Trials Tribulation CNC Milling A Complete Beginner

[ATGNI]

Hello and thankyou for reading my post and any help.

I thought I would start a new thread detailing my journey on learning to operate a small hobby milling machine. I am using Mach3 for machine control and Fusion 360 for generation of the Gcodes. I did start a previous thread about selecting the post processing file in fusion but that thread was very specific whereas I have a whole host of little problems I need some help getting started with, so thought a new thread would be better to consolidate all of those.

I have now managed to load the Mach3Mill post file and I am generating Gcodes. I still don’t have a good understanding of Gcode instructions as yet and this is going to take some time to learn.

After zeroing the DRO XYZ with the tool touching the back left corner of the material and regenerating the tool path when I run the Gcode the milling machine slams into the hard limits and resets. I think that this is something wrong with the Post configuration maybe homing command G28 but not sure what I need to do different. I see that there also some homing option in Mach3 but again not sure what these need to be. I intend to always start my cuts with the tool touching the material datum point so I don’t want the machine to move to the home position as defined by the limit switches.

Hopeful this little video should explain this better. I am trying to do a 2D contour. Note this was just a first test so I had zeroed the DRO well away from the table and just wanted to see the machine trace a the contour in free space.

Any help much appreciated regards Chris

 

[Misterg]

To solve your immediate problem, change the 'Safe Retracts and Home Position' option in the post processor to 'Clearance Height', not G28*.

I intend to always start my cuts with the tool touching the material datum point so I don’t want the machine to move to the home position as defined by the limit switches.

You should only need to home the machine when you first switch it on - It gives the controller a reference to where each axis is.

If you don't home it, you will probably get all sorts of issues with soft limits, or anything that uses machine coordinates rather than work coordinates (e.g. G28, G30, G53, G10 L2) - possibly resulting in a real crash. You would also need to reset your work coordinates every time you switch the machine on (provided the machine is homed, then they should be the same every time).

[* By way of explanation: The G28 command moves to a predefined position. If you haven't defined it, it is probably 0,0,0. If you wished to set the G28 position, then you would move the machine to where you want it to go and send 'G28.1'. The position is stored in machine coordinates, so the machine needs to have been homed before doing this or the position will (effectively) be random, depending on where the axes happened to be when the machine was powered up.]

 

[Hopefuldave]

https://gcodetutor.com/gcode-tutorial/g90-g91-gcode.html is a good place to start!

line 3 G90 G94 G91.1 G40 G49 G17
G90 - sets absolute positioning (relative to the machine's physical zeroes, i.e. home position)
G94 - should be setting feedrate in mm/minute but has no value?
G91.1 - defaults *incremental* positioning, don't think this enables it?
G40 - cancels cutter radius compensation - not sure you want this! can't see G41/42 to set it
G49 - ignores tool length
G17 - sets commands to XY plane (which you want)
Line 4 G21 - specifies mm
(comments)
Line 9 G28 G91 Z0 - looks like this is where it stops... see Misterg's post above! Moves it to the machine's Z=0 reference - guessing this is the upper limit switch?
Line 10 G90

But what do I know?

 

[Misterg]

G90 - sets absolute positioning (relative to the machine's physical zeroes, i.e. home position)

G90 means positions are measured from to the current work coordinate system (WCS) origin. (What you describe is achieved by G53.)

G94 - should be setting feedrate in mm/minute but has no value?

G94 just tells the controller to expect feeds specified in 'units' / minute - just a bit of housekeeping in case a previous program has left the controller in G93 or G95. Actual feeds are specified in the body of the GCode.

G91.1 - defaults *incremental* positioning, don't think this enables it?

G91.1 restores the default behaviour for I,J,K offsets when specifying arcs - of little significance here; just a bit of housekeeping.

G40 - cancels cutter radius compensation - not sure you want this! can't see G41/42 to set it

I suspect that the F360 post applies cutter compensation in the computer by default, hence you wouldn't want the machine to do it too. There is an option in F360 to enable 'on-machine' compensation (in the case where you have a tool table in the machine controller).

G49 - ignores tool length
G17 - sets commands to XY plane (which you want)
Line 4 G21 - specifies mm

Again, just a bit of housekeeping to make sure that the machine is in a known state before anything starts moving.

Line 9 G28 G91 Z0 - looks like this is where it stops... see Misterg's post above! Moves it to the machine's Z=0 reference - guessing this is the upper limit switch?

G28 refers to a user defined position (can be anything), as above, but the G28 command can include axes and offsets in it, so what [ G28 G91 Z0 ] actually means is 'make a rapid move to the Z position of G28 offset by zero' - effectively move to the Z height of G28 without moving the X or Y axes. If the machine hasn't been homed, it doesn't 'know' where the limit switches are. It is likely that homing would set Z=0 at the top limit switch, though. (Also, if G28 has never been set, it may well be at 0,0,0.)

Hopefully I've got that right!

I find this page a handy reference for the basics (although beware that there are different dialects of Gcode).

(Sorry @Hopefuldave - not meaning to pick on you!)

 

[Hopefuldave]

G90 means positions are measured from to the current work coordinate system (WCS) origin. (What you describe is achieved by G53.)


G94 just tells the controller to expect feeds specified in 'units' / minute - just a bit of housekeeping in case a previous program has left the controller in G93 or G95. Actual feeds are specified in the body of the GCode.


G91.1 restores the default behaviour for I,J,K offsets when specifying arcs - of little significance here; just a bit of housekeeping.


I suspect that the F360 post applies cutter compensation in the computer by default, hence you wouldn't want the machine to do it too. There is an option in F360 to enable 'on-machine' compensation (in the case where you have a tool table in the machine controller).


Again, just a bit of housekeeping to make sure that the machine is in a known state before anything starts moving.



G28 refers to a user defined position (can be anything), as above, but the G28 command can include axes and offsets in it, so what [ G28 G91 Z0 ] actually means is 'make a rapid move to the Z position of G28 offset by zero' - effectively move to the Z height of G28 without moving the X or Y axes. If the machine hasn't been homed, it doesn't 'know' where the limit switches are. It is likely that homing would set Z=0 at the top limit switch, though. (Also, if G28 has never been set, it may well be at 0,0,0.)

Hopefully I've got that right!

I find this page a handy reference for the basics (although beware that there are different dialect of Gcode).

(Sorry @Hopefuldave - not meaning to pick on you!)

No offence taken, I'm still new to this, and trying to get my head around it all before I put some coke-can sized steppers to use in a metre cube of ally extrusions! Always keen to learn

I did have to adjust the 1KW psu down from 48 to 40v for the stepper drivers, and I shall see whether an Aldi router is up to the job of light 3D milling*... and LinuxCNC looks like the way to go? I wrote some Arduino code to "exercise" the steppers which worked, but I'm much more low-level programmer than Linux guru....

*I'd like to try 3D carving for an archtop-looking guitar and bass duo, as you do! Then on to casting patterns, I have a Daft Idea or three for one of my bikes...

 

[m_c]

I've not watched the video, but the origin needs to be configured correctly in F360, with the axes pointing the correct way.

Also have you checked that the machine axes move the correct direction when jogged?

Stand in front of the machine, with X running left/right and Y moving towards/away from you
X positive is the table moving left/spindle moving right.
Y positive is the table moving towards you/spindle moving away from you.
Z is typically positive up/away from the table.

 

[Misterg]

LinuxCNC looks like the way to go?

Quite possibly - I've stayed with GRBL (& its 32 bit offshoots) for my machine, but that doesn't mean it's right!

 

[ATGNI]

Thanks Everyone

Such a lot of information here for me to take in.

I had a little toy machine router running GRBL and have to admit was very easy.

I have been watch the Gcode Tutor, what amazing videos such well taught. I was actually thinking of paying for a course as its not much different than buyying an expensive tools etc and nothing better than Knowlledge in the toolbox.

I guess Im still a bit confused why I have to do any of this homing stuff. I assumed I could set the tool to the material edge that corrisponds to the start point withing fusion CAM then Zero out the the X Y Z and just press start. To me this appear to very very complicated. Its like learning to fly by first jumping off a cliff!

Going to try Daves suggestion on fusion post config - dont use g28

Have printed off the Gcode reference guide Thanks

Last time I used Gcode I was at Salford Technical colledge 30 years ago. We wrote the code using grid paper then simulated it on green screen Comadore Pets computers. I think we cut out a block of foam using a converted bridgport. Happy days to be 18 years old again

Chris

 

[ATGNI]

Ok tweaked the config and generated new code. Giving that a try now

(1001)
(T3 D=10. CR=0. - ZMIN=-6. - FLAT END MILL)
G90 G94 G91.1 G40 G49 G17
G21
(-ATTENTION- PROPERTY SAFE RETRACTS IS SET TO CLEARANCE HEIGHT.)
(ENSURE THE CLEARANCE HEIGHT WILL CLEAR THE PART AND OR FIXTURES.)
(RAISE THE Z-AXIS TO A SAFE HEIGHT BEFORE STARTING THE PROGRAM.)
(WHEN USING FUSION 360 FOR PERSONAL USE, THE FEEDRATE OF)
(RAPID MOVES IS REDUCED TO MATCH THE FEEDRATE OF CUTTING)
(MOVES, WHICH CAN INCREASE MACHINING TIME. UNRESTRICTED RAPID)
(MOVES ARE AVAILABLE WITH A FUSION 360 SUBSCRIPTION.)

(2D CONTOUR2)
T3 M6
S1000 M3
G17 G90 G94
G54
M8

 

[ATGNI]

Success

thanks guy. Until the next time. Don’t worry you won’t have very long to wait.

 

[Misterg]

I guess Im still a bit confused why I have to do any of this homing stuff. I assumed I could set the tool to the material edge that corrisponds to the start point withing fusion CAM then Zero out the the X Y Z and just press start.

You *can* do just that.

However if you do, you won't be able to do any of the stuff that the machine needs an absolute reference for. Off the top of my head:

Soft limits (these will trigger seemingly at random because the machine thinks it is exceeding its travel - you'll probably have to disable them which is one less layer of error proofing);
Having a tool length probe;
Run any macros that use G28, G30, G54, etc;
'Remembering' WCS offsets through power cycles (once you fit a vice, it's really handy to have the end of the fixed jaw as a WCS origin. Re-establishing it every time gets old).
etc.

Whether this matters is up to you

 

[ATGNI]

The Best Way To Avoid Learning Speed And Feed

Yes I’m sure you’re correct. I don’t know what I don’t know yet.

I have only cut air so far, but this morning it’s going to be some aluminium. given my small experience with manual machining I set feeds by eye no idea how many mm per minute this is. I had most of my contours set at 1000mm for a 10mm two flute slot drill. Watching the machine cutting air this looked faster than I would have turned the hand wheels so I think I will try 500. i am very very experienced at breaking small milling cutter and drills, so i think slow is better. My thoughts is that all the published feed and speed data has been developed for production and rigid industrial machine. Does any one have any tables more applicable to hobby mills. I had a quick google but didn’t find anything. The spindle speed on my machine I think maxes out a 2000. But a lot of cutter data in fusion state’s figures like 15k

Video coming today making swarf.

Thanks

Regards Chris

 

[Misterg]

I have only cut air so far, but this morning it’s going to be some aluminium. given my small experience with manual machining I set feeds by eye no idea how many mm per minute this is. I had most of my contours set at 1000mm for a 10mm two flute slot drill. Watching the machine cutting air this looked faster than I would have turned the hand wheels so I think I will try 500. i am very very experienced at breaking small milling cutter and drills, so i think slow is better. My thoughts is that all the published feed and speed data has been developed for production and rigid industrial machine. Does any one have any tables more applicable to hobby mills. I had a quick google but didn’t find anything. The spindle speed on my machine I think maxes out a 2000. But a lot of cutter data in fusion state’s figures like 15k

1) Check your cutting speed: pi x cutter dia(mm) x RPM/1000
3.14 x 10 x 2000/1000 = 62 m/min

You don't say whether it is a carbide or HSS cutter, but (IMHO) this is pretty low for aluminium in any case, so run at max RPM. (I work on ~160m/min for carbide cutters in aluminium on my desktop cnc).

Cutter manufacturers publish recommended cutting speed (vc) for various tools / materials.

2) Work out your 'feed per tooth' at your chosen RPM:

A 2 flute cutter at 2000 RPM makes 4000 cuts/minute.
500 mm/minute feed rate means that each cut will be 500/4000 = 0.125mm

Cutter manufacturers also include 'feed per tooth' in their data (fz)- typically ~0.05mm for a 10mm carbide cutter from the Guhring datasheet I've got in front of me. (I work on about 0.01mm for my little machine).
0.05mm feed per tooth, with a 2 flute cutter at 2000 RPM (4000 cuts/minute) equates to 0.05 x 4000 = 200mm/min feedrate.

*I* would start there and see how it went.

The amount of material you can remove (depth / width of cut) depend on how rigid your mill is, and how powerful your spindle is - trial and error required!

P.S - the default feeds and speeds in F360 tend to be very aggressive IMHO. I certainly wouldn't recommend accepting their defaults!
The 'tool' tab in F360 gives you the cutting speed and feed per tooth when you enter the RPM and feed, so no need for the maths above.

PPS - slow feed down by at least 50% if slotting.

 

[m_c]

The key feed/speed component is feed per tooth.
Too low (very common approach by inexperienced users) and the tooth rubs resulting in poor surface finishd/blunt tools.
Too high and the tool will likely snap/chip.

I'd suggest trying some figures in a feeds and speed calculator, but be aware that you'll likely have to adjust them to suit your machine.

 

[ATGNI]

Thanks

I am aware of cutting speed and how to calculate them, I just dont find the need to do it as process times not really a thing for me. For Small tools go as fast as your spindle will go, big tool go slower than you think.

What I am saying is they are pretty meaningless for small hobby machines as they dont have either the rigidity, spindle torque or with the exception of router the spindle speed. historically my preffence is for HSS tooling because it is sharper generally produces a better finish and requires less power. I was really enquiring if anyone with a similiar hobby mill to my own had a cheat sheet for what works for them. Im guessing something out of model engineering box rather than machinery handbook.

Yes I think the feeds and speeds in fusion are very agressive, my defualt will be 40 percent of suggested feed . The good thing about Mach 3 is I can change the feed rate on the fly if it doesnt sound right.

off out now to break some 5mm slot drills!

Thanks

 

[Misterg]

I am aware of cutting speed and how to calculate them, I just dont find the need to do it as process times not really a thing for me.

Process times are pretty much irrelevant - you need the tool to have a manageable chip load which is what the 'feed per tooth' calculation achieves. You won't get 'production speeds' because you're only spinning the tool at 2000 RPM, so your surface speed is way low, and you probably won't push either the depth or width of cut. The 'feed per tooth' is pretty much fundamental. Once you've decided on a value you're comfortable with, everything else follows. I think you'll be in for a frustrating time if you ignore this

There are 'cheat sheets' for hobby machines (like this one in inches), but they will only be of limited use as they assume a high speed spindle, and will be limited by a relatively flimsy machine. (You can scale the feed rates by RPM if you want to try and use them 8 feet/min (2400 mm/min) @9000 RPM will be the same load as 1.77 feet/min (540mm/min) @2000 RPM).

For Small tools go as fast as your spindle will go, big tool go slower than you think.

Just keep an eye on your surface speeds to make sure you don't burn up your HSS tool (pretty unlikely at 2000 RPM on aluminium, but possible on ferrous).

Good luck!

 

[ATGNI]

WHEN FAILURE IS A SUCCESS

 

[m_c]

I'm surprised the glue/tape held for as long as it did.

Tape/glue really isn't a good option for anything more than very light cuts.
Depending on what you plan to machine, I'd be looking at more suitable/secure workholding methods.

 

[ATGNI]

in the past I have done ok with this method it actually worked well. I think the heat of the day caused this failure. I think I will use the vice next.

 

[Wedg1e]

Rather than blowing the chips everywhere with an airline, I'd vacuum them up...