G2 slow feed down

[digger]

Couldn't figure out why it is happening, whenever code goes from G1 to G2 it slows down the feed rate for a bit and movement looks like hick ups. G code is generated in Fusion 360 with Mach3 post. Controller is UC100 with win7. Here is the code:
(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-3.669 Y-2.304
G43 Z0.7521 H1
Z0.2894
G1 Z0.1 F60.
G2 X-3.342 Y2.3564 Z-0.1333 I0.5368 J2.304 F100.
X-3.3198 Y2.3574 Z-0.1341 I0.0222 J-0.249
G1 X0. Z-0.25
X2.969 F120.
G2 X5.1775 Y1.1884 I0.1658 J-2.3574
X5.498 Y0. I-2.0427 J-1.1884
X2.969 Y-2.3574 I-2.3632 J0.
G1 X-3.3198
G2 X-3.342 Y-2.3564 I0. J0.25
Y2.3564 I0.2097 J2.3564
X-3.3198 Y2.3574 I0.0222 J-0.249
G1 X0.
X2.969 Z-0.3537 F100.
G2 X5.1775 Y1.1884 Z-0.4456 I0.1658 J-2.3574
X5.498 Y0. Z-0.4891 I-2.0427 J-1.1884
X5.4774 Y-0.3111 Z-0.5 I-2.3632 J0.
X2.969 Y-2.3574 I-2.3426 J0.3111 F120.
G1 X-3.3198
G2 X-3.342 Y-2.3564 I0. J0.25
Y2.3564 I0.2097 J2.3564
X-3.3198 Y2.3574 I0.0222 J-0.249
G1 X2.969
G2 X5.1775 Y1.1884 I0.1658 J-2.3574
X5.498 Y0. I-2.0427 J-1.1884
X5.4774 Y-0.3111 I-2.3632 J0.
X2.969 Y-2.3574 Z-0.6245 I-2.3426 J0.3111 F100.
G1 X2.42 Z-0.6437
X-3.3198 F120.
G2 X-3.342 Y-2.3564 I0. J0.25
Y2.3564 I0.2097 J2.3564
X-3.3198 Y2.3574 I0.0222 J-0.249
G1 X2.969
G2 X5.1775 Y1.1884 I0.1658 J-2.3574
X5.498 Y0. I-2.0427 J-1.1884
X2.969 Y-2.3574 I-2.3632 J0.
G1 X2.42
X-1.6951 Z-0.7874 F100.
X-3.3198 F120.
G2 X-3.342 Y-2.3564 I0. J0.25
Y2.3564 I0.2097 J2.3564
X-3.3198 Y2.3574 I0.0222 J-0.249
G1 X2.969
G2 X5.1775 Y1.1884 I0.1658 J-2.3574
X5.498 Y0. I-2.0427 J-1.1884
X2.969 Y-2.3574 I-2.3632 J0.
G1 X-1.6951
G0 Z0.7521

M30


Thanks,
Milosh

[cncdrive]

It is because at some points you have miniature arcs after the main arcs.
And at other points you changing the Z height and the direction vector changes and so the software must use some decceleration to change that, because direction vector change requires different axes speeds, it can't be done without decceleration.
You can try to improve your code and also you can try to increase the acceleration parameter of the axes if possible so the axes can change speed faster and so the decceleration will be then smaller.
And you can try to adjust the tolerances, but that might not be a good solution depending on what are the tolerance requirements for the job.

[digger]

Thanks for response.
Small arcs you are talking about are from the model. Arcs are not tangent to the straight curves and that is the reason why are there. I modified same model and made right arc tangent to the straight lines, and I got one G2, while other side still has three G2 lines. While cutting this there is no change in Z direction. Later today I will try with increasing the acceleration. Still don't understand why there is a change in speed. Please, I do not blame anybody or anything. Just want to understand why is this happening and how to prevent it. That is all.

Thanks,
Milosh

[cncdrive]

Code: Select all

G2 X5.1775 Y1.1884 I0.1658 J-2.3574
X5.498 Y0. I-2.0427 J-1.1884
X5.4774 Y-0.3111 I-2.3632 J0.
X2.969 Y-2.3574 Z-0.6245 I-2.3426 J0.3111 F100.
G1 X2.42 Z-0.6437

You said there is no Z change, but there is.
Look at the above code.
Z is -0.6245 at the last arc (G2) and in the next linear interpolation (G1) line it is -0.6437.
So, the Z moves level and so the direction vector is changing.

[Robertspark]

What is your "Corners error max" and "Linear error max" parameters set to?

Configuration >> General Settings tab?

[digger]

I think I figured it out why it is happening. My programming for speed for different motion is causing this. For cutting I use 120 ipm, for ramping 100 imp and for plunge 60. Later today I can check if it is happening if I change ramping to have same feed as cutting.

Robert, it is set to 0.001". Behave doesn't change regardless of the value.

Milosh

[Robertspark]

What are you machining? (wood, aluminium, steel?)

For what application / industry?

Trying to get an idea of what precision you require

by setting the corner error max to 0.001 " (1 thou) that will require your machine to slow down in order to make sure it does not exceed 1 thou in the corners...

Look at example 1 here:
https://www.khanacademy.org/science/phy ... celeration

plug in your acceleration and your corner radius (0.001) and it will tell you how low your feedrate must slow down in transitions between junctions to achieve your 1 thou precision.

[Robertspark]

If you are using roughing and finishing cuts you could use different linear and corner error max settings.

This may actually speed up your cut time given you are running course settings for the rough cut and fine settings for finishing cut profile.

(It may be worthwhile cncdrive considering if such an inbuilt feature may be beneficial)

[cncdrive]

Rob,

The G64 has all the tolerance parameters.
You can code G64 with it's parameters to change tolerance parameters.
There is no need to go into setup to make the change, the G64 code can do the same from g-code file or from MDI.

[Robertspark]

Ahhh. Thanks... I learnt something...

I knew what g64 was, never changed it to exact stop and have never used the g64 settings before...

Time for play required