[jcarpenter2]

According to everything i read you need to use a MACH3 post with UCCNC. I have ran multiple post and Mach3 has done the best, however, there are still issues when bobcad-cam creates a toolpath and then is interpreted by UCCNC. Here is the latest file i have created and of course its NOT being read by UCCNC how i am expecting it to. The code looks clean, however, there are specific areas that UCCNC is ignoring causing a destroyed project. See Image. It ran fine through the vcarve, but when it started to do the z-rough it cut right through the project (currently yellow in the screenshot as it is on the trajectory of the blue line before it completed that portion of the code). There is one remaining blue line on the screen shot which is where it will plow through the project when it gets ready to do the z-finish. So, why did UCCNC not read the N54682 line coordinates? Why did UCCNC not lift the Z to .1 on line N54684?

[ger21]

When you try to load code that is not compatible with the control, it's not the control's fault.
You need to make sure that your BobCAD code is compatible with UCCNC.

[BanduraMaker]

Modify your post to put any G0 or G1 (and probably G2&G3) moves on a new line and it should fix it. e.g.:

G90 G54
X4.5 Y-2.4
G43 H2
G00 Z.12
M08

Should work fine.

[jcarpenter2]

Tell me how/why a G90 G54 is not compatible with UCCNC. Tell me how/why a G43 H2 is not compatible with UCCNC. Obviously building software like UCCNC is way above me, however, G90, G54, G43 codes are universal codes, so what is the problem.

[BanduraMaker]

They are compatible. Apparently UCCNC just doesn't like coordinated moves on the same line as modal commands or something like that.

Lookit here:

Attachment 310938

In the top version, the coordinated moves are ignored, in the bottom version, they work fine.

[jcarpenter2]

Great bit of info BanduraMaker. Thank you for identifying that, but how do i correct it? Yes i see how i can correct that in my post from your previous reply, but how i do i correct this within the post processor instead of every file i create? Or is that a question for a different forum?

[BanduraMaker]

I don't own bobcad so I don't know the specifics for how to do it in that but, bobcad should have some sort of post processor editor in there. What you need to do is find the sections for G0~G3 and have bobcad always output those on a new line. In my first post I wrote "modify your post"...what I really meant and should have written was "modify your post processor to output those commands on a new line".

If you can't figure it out yourself, someone at bobcad should be able to answer how to do it in 30sec. Send them an e-mail with the screenshot I provided telling them what you want to do and it should be really quick to fix.

[mactec54]

I don't own bobcad so I don't know the specifics for how to do it in that but, bobcad should have some sort of post processor editor in there. What you need to do is find the sections for G0~G3 and have bobcad always output those on a new line. In my first post I wrote "modify your post"...what I really meant and should have written was "modify your post processor to output those commands on a new line".

If you can't figure it out yourself, someone at bobcad should be able to answer how to do it in 30sec. Send them an e-mail with the screenshot I provided telling them what you want to do and it should be really quick to fix.

Each piece/line of code that is Modal, should stay in effect until it is changed or given a different action, there is a problem in the control if this is not happening, this is not a postprocessor problem

When you call a G0 it will stay a G0 until it is changed, the same for G1 G2 G3 and others there are lots of code that is Modal M codes as well, there is no need to have a G-code entry, on every line if the Control is working correct, this is in the control that has not been programed correct, to the RS 274 standard G-code Format

Doing a work around to make this work, is not helping to make this control better, this is a must fix and should be a priority for UNCNC to get this fixed

[mactec54]

Tell me how/why a G90 G54 is not compatible with UCCNC. Tell me how/why a G43 H2 is not compatible with UCCNC. Obviously building software like UCCNC is way above me, however, G90, G54, G43 codes are universal codes, so what is the problem.

G54 In lots of controls should be on a line by itself, G90 is fine with the start of most operations, but if it is in the safety line it is not needed in your program
G90 G1 X---Y---, this is normal

Safety line normally have G17 G40 G80 and can have G90 Having the G90 in the safety line you would then not need it in your program unless you used a G91 somewhere & then you would need to add a G90 to cancel the G91

As we can't see the start of your program this can play a big part on what action is going to happen

[jcarpenter2]

Here is the actual code with all the irrelevant stuff removed. There are actually three areas that were not read by the UCCNC. N05, N06, N54682, N54683, N59740, N59740. Each of those areas go back to what has been discussed in this thread. However if there appears to be another reason than already discussed this may help to identify any other issue causing UCCNC not reading it. I did notice in job4 that the G90, G54, and the G43 where not used. With job4 i did not change out the tool, i just changed the depth of the start point.

(BEGIN PREDATOR NC HEADER)
(MACH_FILE=HAAS - 3XVMILL.MCH)
(MTOOL T1 S7 D.5625 H2.25 A60. C0. DIAM_OFFSET 1 = .2813)
(MTOOL T2 S2 D.25 H2.5 A0. C.125 DIAM_OFFSET 2 = .125)
(MTOOL T3 S2 D.125 H2. A0. C.0625 DIAM_OFFSET 3 = .0625)
(SBOX X0. Y-7.75 Z-.75 L6.25 W7.75 H.75)
(END PREDATOR NC HEADER)

%
O100
(PROGRAM NUMBER)
(PROGRAM NAME - BORDER AND CROSS.NC)
(POST - MACH 3 MILL NO ATC)
(DATE - SAT. 03/05/2016)
(TIME - 08:05AM)
N01 G20 G40 G49 G54 G80 G90 G91.1
N02 G53 Z0.
(JOB 1 V-CARVING)
(FEATURE V-CARVE)
N03 T1 M6
N04 S1113 M03
N05 G00 G90 G54 X2.3612 Y-6.2963
N06 G43 H1 Z.1
N07 G01 Z-.0552 F20.
N08 X2.36 Y-6.2974 Z-.0531 F24.
N54674 X4.4949 Y-3.2581 Z0.
N54675 G00 Z.1
N54676 M05
N54677 G53 Z0.
N54678 G53 X0. Y0.
N54679 M00
(JOB 2 ZLEVEL ROUGH)
(FEATURE Z-LEVEL ROUGH)
N54680 T2 M6
N54681 S5011 M03
N54682 G90 G54 X4.6743 Y-2.4774
N54683 G43 H2 Z.1 M08
N54684 G00 Z.12
N54685 G01 Z-.0302 F40.
N54686 X4.6761 Y-2.4821
N59729 X3.1597 Y-1.1017
N59730 X3.1253
N59731 G00 Z.12
N59732 Z.1
N59733 M09
N59734 M05
N59735 G53 Z0.
N59736 G53 X0. Y0.
N59737 M00
(JOB 3 ZLEVEL FINISH)
(FEATURE Z-LEVEL UPPER FINISH)
N59738 T3 M6
N59739 S10000 M03
N59740 G90 G54 X4.5853 Y-2.9421
N59741 G43 H3 Z.1
N59742 G01 Z-.0002 F40.
N59743 Y-3.3424 F48.
N59744 X4.5849 Y-3.3455
N141930 X1.889 Y-2.001
N141931 X1.8793 Y-2.0008
N141932 X1.8683 Y-2.0167
N141933 G00 Z.1
(JOB 4 ZLEVEL FINISH)
(FEATURE Z-LEVEL FINISH)
N141934 S10000
N141935 X1.6427 Y-2.3614
N141936 G01 Z-.3002 F40.
N194186 X2.4956 Y-1.563
N194187 X2.4831 Y-1.5693
N194188 G00 Z.1
N194189 M05
N194190 G53 Z0.
N194191 G53 X0 Y0.

(END OF PROGRAM)

N194192 M30
%

[mactec54]

[QUOTE=jcarpenter2;1846244]Here is the actual code with all the irrelevant stuff removed. There are actually three areas that were not read by the UCCNC. N05, N06, N54682, N54683, N59740, N59740. Each of those areas go back to what has been discussed in this thread. However if there appears to be another reason than already discussed this may help to identify any other issue causing UCCNC not reading it. I did notice in job4 that the G90, G54, and the G43 where not used. With job4 i did not change out the tool, i just changed the depth of the start point.[QUOTE]

Try this you have to make changes to your post processor to correct these lines of code, they are not correct
%
O100
N01 G20 G40 G49 G80 G90 G91.1 ( Removed the G54 this is no place for it)
N02 G0 Z0. (Removed the G53 some controls will not run this )
G54 ( Can be anywhere but on a line by it's self )
N03 T1 M6
N04 S1113 M03
N05 G00 G90 X2.3612 Y-6.2963 (Removed the G54 from this line )
N06 G43 H1 Z.1
N07 G01 Z-.0552 F20.
N08 X2.36 Y-6.2974 Z-.0531 F24.
N54674 X4.4949 Y-3.2581 Z0.
N54675 G00 Z.1
N54676 M05
N54677 G53 Z0.
N54678 G53 X0. Y0.
N54679 M00
(JOB 2 ZLEVEL ROUGH)
(FEATURE Z-LEVEL ROUGH)
N54680 T2 M6
G54
N54681 S5011 M03
N54682 G90 X4.6743 Y-2.4774 (You have no action in this line you would need a G0 or a G1 Etc )
N54683 G43 H2 Z.1 M08
N54684 G00 Z.12
N54685 G01 Z-.0302 F40.
N54686 X4.6761 Y-2.4821
N59729 X3.1597 Y-1.1017
N59730 X3.1253
N59731 G00 Z.12
N59732 Z.1
N59733 M09
N59734 M05
N59735 G53 Z0.
N59736 G53 X0. Y0.
N59737 M00
(JOB 3 ZLEVEL FINISH)
(FEATURE Z-LEVEL UPPER FINISH)
N59738 T3 M6
G54
N59739 S10000 M03
N59740 G90 X4.5853 Y-2.9421 (You have no action in this line you would need a G0 or a G1 Etc )
N59741 G43 H3 Z.1
N59742 G01 Z-.0002 F40.
N59743 Y-3.3424 F48.
N59744 X4.5849 Y-3.3455
N141930 X1.889 Y-2.001
N141931 X1.8793 Y-2.0008
N141932 X1.8683 Y-2.0167
N141933 G00 Z.1
(JOB 4 ZLEVEL FINISH)
(FEATURE Z-LEVEL FINISH)
N141934 S10000
N141935 X1.6427 Y-2.3614
N141936 G01 Z-.3002 F40.
N194186 X2.4956 Y-1.563
N194187 X2.4831 Y-1.5693
N194188 G00 Z.1
N194189 M05
N194190 G53 Z0.
N194191 G53 X0 Y0.
N194192 M30
%

[The Engine Guy]

OK, try this code in your UCCNC, I have modified a Mach3_No_ATC PP to output this code, the PP is attached in the Zip file, just open the Zip file and do a "Copy and Paste" into your V24 Mill Post Folder, DO NOT do a "Save As" as that will change the file extension from a .MillPst file to a .txt file which cannot be read by BobCAD.
The PP is set for English (Inch) format output if that is what you need, can be easily changed if required

(BEGIN PREDATOR NC HEADER)
(MACH_FILE=HAAS - 3XVMILL.MCH)
(MTOOL T1 S1 D.315 H2.4409 A0. C0. DIAM_OFFSET 1 = .1575)
(MTOOL T2 S1 D.3937 H3.6496 A0. C0. DIAM_OFFSET 2 = .1969)
(SBOX X-1.9685 Y-1.9685 Z-1.1811 L3.937 W3.937 H1.1811)
(END PREDATOR NC HEADER)

%
O100
(PROGRAM NUMBER)
(PROGRAM NAME - SIMPLE POCKET TEST)
(POST - MACH 3 MILL NO ATC)
(DATE - SUN. 03/06/2016)
(TIME - 02:23PM)

N01 G20 G40 G49 G80 G90
N02 G28 Z0.

N03 T1 M6
N04 S4000 M03
N05 G00 G90 G54
N06 X.3614 Y-.0731
N07 G43 H1 M08
N08 Z.1969
N09 G01 Z0. F7.874
N10 Y-.1928 Z-.0063
N11 X-.0788 Z-.0293
N12 Y.3933 Z-.0601
N13 X.0787 Z-.0683
N14 Y.2359 Z-.0766
N15 X.204 Z-.0831
N16 Y-.0353 Z-.0973
N17 X.0787 Z-.1039
N18 Y.2359 Z-.1181
N19 Y-.0353 F23.622
N20 X.204
N21 Y.2359
N22 X.0787
N23 Y.3933
N24 X-.0788
N25 Y-.1928
N26 X.3614
N27 Y.3933
N28 X.0787
N29 Y.5508
N30 X-.2363
N31 Y-.3502
N32 X.5189
N33 Y.5508
N34 X.0787
N35 Y.7083
N36 X-.3937
N37 Y-.5077
N38 X.6764
N39 Y.7083
N40 X.0787
N41 Y.8658
N42 X-.5512
N43 Y-.6652
N44 X.8339
N45 Y.8658
N46 X.0787
N47 X-.5512
N48 X-.7087
N49 Y-.6652
N50 G17 G03 X-.5512 Y-.8227 I.1575 J0.
N51 G01 X.8339
N52 G03 X.9914 Y-.6652 I0. J.1575
N53 G01 Y.8658
N54 G03 X.8339 Y1.0233 I-.1575 J0.
N55 G01 X-.5512
N56 G03 X-.7087 Y.8658 I0. J-.1575
N57 G00 Z.1969
N58 M09
N59 M05
N60 G28 Z0.
N61 G28 X0. Y0.
N62 M00


N63 T2 M6
N64 S4000 M03
N65 G90 G54
N66 X-.2756 Y.1003
N67 G43 H2 M08
N68 G01 Z-.1181 F7.874
N69 Y.494 F39.3701
N70 G17 G03 X-.6693 Y.1003 I0. J-.3937
N71 G01 Y-.6652
N72 G03 X-.5512 Y-.7833 I.1181 J0.
N73 G01 X.8339
N74 G03 X.952 Y-.6652 I0. J.1181
N75 G01 Y.8658
N76 G03 X.8339 Y.9839 I-.1181 J0.
N77 G01 X-.5512
N78 G03 X-.6693 Y.8658 I0. J-.1181
N79 G01 Y.1003
N80 G03 X-.2756 Y-.2934 I.3937 J0.
N81 G01 Y.1003
N82 G00 Z.1969
N83 M09
N84 M05
N85 G28 Z0.
N86 G28 Y0.

(END OF PROGRAM)

N87 M30
%


Let me know if it is close to what you need and any "tweaks" you would like as well
For example if you would like the code to show the Tool information for the next operation at the Tool Change as a reminder then I can do that if you want it
The above code is for a simple pocket with a profile finish

I have substituted G28 for the G53 as that is what the UCCNC Manual says it uses, it may be OK as is but it may need a G91 on the same line as the G28, a lot of controllers do require it but quite possibly UCCNC have set up their control firmware to not need it
Caveat, always make sure the machine is properly HOMED before you start any code as the G28 could easily send the machine overtravel with possible damage to ballscrews etc

Anyway, try the code out first and if it is OK then give the attached PP a go and let me know how it goes

Attachment 311012

Regards
Rob
:rainfro: :rainfro: :rainfro:

[The Engine Guy]

P.S.

Sorry, I forgot to set the PP to output the G17 in the "Safety Line" see the attached modified PP

(BEGIN PREDATOR NC HEADER)
(MACH_FILE=HAAS - 3XVMILL.MCH)
(MTOOL T1 S1 D.315 H2.4409 A0. C0. DIAM_OFFSET 1 = .1575)
(MTOOL T2 S1 D.3937 H3.6496 A0. C0. DIAM_OFFSET 2 = .1969)
(SBOX X-1.9685 Y-1.9685 Z-1.1811 L3.937 W3.937 H1.1811)
(END PREDATOR NC HEADER)

%
O100
(PROGRAM NUMBER)
(PROGRAM NAME - SIMPLE POCKET TEST)
(POST - MACH 3 MILL NO ATC)
(DATE - SUN. 03/06/2016)
(TIME - 03:03PM)

N01 G17 G20 G40 G49 G80 G90
N02 G28 Z0.

N03 T1 M6
N04 S4000 M03
N05 G00 G90 G54
N06 X.3614 Y-.0731
N07 G43 H1 M08
N08 Z.1969
N09 G01 Z0. F7.874
N10 Y-.1928 Z-.0063
N11 X-.0788 Z-.0293
N12 Y.3933 Z-.0601
N13 X.0787 Z-.0683
N14 Y.2359 Z-.0766
N15 X.204 Z-.0831
N16 Y-.0353 Z-.0973
N17 X.0787 Z-.1039
N18 Y.2359 Z-.1181
N19 Y-.0353 F23.622
N20 X.204
N21 Y.2359
N22 X.0787
N23 Y.3933
N24 X-.0788
N25 Y-.1928
N26 X.3614
N27 Y.3933
N28 X.0787
N29 Y.5508
N30 X-.2363
N31 Y-.3502
N32 X.5189
N33 Y.5508
N34 X.0787
N35 Y.7083
N36 X-.3937
N37 Y-.5077
N38 X.6764
N39 Y.7083
N40 X.0787
N41 Y.8658
N42 X-.5512
N43 Y-.6652
N44 X.8339
N45 Y.8658
N46 X.0787
N47 X-.5512
N48 X-.7087
N49 Y-.6652
N50 G17 G03 X-.5512 Y-.8227 I.1575 J0.
N51 G01 X.8339
N52 G03 X.9914 Y-.6652 I0. J.1575
N53 G01 Y.8658
N54 G03 X.8339 Y1.0233 I-.1575 J0.
N55 G01 X-.5512
N56 G03 X-.7087 Y.8658 I0. J-.1575
N57 G00 Z.1969
N58 M09
N59 M05
N60 G28 Z0.
N61 G28 X0. Y0.
N62 M00


N63 T2 M6
N64 S4000 M03
N65 G90 G54
N66 X-.2756 Y.1003
N67 G43 H2 M08
N68 G01 Z-.1181 F7.874
N69 Y.494 F39.3701
N70 G17 G03 X-.6693 Y.1003 I0. J-.3937
N71 G01 Y-.6652
N72 G03 X-.5512 Y-.7833 I.1181 J0.
N73 G01 X.8339
N74 G03 X.952 Y-.6652 I0. J.1181
N75 G01 Y.8658
N76 G03 X.8339 Y.9839 I-.1181 J0.
N77 G01 X-.5512
N78 G03 X-.6693 Y.8658 I0. J-.1181
N79 G01 Y.1003
N80 G03 X-.2756 Y-.2934 I.3937 J0.
N81 G01 Y.1003
N82 G00 Z.1969
N83 M09
N84 M05
N85 G28 Z0.
N86 G28 Y0.

(END OF PROGRAM)

N87 M30
%


See modified code and modified PP below

Regards
Rob
:rainfro: :rainfro: :rainfro:

[mactec54]

The Engine Guy

G53 is fully supported by UCCNC control, and is a better choice to use than a G28, also G54 should be on a separate line

[jcarpenter2]

Wow, now im feeling guilty. Been up since 0500 working on the celtic cross from a guy on here named trotline (and not once did i log into cnczone). I actually ran across his videos a few days ago and thought i wanted to try that as it is offering some of things i have been wanting to learn. I ran two runs last night but then decided to clean up the dxf he had posted even further. The code i posted was from this trial run so i do appreciate all of you that have looked at the code. Currently i just started to run the gcode on my machine so it will be down for about 2-2.5 hours, but then i plan on checking the post processor that is posted below and see how that pans out.

[jcarpenter2]

Well it did take four hours to run. This is only with the simple changes that BanduraMaker said. Still dont like it though - to choppy. For some reason the circular moves arent coming out. The lines are circular so its not the lines causing the choppiness.

[jcarpenter2]

@The Engine Guy
Loaded the gcode below and it looked good in my uccnc controller. I did not run it at it was outside of my envelope. I set my to run only in the y- and the x+, just a preference thing because of where my machine is.
I also loaded the pp into bobcad and recreated my toolpath then loaded it into uccnc. The issues from earlier are gone. UCCNC still does not read the G17 (turns red) but everything else looked good, even the toolpaths all looked good. I have not ran that gcode either but that is because i am still trying to figure out why i am not getting arcs as you can see in the photos i posted. They are arcs in bobcad, but they are not being translated as arcs in the post and uccnc is then vcarving them as line segments. I know uccnc can not do KZ arcs, but it does do IY, JX arcs so im not sure what the issue is but am trying to figure it out.
Anyway, once i figure that out i will try the updates pp. You mentioned adding in reminders of what tool is supposed to be changed in the pp, where is that done? Didnt realize that would be important until i ran the project below and then it had me scratching my head trying to remember what tool i needed to change to.

[OlfCNC]

Noticed that you working with imperial units. Did you adjust the CV parameters in the UCCNC on the general settings page?
You may need to set them lower because too high values will allow high tolerances for the UCCNC and that can cause this kind of jagged looking paths.
The default setting for the CV planner is good for metric, but 1 inch is 25.40 times longer, so are the tolerances then.
The tighter you set the CV settings the more close the UCCNC will follow the path but the same time the machining time can go up.

[jcarpenter2]

Here is a screenshot of my general settings. I have not adjusted the CV.

Noticed that you working with imperial units. Did you adjust the CV parameters in the UCCNC on the general settings page?
You may need to set them lower because too high values will allow high tolerances for the UCCNC and that can cause this kind of jagged looking paths.
The default setting for the CV planner is good for metric, but 1 inch is 25.40 times longer, so are the tolerances then.
The tighter you set the CV settings the more close the UCCNC will follow the path but the same time the machining time can go up.

[The Engine Guy]

Try the attached PP, I have modified it to output the tool information you asked for and also removed the G17 from the "Safety Line" so you shouldn`t get any error for that anymore.

Attachment 311352

Regards
Rob
:rainfro: :rainfro: :rainfro: