Okay, I think my Crashing in CNC mode thread has largely run it’s course and the answer was the Luban software is nowhere near mature enough for serious use in CNC mode. Okay, so the two primary alternatives seem to be Fusion 360 and Carbide Create. Since Carbide Create seems to have the shallower learning curve, I figure I’ll go from there.
Which brings me to the actual question, when generating toolpaths & gcode what machine settings should I use?
First, Chris, Fusion 360 is undergoing use changes. The following link is informative:
Carbide Create is free to use.
Making CNC settings… Speeds & Feeds
Chip load calculations…
https://www.cutter-shop.com/information/chip-load-chart.html
End mill anatomy…
I guess that should be enough information to make a start.
Forgot to add that you should also download Carbide Motion for free.
There is also FreeCAD, it has a full CAM suit, offers the same kind of power as fusion 360 (can be used for 3d modeling and cnc as well as many other things) its also open-source so no risk of it costing money.
Downside is that it is quite complex (like fusion 360) so it has a pretty steep learning curve.
Just wanted you to have all the options, carbide create would be a great choice.
-Atom
Maybe im not able to handle FreeCad right bit i havent found a way to make round carvings yet. CNCing circels is not a problem (on a SN1) but i couldn’t make nice dome shapes so far. (iirc Freecad doesnt support it). Ive looked at BlenderCAM but just briefly as it has some stuff to get used to aswell.
Easel is available and useful.
I have now managed to bring easel files into Luban 3.8.0. Downloading the .zip file gets you an .svg file of your design. Saving the GCode from the Machine tab saves the code and then an Export GCode button appears. The machine tab’s two options must be set to other (grbl) and other. Don’t then set up the machine (although it may talk to snapmaker via a USB lead) just pressed the Advanced link and you get to the save and export options.
You can just export g-code directly from Easel.
Go under machine, click on ‘advanced’ and then generate g-code.
With the pro version t will create two tool paths for two bits, roughing and finishing (flat and v or ball nose)
Rename it .cnc and it works perfectly. Just drag it straight into the workspace
Only annoying thing is you have to remember that it sets origin as bottom left.
So be careful running boundaries!!!
Takes a little bit to get used to centering things.
-S
So with Carbide Create is there something special you have to do with the g-code to make it work with Snapmaker? I just went through and created the tool paths for the lines on my cribbage board and it looked good, the simulation looked reasonable but when I transferred it to the Snapmaker (named appropriated with .cnc), set the origin, verified the work area and told it to start it computed a time estimate of 26 minutes and then it just sat there not doing anything.
So with Carbide Create is there something special you have to do with the g-code to make it work with Snapmaker?
On one of the programs I was playing with it added a pause command. That didn’t work too well.
If you want to post the code I’ll take a look at it.
-S
Here’s the g-code it gave me.
CribbageBoard_Lines3.cnc (205.7 KB)
First few lines:
G90
G21
(LeftCenter)
M05
M0 ;T102
M03S10000
G0X7.28Y29.99Z12.70
G1Z-1.00F203.2
Y341.61F508.0
X87.00
1st three lines are fine but then you have an M05 which is ‘spindle stop’ (which isn’t really necessary)
Then you have an M0 command which is ‘stop and wait for user input’. Which since the SM doesn’t have an unpause or resume input on the controller, just stops everything dead.
Then you have M03S10000 . That should be spindle start, 10000 speed, but I think there needs to be a space between the two: M03 S10000
Actually there’s a lot of places where I think there should be spaces and aren’t (I don’t know if it actually matters or not).
Here’s the start of a simple milling square pass I made using luban:
G21
M3 S12000
G90
G1 Z3.810 F228.6
G0 X100.285 Y3.445
G1 Z-0.500 F240.0
G1 X100.285 Y116.556 F340.0
G1 X97.744 Y116.556 F340.0
Haven’t played with CC at all so I don’t know if there are settings to tell it how to format, or what gcode language you’re using.
You could try eliminating the M0 and then see if it works. That might be enough.
As always, keep your hand on the power switch anytime you’re using code from a new program. I’ve had it try to start doing a 1mm step-down at full travel speed on a piece of oak. Not pretty.
FYI, here’s a good site for decoding commands:
(remember that not all work with SM)
-S
FYI - firmware specifically ignores all spaces. This snippet just removes leading spaces, and there are other sections to ignore all remaining spaces in the line.
FYI - firmware specifically ignores all spaces.
Good to know! That’s the first time I’ve encountered that with the dozen or so different CAM programs I’ve played with.
-S
Okay, so I took the g-code that I posted above and edited out the “M0 ;T102” line and this is what the g-code looked like when I loaded it into Luban.
But when I sent it to the printer to be milled, it produced this:
Any idea what might be going on?
Good lookin pine, that’s a shame.
If nothing else, looks like the travel moves were dragging through the piece, so maybe a z-offset issue.
The …curves…look…artistically interpreted…
I loaded your file into NC Viewer and it plots like Luban shows, but I’m concerned the .CNC file is not being interpreted correctly in the controller - many lines start with X, but that’s not valid gcode according to the controller I think. I’m thinking those moves are being ignored until the next G0 or G1 command comes through, and it does a beeline straight to it.
Here’s the gcode parser in the firmware:
Your file has this:
Y341.61F508.0
X87.00
Y312.41
X86.98Y260.83
Maybe try sending those commands in the console manually? But I don’t think that’s going to do anything.
A simple post-process you can do, load it in notepad++ or some other text editor capable of running regular expressions and do this:
Find: ^([XYZ])
Replace with: G1\1
That will add G1 to the beginning of any line starting with an X, Y, or Z
Looks fine when I load it into Luban and into ncviewer.com too.
It must be a CC setting. It’s beyond what I’ve had experience with. Maybe someone else with more CC experience can chime in.
One suggestion for when you’re first trying to print a new file. Set your z origin 10mm high or so then start to run it. You can see if it’s doing the correct moves and speeds before you even try it on a piece of scrap wood. When I was having problems getting one of my tool paths from a program to not try to run at 3000mm/m for the whole thing, this saved me a bunch of broken bits and wasted material.
-S
What do you get when you throw the resulting gcode into a viewer before hitting a board with it?
alos how much of a step down did you choose? maybe run a test above the actual work surface next time first to see if its making dumb movements again?
Looking at your gcode/cnc file and comparign it to a test generation in Freecad, arent you missing all the Move commands (G0 or G1) at the start of each line? Or is that Luban not needing the infos as it “knows” what to do as its a file with .cnc so it has to be a file where G1/G0 is at teh start of a line unless specified otherwise? Not sure just asking.
Your code:
X86.98Y260.83
X86.97Y220.09
X86.98Y202.92
X87.00Y190.51
X87.01Y178.24
X87.02Y155.52
X87.01Y93.59
X87.00Y8.25
My Code:
G1 X51.768 Y51.768 Z46.000
G2 X52.500 Y50.000 Z46.000 I-1.768 J-1.768
G1 X52.500 Y0.000 Z46.000
G2 X50.000 Y-2.500 Z46.000 I-2.500 J0.000
G1 X0.000 Y-2.500 Z46.000
G2 X-2.500 Y0.000 Z46.000 I0.000 J2.500
G1 X-2.500 Y50.000 Z46.000
G2 X0.000 Y52.500 Z46.000 I2.500 J-0.000
G1 X50.000 Y52.500 Z46.000
Yea, I haven’t seen this syntax either - must be a different flavor of gcode, where if not specified the controller could assume the previous command is still in effect? I like it, would really speed up manual commands, not having to type in G0 every time. But yea, I agree with you, not going to work here.
You could do a find and replace that replaces every X with G1X.
And then every G0G1X with G0X
Same with Z.
-S
Fortunately the pine was the test wood. I bought a 6’ plank and cut it into 18" sections so that I could play around with and get things right before I move on to the Ash and Rosewood.
I’m wondering if there are target machine settings in Carbide Create that offer slightly different flavors of g-code or I could try the find & replace with G1’s and see how that goes but I’d be a little scared I’d just kicked the problem down the road a bit and find some other bit of non-standard code that breaks elsewhere.