G2 slow feed down

[digger]

Well, I appreciate all answeres, but have to admit that it is not what I tough it is. I changed and made equal cutting, ramping and plunging speed, and run the file. On the machine, as well as on the run screen I can see the changes in speed like hick ups. And they are happening only where is the transition from linear interpolation to circular. Here is the video of this:

https://youtu.be/jQ_CSWQ3ZrM

Look at 10sec, and 22sec. All those moves are on the same Z level. Corner and linear error (on video clip) are set to 0.01". Maybe it is to much for wood, but haven't noticed any difference in movement when set up to 0.1". As I said, I cut wood using Mechmate.

Here is the code from the video.

(1001)
(T1 D=0.5 CR=0. - ZMIN=-0.7874 - FLAT END MILL)
G90 G94 G91.1 G40 G49 G17
G20

(2D CONTOUR2)
M5
M9
T1 M6
S15000 M3
G54
G0 X-3.26 Y2.3622
G43 Z0.6 H1
Z0.2894
G1 Z-0.25 F150.
G2 X-3.238 Y2.3632 I0.022 J-0.249
G1 X3.0594
G2 Y-2.3632 I0. J-2.3632
G1 X-3.2385
G2 X-3.2606 Y-2.3622 I0. J0.25
X-3.26 Y2.3622 I0.2094 J2.3622
G1 Z-0.5
G2 X-3.238 Y2.3632 I0.022 J-0.249
G1 X3.0594
G2 Y-2.3632 I0. J-2.3632
G1 X-3.2385
G2 X-3.2606 Y-2.3622 I0. J0.25
X-3.26 Y2.3622 I0.2094 J2.3622
G1 Z-0.6437
G2 X-3.238 Y2.3632 I0.022 J-0.249
G1 X3.0594
G2 Y-2.3632 I0. J-2.3632
G1 X-3.2385
G2 X-3.2606 Y-2.3622 I0. J0.25
X-3.26 Y2.3622 I0.2094 J2.3622
G1 Z-0.7874
G2 X-3.238 Y2.3632 I0.022 J-0.249
G1 X3.0594
G2 Y-2.3632 I0. J-2.3632
G1 X-3.2385
G2 X-3.2606 Y-2.3622 I0. J0.25
X-3.26 Y2.3622 I0.2094 J2.3622
G0 Z0.6

M30

[ger21]

What are your other CV settings?
Stop Angle Degrees?
Linear Unify Max?
Linear Addition Length Max?

And what are your X and Y acceleration?

[digger]

Hi Ger,

Acceleration is set to 12.5. Max Linear Addition Length is 1 and Maximum linear Unify Length is 2. Exact stop at 89.

To be honest, I am not sure what values should be ok for max linear addition and unify length.

[ger21]

12.5 accel is very low? Have you tried increasing it? That'll make the biggest difference. Or change the model to have a tangent transition from straight to arc.

Question for CNC Drive.
With code like this, increasing the tolerance settings don't seem to smooth out the motion, as it still wants to slow down at the transitions.

When you start on the new S-Curve planner, can you look into a better method of blending moves, to eliminate issues like this. Other controls do a better job of blending non tangent moves together, smoothing out the motion, at the expense of precision.

[cncdrive]

Gerry,

There are things which can and which can't be elliminated. The limit is the earth physics and settings.
But we will put the motion planner on different basics than it is now to make it simpler for ourselves to follow and to make it more flexible and as good as possible.
To achive this we will use the things we have learnt so far from the long development cycle.

And you are right, that some controls handle these things differently, but I wouldn't say they handle it better.
Taking mach3 as an example it resolves this kind of issue with cutting a part of the path off and you can only guess about how much it will cut off.
I would not call it "better".

[ger21]

Taking mach3 as an example it resolves this kind of issue with cutting a part of the path off and you can only guess about how much it will cut off.
I would not call it "better".

Actually, in some cases it may be better. I would expect by increasing the error tolerance in UCCNC, it would do the same thing, but it does not appear to, at least in this case.

In some cases, adding the option to "blend" moves together can greatly decrease cut times, and improve the finish. Of course, this is at the expense of being slightly less precise.

I understand that it's more accurate the way it is, but adding the option for more blending may be beneficial, especially with lower powered machines with lower acceleration settings.

[Derek]

It doesn't matter what I set tolerances to on any of my 4 machines. There are always slowdowns between segments. As has been said I believe this is due to low acceleration because like a lot of machines they are under built and or under powered. On the majority of my projects I would sacrifice accuracy for smooth motion. If I turn the acceleration up on my routers I go from slowdowns to bangs and shakes.

I'm really hoping the S planer alleviates this because the slowing at each segment adds a ton of time to a project that has 200,000 lines of code or more not to mention changes the chip load.

[Robertspark]

At a F150 "/min and an acceleration of 12.5 "/s/s

It accelerates from 0 to the specified feedrate in ~0.2 sec (and deceleration takes the same amount of time).

I think the problem occurs when you have a G02 leading to a G02. {it may also occur with a G02 > G03 / G03 >G03 / G03 >G02 but you've not got any of those}

eg from the code below:

Code: Select all

G1 X-3.2385
G2 X-3.2606 Y-2.3622 I0. J0.25
X-3.26 Y2.3622 I0.2094 J2.3622
G1 Z-0.5

Being a layman..... I think maybe the problem is the motion planner at the end of one arc does not know the direction that the next arc is going to shoot off in (bear with me.... as I know that the terminology is not correct....)

Before shooting the messenger, spare a moment of thought...

If I send you in a straight line and then an arc, given you know the angle of intercept between the arc and the line (tangent) you can slow down accordingly allowing for following the corner error max between the two rigid moves.

With two arcs.... you'll have a problem to estimate the coincident angle especially if the arcs are are different sizes or directions, because you now have to add in a third minor arc which is the corner error max, and it should be applied to the junctions between the arcs {is this how it works cncdrive? does the corner error max get applied to juctions between arcs or is it just from linear to linear and linear to arc motion?}

(just my 2 pence assessment ..... remember I know nothing! But always trying to learn and understand)

Another thought....

To me you look to being a little harsh on your endmill.

I mean consider this line of code extracted from the below:

Code: Select all

G2 X-3.2606 Y-2.3622 I0. J0.25
X-3.26 Y2.3622 I0.2094 J2.3622
G1 Z-0.7874
G2 X-3.238 Y2.3632 I0.022 J-0.249

The cutter has to finish the double arcs, then drops / cuts into the material and then goes off for another arc

Is your post processor not able to provide you with a leadin?

I've not done any wood milling but I know with aluminium I've got to be gentle when feeding into the material or I end up chipping the end of the end mill. They like milling but not drilling. II know it depends on the end mill, but it may also help your transition.

What size cutter are you using?

[ger21]

When just running in demo mode, with accel set to 12.5 for all axis, it slows down at the transitions from straight to arc, and no amount of error tolerance will keep it from slowing down.

[Robertspark]

Thats strange , I would have thought that the a larger corner error max would have minimised the the effect

What version UCCNC are we all using?

using the feedrate and acceleration listed earlier in posts (F150 a12.5)

The minumum radius size (corner error max) that should lead to no deceleration is 0.5

(V/60)^2 / acc = (150/60)^2 / 12.5 = 0.5

hence if you set it the corner error max like earlier in the posts at 0.001, the velocity HAS to slow to 6.7 units / min

(SQ RT ( r x acc )) = (SQ RT (0.001 x 0.5 )) x 60 = 6.7

https://www.khanacademy.org/science/phy ... celeration

physics, no choice.

to decelerate from 150 units / min to 6.7 units / min will take ~0.191 sec, hence to slow down and speed back up at the junction will take ~0.4 sec

How big is the tool you are using?

If the cutter is 1/4" dia say..... why use 0.001" corner error max ..... suggest use something a little less than 1/2 the tool diameter (1/8")

that way the machine will only low to 75 units per min (1/2 feedrate) , and the deceleration will only take 0.1 sec, so the total move (decelerate + accelerate at the junctions will be 0.2 sec (half the time).