Go to main site 3dtek.xyz

Correct CNC Cookbook Settings for XYZ Carve

I’m using these settings for CNC Cookbook. The spindle speeds are taken from my UGS set up and the 1 is for 1 Horsepower which I got from Amazon.com specs for the Makita (although it said 1-1/4 but don’t know what that is - 1.25 maybe?)

But what is the max feed rate? In the UGS set up file it’s 3000 for x and y but 150 for z, which I’m guessing is mm/min?

The Makita is 710W so just shy of 1 HP (735W).

Not sure what this setup file is, though 150mm sounds far too slow for the Z axis - change that to 500mm/min.

To understand where speeds are all coming from consider these notes:

  1. All speeds are in MM per Minute. Accelerations are in MM per second squared.

  2. The feed rate shown in the UGS jogging screen is only for jogging. It’s the speed at which the machine will jog when you hit the XYZ + & - buttons - unless this happens to be over the speed set in parameters $110,$111, or $112 - which are max overrides.

  3. The speed used for your cutting feed rate is specified in cam. If you look in your G-code you will see F commands in line with the movement commands. These are modal (sticky) so all movements after an F command will continue to move at this speed until a new F command is issued. Assuming again that they are not reduced by your overrides - $110,$111, or $112.

  4. The $110,$111, or $112 override speeds are also used for rapids. Rapids are movements where the spindle is in the air and moving over to start or reposition during a job. Rapids movements have no associated speed set in G-code, they are telling the machine to move as fast as it is allowed to and this is the speed set in $110,$111, or $112.

So the idea is set in $110,$111, or $112 max speed overrides as the fastest you are comfortable with the machine moving and at a speed you are sure the movements will be made correctly.
Consider also the acceleration rates at the same time $120,$121,$122. These are how quickly the machine will get up to speed. Too high acceleration rates can lead to motor stall so test any new settings before running a job and watch them for the first few jobs as the motors likeliness to stall under high acceleration or speed is increased under the load of actually cutting something
Its usually safe to run up to 10000mm/m (10 meters) in max speed for X & Y at around 200mm/s/s acceleration rate. That said, there is not much time to get your hand out of the way or hit the estop if something goes wrong at that speed.

Leave the acceleration for Z axis at 50 or so unless you are doing 3D work. For 3D Work read on otherwise skip to next paragraph of my reply. 3D Jobs can have the job times blown right out by slow acceleration or max speed rates (mostly by slow acceleration rates) and so you may want to play with finding the max reliable acceleration and speed recipe if you are doing this type of work. At this point you also need to factor in the amount of power you are supplying the Z axis and the ambient temperature. If you want max speed and acceleration you also need max current for the motors. If you find the sweet spot of max power to the motor without going into shutdown, its a good idea to step back a little to allow for a variation in ambient temperature.

Then set the Jogging speed in UGS to that which you’re comfortable moving the machine manually with the jogging buttons. Remembering that they are overridden so if you have 3000mm set as your jogging speed while moving around the X & Y axis you don’t have to reduce this value in order to hit the Z+ button because it will be reduced to 500 or less by your $112 max z speed parameter anyway.

Turn on the feed overrides (under the window menu). This allows you to increase or decrease the speed while the job is running so that you can make changes on the fly and this is super handy!
What ever speed you pick, even with the help of G Wizzard, it’s unlikely to be perfect. Both because a) its just not and b) you don’t actually have a valid spindle speed value to put into the calculator because the dial on the spindle is not an accurate assumption of speed.

So once you start the job, but a check in the feed toggle box and use the ++ & – buttons to modify your feed on the fly by 10% at a time and the + & - buttons to make smaller 1% changes. Listen to the sound of the machine and the sound of the cut. Look at the size of the chips coming off the machine as you are changing the feed rate and you will find a good speed quickly.