Trying to learn, Im using this calculator Chipload Calculator | GDP Tooling to find feedrate for chipload.
11.78 mm/min for MDF. Question is how should i enter this into my software, im using rhinocam, do i enter 1178? 11.78 is way too slow…
Your units differ. You are entering 11.78 mm/min ant the calculator says 11.78 m/min. You would have to enter 11,780 for mm.
1 Like
i do have set my masso units to mm. It does not work, still too slow, does onefinity elite masso read the gcode in mm/min or do i need to change to units in the gcode to inch/min.
In the Masso setup you select mm or inch and in your cad program you also select the units you want to work in. You should keep both same. Just pick one.
1 Like
i have cad/cam software set to mm and masso to mm, what i dont understand is that how should i enter the feedrate in mm/min 11.780 or 1178… 11.780 is way too slow.
Masso doesnt read the code in mm/m? i changed the unites to inch and back to mm, its the same feedrate speed. Do i need to use Inch/m ?
Here is example code start of the toolpath.
%
G21
G90
(2 1/2 Axis Facing)
(Amana 46202-K )
M6T2
M3 S18000
G0 Z15.250
G0 X-110.497 Y0.011
G1 Z-3.675 F11.780
G1 Y-105.302 F11.780
G17
G3 X-108.497 Y-107.302 I2.000 J0.000
G1 X108.497
G3 X110.497 Y-105.302 I0.000 J2.000
G1 Y105.302
G3 X108.497 Y107.302 I-2.000 J0.000
I am using Rhinoceros 3D & Rhinocam, and the value I enter in rhinocam is saved to gcode, it should output the fvalue in the gcode, something is wrong. I just read this.
F values
The F values stand for feed rate, but essentially mean the speed at which the extruder is traveling. F values are in terms of mm/min, so just divide by 60 to get mm/s (ex: F300 = 5 mm/s). There are two types of speed: travel and printing. Travel speed is how fast the extruder moves while not extruding. This is a setting in slic3r and can be set independently of material type. Print speed is how fast the extruder moves while extruding material. This is a printing parameter that is depending on the bioink used.
GCode FValue is not in MM or inches. so if i want feed rate 11.78 m/m, 11.78 * 60 = F706.8. The feed rate in the code should be F706.8? Is this correct? does anyone know?
I think i fixed it, i had to change my post processor settings.
Hey Patrick, hey Rob, hey Woodpecker, hey all,
F: Set Feed Rate
Fx - set the feed rate to x. x is usually in machine units (inches or millimeters) per minute.
The application of the feed rate is as described in the Feed Rate Section, unless inverse time feed rate mode or feed per revolution mode are in effect, in which case the feed rate is as described in the G93 G94 G95 section.
G20, G21 Units
G20 - to use inches for length units.
G21 - to use millimeters for length units.It is a good idea to include units in the preamble of each G-code file.
Often feed rate is given in m/min, e.g. here in this feed rate table, this is 1000 * mm/min.
See also
1 Like
I just want to know how do i enter the feedrate in GCODE manually and not in the software. It seems like the software postprocessor converts it to another number.
Using calculator: 18000RMP | 2 Flutes | 11.78 m/m Feedrate | Chipload 0.013
11.78 * 60 = F706.8
Is F706.8 Correct? Can anyone explain.
Here is a toolpath from carveco, i entered 11.78 and output in GCODE is F707.
N10(testfeedrate1)
N20(Masso Carveco Post Processor 2023)
N30(Post Processor version Metric v1.1)
N40(Material Size) (X=146.000, Y=1500.000, Z=10.000)
N50 G17
N60 G21
N70 G80
N80 G90
N90 G00
N100(Tool Number:1) (6.000 mm dia. slot drill)
N110 T1 M06
N120 M08
N130 S15000 M3
N140 G00 X15.929 Y1424.960 Z40.000
N150 G01 Z9.000 F707 <----------------------------------------------------------------------
N160 G01 X128.301
N170 G00 Z40.000
N180 G00 X0.000 Y0.000
N190 G00Z40.000
N200 G00X0.000Y0.000
N210 M05
N220 M09
N230 M30
Hey Patrick,
If G20 is set, “F706.8” means 706.8 inches/min. if G21 is set, “F706.8” means 706.8 mm/min.
Note that using “N” codes as line numbers is obsolete. The lines are usually counted by the line number of the g-code file. Many people know numbered lines from BASIC programming language but they were abandoned a long time ago (see GOTO #Criticism). In G-code, if you want to jump to a specific line, you use a “O” subroutine.
I know that today the CAM software provides the N numbers, but that makes the code quite illegible.
Before:
N10(testfeedrate1)
N20(Masso Carveco Post Processor 2023)
N30(Post Processor version Metric v1.1)
N40(Material Size) (X=146.000, Y=1500.000, Z=10.000)
N50 G17
N60 G21
N70 G80
N80 G90
N90 G00
N100(Tool Number:1) (6.000 mm dia. slot drill)
N110 T1 M06
N120 M08
N130 S15000 M3
N140 G00 X15.929 Y1424.960 Z40.000
N150 G01 Z9.000 F707 <----------------------------------------------------------------------
N160 G01 X128.301
N170 G00 Z40.000
N180 G00 X0.000 Y0.000
N190 G00Z40.000
N200 G00X0.000Y0.000
N210 M05
N220 M09
N230 M30
After:
(testfeedrate1)
(Masso Carveco Post Processor 2023)
(Post Processor version Metric v1.1)
(Material Size) (X=146.000, Y=1500.000, Z=10.000)
G17
G21
G80
G90
G00
(Tool Number:1) (6.000 mm dia. slot drill)
T1 M06
M08
S15000 M3
G00 X15.929 Y1424.960 Z40.000
G01 Z9.000 F707 ; <----------------------------------------------------------------------
G01 X128.301
G00 Z40.000
G00 X0.000 Y0.000
G00Z40.000
G00X0.000Y0.000
M05
M09
M30
1 Like
PS:
11.78 m/m is 11780 mm/m which is 463.98 inches/m.
11.78 m/min would be 706.8 m/h, which is a unusual unit. The number F707 after a G21 should be the number in millimeters per minute. 706.8 mm/min is 0.7068 m/min, which would mean 27.82 IPM.
11.78 mm/s would be 706.8 mm/min
For which CNC machine brand is your post processor made?
Just had a look at RS274/NGC reference, there the feedrate is length unit/minute too.
A. For motion involving one or more of the X, Y, and Z axes (with or without simultaneous rotational axis motion), the feed rate means length units per minute along the programmed XYZ path, as if the rotational axes were not movi
This would mean your post processor assumes that it has to be entered in length unit/second.
Hey Patrick,
2.5 Feed rate
The rate at which the controlled point moves is nominally a steady rate which may be set by the user. In the Interpreter, the feed rate is interpreted as follows (unless inverse time feed or feed per revolution modes are being used, in which case see section G93-G94-G95-Mode).
- If any of XYZ are moving, F is in units per minute in the XYZ cartesian system, and all other axes (ABCUVW) move so as to start and stop in coordinated fashion.
– Source: CNC Machine Overview – LinuxCNC
LinuxCNC evolved from the NIST EMC² project, the NIST Enhanced Machine Controller.
LinuxCNC G-code language is based on the RS274/NGC language.
Buildbotics G-code language is a dialect of LinuxCNC G-Code.
Masso G-code is proprietary.
3.5.7 Length Units — G20 and G21
Program G20 to use inches for length units. Program G21 to use millimeters.
It is usually a good idea to program either G20 or G21 near the beginning of a program before any motion occurs, and not to use either one anywhere else in the program. It is the responsibility of
the user to be sure all numbers are appropriate for use with the current length units.
Further reading
1.2 Background*
1.2.1 Enhanced Machine Controller Project
The Intelligent Systems Division of the National Institute of Standards and Technology (NIST) is carrying out an Enhanced Machine Controller project. The primary objective of the project is to build a testbed for evaluating application programming interface standards for open-architecture machine controllers. A secondary objective is to demonstrate implementations of the Next Generation Controller (NGC) architecture.
1.2.2 Numerical Control Programming Language RS274
RS274 is a programming language for numerically controlled (NC) machine tools, which has been used for many years. The most recent standard version of RS274 is RS274-D, which was completed in 1979. It is described in the document “EIA Standard EIA-274-D” by the Electronic Industries Association [EIA]. Most NC machine tools can be run using programs written in RS274. Implementations of the language differ from machine to machine, however, and a program that runs on one machine probably will not run on one from a different maker.
[…]
Im from sweden and dont understand inches. Use metric here.
Trying to explain with pictures how I got the feed rate and entered it into the carveco maker software and it output a F number in gcode. I don’t know if I’m doing it right. does anyone know what im doing wrong? how should i enter the number in carveco i got from the calculator?
Hey Patrick,
I’m from germany and am not used to think in inches either, but according to Onefinity, 95% of the forum users think in Fahrenheit and IPM 
.
Unfortunately, as I see on your screenshot, it does not tell you which unit is meant. But what I wanted to explain above, the internal formula seems to assume it has to be converted by computing the value × 60 (which you already found out).
So if we can assume that feed rate is expected in mm/min at the F code, the number entered into the input field would be mm/s
EDIT: Got it right now.
1 Like
I just got my onefinity up and running a few weeks ago, havnt really used any cnc before and need to learn everyting by myself looking up information. I did mill a test guitar body pickup pocket in MDF today with rhinocam, 5/16" 8mm ENDMILL / Fedrate F706.8 / S18000rpm and it turned out great, but im still unsure if its the correct number.
The pickup pocket is made with rhinocam(not carveco) i use GRBL-mm post processor.
1 Like
Hey Patrik,
11.78 mm/s would be 706.8 mm/min, and this is the unit the F code expects if G21 is set (metric units set).
That is 0.7068 m/min. That sounds reasonable.
PS: yum, a nice EMG
Just planning a reverse headstock with Seymour Duncan SVR-1B and SVR-1N 
1 Like
Nice, Do you build guitars? that’s the reason I bought a cnc to learn how to build my own, I draw guitars in Rhinoceros 3D.
Hey Patrik,
yes, and a few other instruments. Although I started to learn it early in life, I did not make it my main profession. I worked exclusively with hand tools (no power) for at least 25 years (make also my own furniture), but specifically shaping arched tops like on bowed instruments like the gambes and the archtop guitars takes much time and effort so that their price must remain high (too high to choose this as my main profession) so my plan was to buy the CNC (Journeyman) to make these parts, and also necks with it. Yet I did not put it into service, waiting for the next bunch of budget being amassed for the large vaccum table to mill the thickness of the sides and flat backs (and lute tops etc.) and the new workshop with big dust collection system. Already have the machine, the spindle and everything to wire and populate the VFD cabinet.
But sometimes I quickly put a strat-like instrument together with parts that I bought, as is the case with the current project. Parts are from a luthiery supplier from Germany, from Fender, and from Seymour Duncan.
PS: powerless tools: Not 100% true, my glue heater, my soldering iron and my side bending iron are electric But I know how to use cabinet scrapers (instead of sanding paper)!
1 Like
It looks like you are entering 11.78 as your feedrate which shows in your screenshot as Metres/Minute instead of mm/min. Change units to mm/min and you should get the correct calculation.
1 Like
I think i figured it out what ive beeing doing wrong. i have entered wrong number all the time. Check picture, i convert from i/min > mm/min > mm/sec > output in gcode is mm/min. I did mill MDF at feedrate F706.8. But should used feed rate F11880? isn’t that too fast?
Hey Patrik,
not so nice that the program lacks the units in the window.
It is plausible as the result of the calculator, but for this machine I think 10 000 mm/min (400 ipm) is rather fast (when using stepper motors).
By the way 15 000 rpm spindle speed for a two-flute bit with a 8 mm ø seems slow. Here they use 24 000 rpm all the time with two-flute 8 mm ø bits, at 5000 mm/min for the pickup pockets (in hardwood):
1 Like