Inventables Community Forum

Feed rate speed > 200%

Hi, is it possible that Easel allows the user to increment the speed over 200%?

I usually start with a very very slow speed for undetermined materials but later I need to speed up and 200% is actually 2x the initial speed only, but 10% is actually 10x less speed than the initial. Why the scale is so tilted to slower speeds?

Would not make sense to have 400% or 800% as the limit? or just call it 8x ?

1 Like

I do not use Easel, but the speed rate change values are set/fixed in grbl, not the GUI in use.

Easel offer 10-200% feed rate override.
It wont push the machine past max rapid rate (Xcarve default 8000mm/min for X&Y)

I know, I am just asking for a simple “simmetric” scale for the override. When unsure is useful to start very slow (100mm/min?) and then increase the speed, but at 100mm/min, maximum increase is to 200mm/min (2x) however you can go as low as 10 mm/min (10x less)

image

Wont that make more sense? 8 steps per side? low/high

It would be nice, but like what @JohnChamplain said, it’s a feature controlled by grbl in your arduino / processor, not in easel.

From GRBL website (https://github.com/gnea/grbl/wiki/Grbl-v1.1-Commands)

Feed Overrides

  • Immediately alters the feed override value. An active feed motion is altered within tens of milliseconds.
  • Does not alter rapid rates, which include G0, G28, and G30, or jog motions.
  • Feed override value can not be 10% or greater than 200%.
  • If feed override value does not change, the command is ignored.
  • Feed override range and increments may be changed in config.h.
  • The commands are:
    • 0x90 : Set 100% of programmed rate.
    • 0x91 : Increase 10%
    • 0x92 : Decrease 10%
    • 0x93 : Increase 1%
    • 0x94 : Decrease 1%

So you could conceivably change your the override increments yourself by changing the config.h file and re-flash your arduino.

1 Like

Looking at the config.h file it appears the max value you can increase it to is 255%. So it’s probably not worth re-flashing the arduino

// Configure rapid, feed, and spindle override settings. These values define the max and min
// allowable override values and the coarse and fine increments per command received. Please
// note the allowable values in the descriptions following each define.
#define DEFAULT_FEED_OVERRIDE 100 // 100%. Don’t change this value.
#define MAX_FEED_RATE_OVERRIDE 200 // Percent of programmed feed rate (100-255). Usually 120% or 200%
#define MIN_FEED_RATE_OVERRIDE 10 // Percent of programmed feed rate (1-100). Usually 50% or 1%
#define FEED_OVERRIDE_COARSE_INCREMENT 10 // (1-99). Usually 10%.
#define FEED_OVERRIDE_FINE_INCREMENT 1 // (1-99). Usually 1%.

1 Like

You have full control of your max speed by changing the max feed rate setting in grbl, and by increasing the feed rate value in your gcode. Generally, going faster without having first established your machine’s maximum limits can, and does, lead to lost steps and messed up carvings.

2 Likes

Oh, this is so strange. Thanks for the answer. I guess I would have to start poking at the grbl code first to get it to Easel :slight_smile:

As @JohnChamplain mentioned, you can increase your Max speed without recompiling. If you’re consistently trying to do an override of over 200%, you probably need to think about your original CAM settings a bit more.

1 Like

Sure but this is not really my point. I just start with a very low feedrate because I do not cut a lot, so I do not have the “feeling” of what is right (I guess this is a lot of Easel users).

As @EthanKinney said, there is another limitation, outside of Easel, so my request is not on the right channel. I guess if the firmware supported different feedrate overrides, Easel would had that option exposed already.


BTW, if someone else was wondering about this feature, my workaround is:

Set a higher feedrate (i.e. 50% more than what I feel comfortable), start carving. Pause carving, drop the feedrate, continue. That way I have room to dial it up and down.

Thats a good and simple approach.

BTW - the fastest way to get a starting point of feed rate is done by a calculator, all you need to know is intended RPM you\d want to use, chip thickness (provided by bit mfgr) and number of flutes of the tool.

Take a typical 1F and 2F 1/8" bit and lets assume 16k RPM and 0.001" ChipThickness (Ct): Ct = slice thickness per flute (cutter edge) per rotation

Feed rate (IPM) = RPM * Ct * Number of flutes
Feed rate for 1F = 16000 * 0.001 * 1F = 16IPM
Feed rate for 2F = 16000 * 0.001 * 2F = 32IPM

Now bump the RPM to say 24k and the math is:
Feed rate for 1F = 24000 * 0.001 * 1F = 24IPM
Feed rate for 2F = 24000 * 0.001 * 2F = 48IPM

Then a 10-200% overspeed range is for many materials a wide enough for most :slight_smile:

1 Like