[jcarpenter2]

Used bobcad-cam to create an embossed image, ran the toolpath and posted it. UCCNC does not recognize any of the K arcs. Does the K arc not work with the Z-axis in UCCNC?

[BanduraMaker]

UCCNC only supports G17. G18 and G19 are not supported. And better yet, when it comes across a G18 or G19, it does a G17 move! It would be really nice if it threw up a warning when it was loading the code that G18's or 19's are present. I've ruined a couple of expensive workpieces when my CAM software inserted a G18 or G19 in there.

[vmax549]

The newest not released yet version DOES alert you to ANY gcode that UCCNC does not understand or support and gives you several options.

(;-) TP

[jcarpenter2]

So im under the impression that UCCNC is incompatible with the slice planar inside bobcad-cam.

[dertsap]

Uc is incapable of doing any z arc code but not totally incompatible with slice planer
if you uncheck arc fit for slice planer then bobcad will put out short line segments rather than arcs . Not efficient but it's an option

[jcarpenter2]

Well it added 1300 new lines. Ill see how it runs.

[dertsap]

Well it added 1300 new lines..

You got off easy . Be sure to keep the tolerance setting in bcad tight , otherwise the planer cuts could end up looking like crap if your metal machining

[Jon.N.CNC]

Sorry digressing slightly, can anyone tell me why I find small ijk arcs uccnc cuts nice and smooth but I cut a large 1200x2400mm oval and it was jerking badly.

The control pc is a quad core and fairly fast. If it wasn't up to it I'd be surprised.

[OlfCNC]

An oval is not an arc. An oval can be made from small lines only and how smooth and precise that will be cut depends on your trajectory settings.

[BanduraMaker]

Sorry digressing slightly, can anyone tell me why I find small ijk arcs uccnc cuts nice and smooth but I cut a large 1200x2400mm oval and it was jerking badly.

The control pc is a quad core and fairly fast. If it wasn't up to it I'd be surprised.

It's probably your CV settings. Does your maximum error and corner tolerance match? I've found that if they don't match you get jerky motion.

[dertsap]

Sorry digressing slightly, can anyone tell me why I find small ijk arcs uccnc cuts nice and smooth but I cut a large 1200x2400mm oval and it was jerking badly.

.

your code shouldnt have k arcs because they are unsupported , which is why you need to uncheck arc fit in bobcad

[Jon.N.CNC]

Sorry Is js g17 arcs. I'll have to double check but I'm almost certain the oval was made up of arcs. Will look into cv rate etc thanks

Edit..Just checked the gcode was made up of

G1 X + y
G2 X + y + I + j

Is this ok with ucnc? The oval was correct just jerky. Should the i + j arcs not been in there?

Linear error max & corner error max both 0.03 :s

[vmax549]

How much video memory do you have ? Is it an integrated video ?? The older screens that ran from Flash can be a memory hog and can cause problems . That is all fixed in the newest version as well. They optimized it to run across a very wide platform of PCs and video setups.

By teh way 1-2gb video cards are CHEAP today $30-40 and they can make a world of difference.

Just a thought, (;-) TP

[Jon.N.CNC]

How much video memory do you have ? Is it an integrated video ?? The older screens that ran from Flash can be a memory hog and can cause problems . That is all fixed in the newest version as well. They optimized it to run across a very wide platform of PCs and video setups.

By teh way 1-2gb video cards are CHEAP today $30-40 and they can make a world of difference.

Just a thought, (;-) TP

Yeah just integrated dell Inspiron laptop graphics. I'm surprised graphics has much to do with when the dro's keep up with the code.

[jcarpenter2]

Well it looked like crap. Went back to bobcad-cam, used a smaller bit, tightened the tolerance considerably and ran it again. When I posted that file in bobcad-cam, the line count went up considerably. Ran the new code for 3.5 hours on my machine and it still looked like crap. I have watched hours and hours of bobcad-cam videos, hours of gcode videos, hours of reading threads here and on a few other forums, and yet I feel like im barely scratching the surface of cnc. It doesn't help that many of the hours ive spent researching and learning that I have to filter out the crap people post, and then there is frustrating situations like uccnc not using "k" arcs. Or Bobcad videos that show how easy something is and then come to find out that "oh, you only have the standard bobart and not the professional so you cant do that either". Yadda, yadda, yadda.

End of small insignificant rant

[vmax549]

Welcome to the world of DIY CNC. CNC is not an instant oatmeal function . It has a steep learning curve in 4-5 different areas ALL at teh same time.

But many have master it and so can you.

(;-) TP

[vmax549]

NOW when you say it looked like crap what exactly does that mean ??? Also Bobcad is known for poor quality post . What post were you using as I dought there was a UCCNC post in Bobcad. Did the post turn ON CV in Gcode or maybe it turned it OFF ??

[jcarpenter2]

Here is what i mean.
Pic1 is the dxf
Pic2 is the emboss
Pic3 is what it looked like. I ran it in two segmants, the first was with an 1/8 bullnose for the roughcut. The second run was with a 1/16th bit with much tighter tolerances.
Here is a brief view of the code using mach3 post processor.
(BEGIN PREDATOR NC HEADER)
(MACH_FILE=HAAS - 3XVMILL.MCH)
(MTOOL T1 S1 D.0625 H2. A0. C0. DIAM_OFFSET 1 = .0313)
(SBOX X0. Y-4.2498 Z-1. L7.248 W4.2515 H1.)
(END PREDATOR NC HEADER)

%
O100
(PROGRAM NUMBER)
(PROGRAM NAME - GONE FISHING.NC)
(POST - MACH 3 MILL NO ATC)
(DATE - SUN. 02/07/2016)
(TIME - 05:43PM)

N01 G20 G40 G49 G54 G80 G90 G91.1
;N02 G53 Z0.

(JOB 1 SLICE CUT PLANAR)
(FEATURE SLICE PLANAR)

;N03 T1 M6
N04 S1252 M03
N05 G00 G90 G54 X0. Y.0018
;N06 G43 H1 Z.3
N07 G01 Z0. F2.023
N08 X7.248 F19.5447
N09 Y-.008
N10 X0.
N11 Y-.018
N12 X7.248
N13 Y-.028
N14 X0.
N33 X3.1137 Z-.0062
N34 X3.1144
N35 X3.1171 Z-.0087
N36 X3.1655 Z-.0175
N114623 X0.
N114624 Y-4.178
N114625 X7.248
N114626 Y-4.188
N114627 X0.
N114628 Y-4.198
N114639 X0.
N114640 Y-4.2498
N114641 X7.248
N114642 G00 Z.3
N114643 M05
;N114644 G53 Z0.
;N114645 G53 Y0.

(END OF PROGRAM)

N114646 M30
%

[Jon.N.CNC]

Here is what i mean.
Pic1 is the dxf
Pic2 is the emboss
Pic3 is what it looked like. I ran it in two segmants, the first was with an 1/8 bullnose for the roughcut. The second run was with a 1/16th bit with much tighter tolerances.
Here is a brief view of the code using mach3 post processor.
(BEGIN PREDATOR NC HEADER)
(MACH_FILE=HAAS - 3XVMILL.MCH)
(MTOOL T1 S1 D.0625 H2. A0. C0. DIAM_OFFSET 1 = .0313)
(SBOX X0. Y-4.2498 Z-1. L7.248 W4.2515 H1.)
(END PREDATOR NC HEADER)

%
O100
(PROGRAM NUMBER)
(PROGRAM NAME - GONE FISHING.NC)
(POST - MACH 3 MILL NO ATC)
(DATE - SUN. 02/07/2016)
(TIME - 05:43PM)

N01 G20 G40 G49 G54 G80 G90 G91.1
;N02 G53 Z0.

(JOB 1 SLICE CUT PLANAR)
(FEATURE SLICE PLANAR)

;N03 T1 M6
N04 S1252 M03
N05 G00 G90 G54 X0. Y.0018
;N06 G43 H1 Z.3
N07 G01 Z0. F2.023
N08 X7.248 F19.5447
N09 Y-.008
N10 X0.
N11 Y-.018
N12 X7.248
N13 Y-.028
N14 X0.
N33 X3.1137 Z-.0062
N34 X3.1144
N35 X3.1171 Z-.0087
N36 X3.1655 Z-.0175
N114623 X0.
N114624 Y-4.178
N114625 X7.248
N114626 Y-4.188
N114627 X0.
N114628 Y-4.198
N114639 X0.
N114640 Y-4.2498
N114641 X7.248
N114642 G00 Z.3
N114643 M05
;N114644 G53 Z0.
;N114645 G53 Y0.

(END OF PROGRAM)

N114646 M30
%

Not really enough code there to say what's going on. Do you have g17 I J arcs allowed?

[jcarpenter2]

Theres a 115,000 lines, so i got rid of all the stuff in the middle (nothing but x, y, z movements). No arcs, because bobcad-cam used g18 codes and tried to use the k code arc which i found out uccnc does not recognize. Hence i ran bobcad-cam without the arc fit and as you see with the picture, that is what was produced. Now i must say, maybe there is some user error since i am still new to all this.