forum.cncdrive.com

It is normal that this code smashes into touch probe with rapid feed?

G1 G94
G31 A90 F90

A axis is rotary (deg/min)

Hi Doncis,

In the manual for UCCNC, it explains that an axis set to 'rotary' doesn't respect feedrate commands, it follows the other linear axes and is only limited by max velocity. Just uncheck 'axis is rotary' box for that axis, but you can leave 'roll over on 360'. It still behaves like a proper rotary, but now will obey feedrates (deg/min).

When I was adding rotary probing to ProbeIt, took me a little bit of trial error to figure it out also. I put the following in my manual for ProbeIt: NOTE: It is recommended that you have "axis is rotary‟ unchecked in UCCNC, having "roll over on 360‟ is fine. The rotary axis will not respect feed rate commands if "axis is rotary‟ is set, and also you may have issues with direction of rotation as UCCNC always tries to make the shortest distance move when set to rotary.

regards,
Eric

Thanks, I will check later.
I assume that it exclude feed rate only for display purposes. Imagine you want to cut simple slot only with A axis, with set G1 deg/min feed rate, and boom crash with rapid feed..it should always respect G1..
btw I always use G93 for 4axis.

Doncis wrote:Thanks, I will check later.
I assume that it exclude feed rate only for display purposes. Imagine you want to cut simple slot only with A axis, with set G1 deg/min feed rate, and boom crash with rapid feed..it should always respect G1..
btw I always use G93 for 4axis.

I side with Donics on this.
A feedrate command invoked on a single axis, no matter what X,Y,Z,A,B,C it should be respected and executed, in multi axis moves, whatever the program does, also tricks like not make it a rotary but rollover it a rotary then it obeys:
Common you guys: it is a rotary. Sounds the same as: tell it is a circle then the square can roll.

For the record, i just finished my upgrade 4th to 5th axis, this was the first thing i found, (not respecting F commands). I'm still shocked i geuss and find this disturbing and an error programmed into UCCNC.
Same as G53 is not a real work space (but that's off topic)
Choose UCCNC for this over mach 3 because of the windows timer clock, as my current controller only does 4 axis.

Please can somebody tell me if a Gcode on UCCNC is run and the CAM is instructing this code for example:
G0 X0. Y0. Z0. A90 B0.
G1 Z-1.0 F150
G01 B45 F100

It will crash my endmill trying to goto C45 with 6000 units/minute (max velocity as per setup) every time. NOT GOOD!.

So basically telling the software that it is NOT a rotary axis causes it to work correctly.

I know this because I just did it on my system. I have wasted 2 1/2 days and $400 trying to figure this out.

This is inexcusable, it is now 2024 and this BUG has not been corrected.

I get the frustrations (I started a thread on this 3 weeks ago) but I don't think it's reasonable to expect:

Code: Select all

G1 Fx

to work correctly on a rotary axis. Unless you have somehow defined the radius of the material, there is no way to determine the actual distance over material the tool has travelled. And as best I can tell, there is no G-Code for defining the radius of a part in a rotary axis.

Thus, rotary feedrates really have to be controlled with G93. Unfortunately, that IS a bug right now, but I don't think it's reasonable to expect

Code: Select all

G94 G1 Fx

to work with rotary moves.

Uncheck rotary axis in axis setup. For simultaneous 4axis milling use G93, and feed rate F MUST be defined in every row.