Slow operation

Feed speed is the max. speed for basic movements available in g-code (linear, circular ..). It is divided into 3 phases: acceleration, constant speed and deceleration. But if you have a 3D contour, you have lots of small movements with lots of direction changes in X, Y and Z. The machine can't accelerate to the full speed within such small distances.

Maybe you can tweak acceleration settings just a bit to make it a little bit faster, but be aware that settings which are too aggressive mean loosing steps.

Thank You

Your words make sense.

But my contour is rather simple. In the top it is a 80mm squire, which transits to 150mm circle at the bottom. total height is 55mm
So the last steps contours are the simple circle with no fast direction changes at all. And it is slow.

I am making a bowl. i do a fast adaptive cleaning first which goes almost the same contour and goes fast fast. Then the contour with "rest mashening"

Also when i manufacture the inside of the bowl i have the same shape. A 130mm circle transiting into 60mm squere in 40mm. For that i use 3D pocket. and it is going fast in fast cleaning and also in the finishing "rest mashening" path with same 0.2 and 0.2mm step over/down.

So having this slow outside contour is a bit strange. Fusion360 simulation says 1:40. In reality it took 5 hours..:((

whwere should i tweek accelerationsettings? Fusion 360 or UCCNS?

Thank You

Thank You

Your words make sense.

But my contour is rather simple. In the top it is a 80mm squire, which transits to D155mm circle at the bottom. total height is 55mm
So the last steps contours are the simple circle with no fast direction changes at all. And it is slow. and the distances are not so small..

I am making a bowl. i do a fast adaptive cleaning first which goes almost the same contour and goes fast fast. Then the contour with "rest mashening"

Also when i manufacture the inside of the bowl i have the same shape. A 130mm circle transiting into 60mm squere in 40mm. For that i use 3D pocket. and it is going fast in fast cleaning and also in the finishing "rest mashening" path with same 0.2 and 0.2mm step over/down.

So having this slow outside contour is a bit strange. Fusion360 simulation says 1:40. In reality it took 5 hours..:((

whwere should i tweek accelerationsettings? Fusion 360 or UCCNS?

Thank You

Hard to say what exactly goes wrong without having a look into the file.

In the cleaning run, the acceptable deviation is much bigger, which gives the program that produces the g-code much more flexibility. So, it can optimize the g-code for example to have lines as long as possible.
The finish on the other hand has to be precise. Some CNC controllers don't allow to have more sophisticated g-code like arcs, which results in dividing each and every little rounding into pretty small lines. I don't know more details about UCCNC and it's controller. Maybe you simply use the wrong post-processor in Fusion, which does not produce g-code optimized for UCCNC?

Fusion shows you an estimation of the runtime and part of the g-code is the speed, so Fusion at least has some speed settings. If it does not have acceleration settings an estimate of course is not precise.

But I think UCCNC also needs to have max. speed and acceleration settings, as it has to operate the machine within it's limits. If g-code says "use speed x" which is to fast for the machine, the controller should use the max. speed allowed by the machine.

So, do these settings match?

Thank You.

You have helped me a lot.
I sure use the right postprocessor.
I attach the files.

I think it is because of the tolerences then.

So Fusion360 gives 0.1 by defoult for 3D pockets and 0.01 for 3D contours.
I was not paying attention to tollerance setting before, leftthe defoults (i am very new CNC operator and manly google educated)

In fact i do not need such a great tolerence. 0.5 will be fine in this case.
I will test it tomorrow... Thank You.

Another question also. D600 has a maximum XY speed set to 3000 in UCCNC.
Is it safe for me to increase this limit?
Or is it specific to this machine, and i should not increase it more?

Also there is a thausand other questions for UCCNC. but maybe i should ask in different topics...
Thank You...

Thank You.

You have helped me a lot.
I sure use the right postprocessor.
I attach the files.

I think it is because of the tolerences then.

So Fusion360 gives 0.1 by defoult for 3D pockets and 0.01 for 3D contours.
I was not paying attention to tollerance setting before, leftthe defoults (i am very new CNC operator and manly google educated)

In fact i do not need such a great tolerence. 0.5 will be fine in this case.
I will test it tomorrow... Thank You.

Another question also. D600 has a maximum XY speed set to 3000 in UCCNC.
Is it safe for me to increase this limit?
Or is it specific to this machine, and i should not increase it more?

Also there is a thausand other questions for UCCNC. but maybe i should ask in different topics...
Thank You...

Well, the maximum speed settings are on the safe side. It is a setting which will work for most SC machines of the same version. The real max. speed for your machine you have to figure out yourself. The factors that have an influence on the real max. speed are manifold ... tolerances of the stepper drivers and their currency settings, step-mode set for the drivers in regards to micro-steps and max. frequency of the controller board, mechanical tolerances of the stepper motors and the quality of the build which has an impact on how easy it is to move the axes .....
Most of those factors are pretty close together or equal for most of the same kind of machines. Biggest effect is the mechanical quality of the build. So, in some rare cases the standard settings are too fast already, but for most builds there is some room to increase the max. speed.
Testing the limit is pretty easy. Change the settings, let the machine run a simple test-job, which produces a small level of stress.
Stress means hardness of the material and size of the tool.
After running the job, check weather the machine lost steps. If so, decrease the max. speed or go back to the last good run, if not increase the speed. I would start to increase by ~10% and for each following test increase or decrease by half the difference of the previous run.

Later on for concrete jobs you would change the speed settings that are tied to the different tools. Makes sense to have a tool list for different materials as well.