
If anyone knows of a freeware for students that will suggest code, let you genertate NC code for text engraving and also verify Please start recommending here, as we will need it very soon.:thinking:
Let`s choose one for all.
Regards.
I just finished evaluating FreeMill, is good, but it only lets you postprocess from the wizard, which limits the Machinning operation to Raster Finish. Which is yet too complicated. We need one that will let you do drills, slots, circular milling, Embosses or islands, Tapping so you can really get a feel or writing a program, and it must show you the NC code generated.

 

[DMS]

The demo versions of Dolphin and AlibreCAD/CAM will let you generate code. For simulating, there is GWizard G-Code editor http://www.cnccookbook.com/CCGWizardE.html which has a free trial, but the full version is $99 per year. LinuxCNC is free, and there is a simulation profile. I'm guessing Mach3 has something similar. With linux CNC you download the image and burn it to a CD, then boot off the CD. You don't have to install anything.

 

[MikeWi]

The demo versions of Dolphin and AlibreCAD/CAM will let you generate code.

I'm demoing the home version of AlibreCAD and it won't do that. Or am I missing something? :think1:

 

[DMS]

You need to get the demo version of AlibreCAM too. Things changed since I did my demo, you used to get both through Alibre, now AlibreCAM is handle through MEC Soft. Now that I'm thinking on it.. I'm not sure if the AlibreCAM demo would actually post, which makes it less than useful for these purposes if I am remembering correctly.

FreeMill is another option, which is also made by MECSoft. As Syaminab said though, it's a one trick pony, it only does one flavor of 3d profiling. The generated code is going to be... difficult to follow.

I just recalled another called cambam. I downloaded the demo, but never spent much time with it. It's free as far as I can tell.

http://www.cambam.info/downloads/

 

[Syaminab]

Please quote Cimco Edit and NCplot

Fellow Machinists: Please contact your local dealers of Cimco Edit and NC Plot. Check their prices and if you all agree we will go with them. Let`s find out if they have a Student version that will not DNC, but will allow you to actually see the G code.

They have a download version that will last 30 Days, But at least I need 60 for this Course. :whiteflag:

 

[Syaminab]

Explanation Codes G15-G49

From G15 to G21, you just write them as that, you do not have to enter anything else.

G28 (Usually accompanied by G91, which sets the machine in relative coordinates) Must be written like this:
G91 G28 Z0.0 ( what it will do, is to send the Z axes, as high as possible, regardless of where it is, to the Z0.0 of the machine,
Once we sent the spindle up as high as possible, whe can then move the part near us or all the machine to its reference points by writing:
G28 Y0.0 (sends the part near the door)
G28 X0.0 Y0.0 (Sends the whole machine table to reference points, Usually to the left corner of the machine, close to the front)
G40 H0 (Means that the machine will cancel the tool compensation in radius and take that of the H0 which is the center of the tool, if thid tool is both compensated in lenght and radius, G40 must be cancelled with D0)
G41 D7 (The tool no. 7 will be charged to the left of the given path by the amount written on the Tool 7 Byte in the control)
G42 D7 (The tool no. 7 Will be charged to the right of the given path by the amount written on the Tool 7 Byte in the control)
G43 H7 (Will compensate the lenght difference of the tool no. 7 and the Probe lenght or Main tool) It obeys sign.
G44 Forget it and stay with G43 but be careful to consider the sign, Positive is tool larger than probe, negative if shorter than probe.
G49 H0 (Cancells the compensation for lenght) It must be used everytime we finish using a tool, note that if I was using Tool 7, with G49 I use H0.

If you have doubts, here is the time.
We will continue tomorrow.:bitingnails:

 

[Charley Davidson]

I have ncplot it was given to me by the local mac