[techtonix]

Hi Madcam user forum, I am looking for a post processor for the Axiom basic4 mill I recently purchased. 24"x24"x6"
The router is a 2hp bosch with the speed controlled manually (not through the gcode).

The controller is the chinese made Rich11,
and is the same controller as the Laguna IQ HHC

I AxiomPrecision had more support for your software on their website, but they are a new company, and I might be the only MadCammer using an Axiom machine.
The post file I get from you, I will forward back to Axiom for their user support.

If you have this post file, your support is greatly appreciated.
many thanks
-Ben

Here is a Vectric (amature sucky software) post file for my controller, maybe I can tweak this myself with a little forum help?

+================================================
+
+Axiom DSP Handheld Control - Vectric machine output configuration file
+
+================================================
+
+ History
+
+ Who When What
+ ======== ========== ===========================
+ Todd 05/08/2014 Written for metric
+================================================


POST_NAME = "AXIOM HHC CNC (mm) (*.mmg)"


FILE_EXTENSION = "mmg"


UNITS = "MM"


SUBSTITUTE = "({)}"


+------------------------------------------------
+ Line terminating characters
+------------------------------------------------


LINE_ENDING = "[13][10]"


+------------------------------------------------
+ Block numbering
+------------------------------------------------


LINE_NUMBER_START = 0
LINE_NUMBER_INCREMENT = 10
LINE_NUMBER_MAXIMUM = 999999


+================================================
+
+ Formating for variables
+
+================================================


VAR LINE_NUMBER = [N|A|N|1.0]
VAR SPINDLE_SPEED = [S|A|S|1.0]
VAR FEED_RATE = [F|C|F|1.1]
VAR X_POSITION = [X|C|X|1.3]
VAR Y_POSITION = [Y|C|Y|1.3]
VAR Z_POSITION = [Z|C|Z|1.3]
VAR ARC_CENTRE_I_INC_POSITION = [I|A|I|1.3]
VAR ARC_CENTRE_J_INC_POSITION = [J|A|J|1.3]
VAR X_HOME_POSITION = [XH|A|X|1.3]
VAR Y_HOME_POSITION = [YH|A|Y|1.3]
VAR Z_HOME_POSITION = [ZH|A|Z|1.3]
VAR SAFE_Z_HEIGHT = [SAFEZ|A|Z|1.3]
+================================================
+
+ Block definitions for toolpath output
+
+================================================


+---------------------------------------------------
+ Commands output at the start of the file
+---------------------------------------------------


begin HEADER
"(Filename: [TP_FILENAME])"
"[N]M03[S]"
"([TOOLPATH_NAME])"
+"[N][XH][YH][F]"




+---------------------------------------------------
+ Commands output for rapid moves
+---------------------------------------------------


begin RAPID_MOVE


"[N]G00[X][Y][Z]"




+---------------------------------------------------
+ Commands output for the first feed rate move
+---------------------------------------------------


begin FIRST_FEED_MOVE


"[N]G1[X][Y][Z][F]"




+---------------------------------------------------
+ Commands output for feed rate moves
+---------------------------------------------------


begin FEED_MOVE


"[N]G1[X][Y][Z]"


+---------------------------------------------------
+ Commands output for the first clockwise arc move
+---------------------------------------------------


begin FIRST_CW_ARC_MOVE


"[N]G2[X][Y][I][J][F]"


+---------------------------------------------------
+ Commands output for clockwise arc move
+---------------------------------------------------


begin CW_ARC_MOVE


"[N]G2[X][Y][I][J]"


+---------------------------------------------------
+ Commands output for the first counterclockwise arc move
+---------------------------------------------------


begin FIRST_CCW_ARC_MOVE


"[N]G3[X][Y][I][J][F]"


+---------------------------------------------------
+ Commands output for counterclockwise arc move
+---------------------------------------------------


begin CCW_ARC_MOVE


"[N]G3[X][Y][I][J]"


+---------------------------------------------------
+ Commands output for a new segment - toolpath
+ with same toolnumber but maybe different feedrates
+---------------------------------------------------


begin NEW_SEGMENT


+"[N][S]M03"
"([TOOLPATH_NAME])"
+"([TOOLPATH_NOTES])"


+---------------------------------------------------
+ Commands output at the end of the file
+---------------------------------------------------


begin FOOTER


"[N]G00[ZH]"
"[N]M05"
"[N]M30"
%



Axiom4 basic
Shenhui 50w laser
Rhino5 expert
Architect / Designer

[Dan B]

It would be more useful to have a sample of good code that drives your machine. Then that can be "reverse engineered" into a madCAM post.

Dan

[techtonix]

It would be more useful to have a sample of good code that drives your machine. Then that can be "reverse engineered" into a madCAM post.

Dan

Hi Dan,
Thanks for the reply,
Here is one sent directly from Axiom

(Filename: Surface8)
N10M03S12000
(Pocket 1)
N30G00X590.442Y18.415Z5.080
N40G1Z-0.500F762.0
N50G1Y1191.585F2540.0
N60G1X577.742
N70G1Y18.415
N80G1X565.042
N90G1Y1191.585
N100G1X552.342
N110G1Y18.415
N120G1X539.642
N130G1Y1191.585
N140G1X526.942
N150G1Y18.415
N160G1X514.242
N170G1Y1191.585
N180G1X501.542
N190G1Y18.415
N200G1X488.842
N210G1Y1191.585
N220G1X476.142
N230G1Y18.415
N240G1X463.442
N250G1Y1191.585
N260G1X450.742
N270G1Y18.415
N280G1X438.042
N290G1Y1191.585
N300G1X425.342
N310G1Y18.415
N320G1X412.642
N330G1Y1191.585
N340G1X399.942
N350G1Y18.415
N360G1X387.242
N370G1Y1191.585
N380G1X374.542
N390G1Y18.415
N400G1X361.842
N410G1Y1191.585
N420G1X349.142
N430G1Y18.415
N440G1X336.442
N450G1Y1191.585
N460G1X323.742
N470G1Y18.415
N480G1X311.042
N490G1Y1191.585
N500G1X298.342
N510G1Y18.415
N520G1X285.642
N530G1Y1191.585
N540G1X272.942
N550G1Y18.415
N560G1X260.242
N570G1Y1191.585
N580G1X247.542
N590G1Y18.415
N600G1X234.842
N610G1Y1191.585
N620G1X222.142
N630G1Y18.415
N640G1X209.442
N650G1Y1191.585
N660G1X196.742
N670G1Y18.415
N680G1X184.042
N690G1Y1191.585
N700G1X171.342
N710G1Y18.415
N720G1X158.642
N730G1Y1191.585
N740G1X145.942
N750G1Y18.415
N760G1X133.242
N770G1Y1191.585
N780G1X120.542
N790G1Y18.415
N800G1X107.842
N810G1Y1191.585
N820G1X95.142
N830G1Y18.415
N840G1X82.442
N850G1Y1191.585
N860G1X69.742
N870G1Y18.415
N880G1X57.042
N890G1Y1191.585
N900G1X44.342
N910G1Y18.415
N920G1X31.642
N930G1Y1191.585
N940G1X18.942
N950G1Y18.415
N960G00Z5.080
N970G00X15.875Y1194.125
N980G1Z-0.500F762.0
N990G1Y15.875F2540.0
N1000G1X594.125
N1010G1Y1194.125
N1020G1X15.875
N1030G00Z5.080
N1040G00Z12.700
N1050M05
N1060M30
%

[Dan B]

This looks like pretty straightforward Fanuc based G-code. Do you have a tool changer? Do you do drilling too? Or is this just for milling? Or both?

I suspect there are some lines in the beginning that should be added. I'll provide a sample from an existing post I have and maybe you can try it on your machine and tell me what happens. First, let me know about the tool changer and the type of work you plan to do.

Thanks,

Dan

[techtonix]

Hi Dan,
Thanks for the reply, no tool changer, just a simple 24x24x6 router mill.
I'll be using the machine mostly for mold making out of soft materials, and for carving finished pieces out of hardwood and soft metals aluminum.
I probably won't be doing much drilling at all, though some occasional 2d profiling.
Thanks,
Ben

[Dan B]

Can you try this code?

%O300
(This code is from madCAM for the Axiom)
(This is path #300)
N1 G0G17G40G80G90M5M9H0Z0
N3 G00X0.637Y-199.999E1S2600M3
N5 G00Z33.350M8
N6 G01Z31.987F7500
N7 G01Z25.637F1000
N8 G01X0.000Z25.000F1200
N9 X0.637
N10 X200.000
N11 G01Z31.350F7500
N12 G01X199.363Y-171.428F7500
N13 G01Z25.637F1000
N14 G01X200.000Z25.000F1200
N15 X199.363
N16 X0.000
N17 G01Z31.350F7500
N18 G01X0.637Y-142.857F7500
N19 G01Z25.637F1000
N20 G01X0.000Z25.000F1200
N21 X0.637
N22 X200.000
N23 G01Z31.350F7500
N24 G01X199.363Y-114.286F7500
N25 G01Z25.637F1000
N26 G01X200.000Z25.000F1200
N27 X199.363
N28 X0.000
N29 G01Z31.350F7500
N30 G01X0.637Y-85.714F7500
N31 G01Z25.637F1000
N32 G01X0.000Z25.000F1200
N33 X0.637
N34 X200.000
N35 G01Z31.350F7500
N36 G01X199.363Y-57.143F7500
N37 G01Z25.637F1000
N38 G01X200.000Z25.000F1200
N39 X199.363
N40 X0.000
N41 G01Z31.350F7500
N42 G01X0.637Y-28.572F7500
N43 G01Z25.637F1000
N44 G01X0.000Z25.000F1200
N45 X0.637
N46 X200.000
N47 G01Z31.350F7500
N48 G01X199.363Y-0.000F7500
N49 G01Z25.637F1000
N50 G01X200.000Z25.000F1200
N51 X199.363
N52 X0.000
N53 G01Z29.175F7500
N54 G01Z33.350F7500
N55 M5
N56 M9
N57 G90G0H0Z0
N58 M30
%

This piece of code tests a number of things. If it fails to run, please let me know where it stopped. I've added support for fixture offsets, using modal code (not repeating G01 every line), put in a "safety line" etc. If this runs, I can "reverse engineer" it into a post fairly quickly.

Thanks,

Dan

[techtonix]

Can you try this code?

This piece of code tests a number of things. If it fails to run, please let me know where it stopped. I've added support for fixture offsets, using modal code (not repeating G01 every line), put in a "safety line" etc. If this runs, I can "reverse engineer" it into a post fairly quickly.

Thanks,

Dan

Hi Dan,
Tested it out just now. it ran through the whole thing without any errors or stops, the controller said it finished successfully and returned back to home origin.
thanks!

[Dan B]

Okay, good.

In the above example I have substituted rapids with fast linear moves. This is because some machines will ignore rapids and do "dog-leg" moves if it encounters a G0. Is this the case with your machine, or am I safe to use rapids (everywhere you see a G1 F7500)? It doesn't hurt to do it as I have shown above, as long as our feed is close to your maximum possible feedrate. How fast can your machine feed? Is 7500mm/min realistic, or can you go faster?

Also, I used E1 for the fixture offset, which works for a Fadal. It didn't cause an error on your machine, but what would happen if you changed that to G54? Can you try that and let me know what happens?

So, N3 G00X0.637Y-199.999E1S2600M3 becomes N3 G00X0.637Y-199.999G54S2600M3

Thanks,

Dan

[Dan B]

Or maybe just run this:

%O302
(This code is from madCAM for the Axiom)
(This is path #302)
N1 G0G17G40G80G90M5M9
N2 G00X0.637Y-199.999G54S2600M3
N3 G00Z33.350M8
N4 G01Z31.987F7500
N5 G01Z25.637F1000
N6 G01X0.000Z25.000F1200
N7 X0.637
N8 X200.000
N9 G01Z31.350F7500
N10 G01X199.363Y-171.428F7500
N11 G01Z25.637F1000
N12 G01X200.000Z25.000F1200
N13 X199.363
N14 X0.000
N15 G01Z31.350F7500
N16 G01X0.637Y-142.857F7500
N17 G01Z25.637F1000
N18 G01X0.000Z25.000F1200
N19 X0.637
N20 X200.000
N21 G01Z31.350F7500
N22 G01X199.363Y-114.286F7500
N23 G01Z25.637F1000
N24 G01X200.000Z25.000F1200
N25 X199.363
N26 X0.000
N27 G01Z31.350F7500
N28 G01X0.637Y-85.714F7500
N29 G01Z25.637F1000
N30 G01X0.000Z25.000F1200
N31 X0.637
N32 X200.000
N33 G01Z31.350F7500
N34 G01X199.363Y-57.143F7500
N35 G01Z25.637F1000
N36 G01X200.000Z25.000F1200
N37 X199.363
N38 X0.000
N39 G01Z31.350F7500
N40 G01X0.637Y-28.572F7500
N41 G01Z25.637F1000
N42 G01X0.000Z25.000F1200
N43 X0.637
N44 X200.000
N45 G01Z31.350F7500
N46 G01X199.363Y-0.000F7500
N47 G01Z25.637F1000
N48 G01X200.000Z25.000F1200
N49 X199.363
N50 X0.000
N51 G01Z29.175F7500
N52 G01Z33.350F7500
N53 M5
N54 M9
N55 M30
%

How does this one work? Do you see machine movement corresponding to the image below?

Attachment 275822

Thanks,

Dan

[techtonix]

Hi Dan,
It seems to have worked out fine.

1>In the past I used to set the z0 to the top of the material, this was on another machine a decade ago.
i'ts been quite a few years since I used a cnc machine extensively, so I'm actively re-learning how to read code again. :violin:
I set the z0 to the top pf the material here and the cut path ran at 25mm above.
*Was the 25mm above the result of the material thickness you programmed in this g-code?
I'm not sure what the norm is now, Z set at material base or material top?

2>I had the machine manually planing some MDF at 5500mm/min at 2200rpm and it seemed totally fine.
The user manual states a feed rate of 8000/min, so for warranty reasons, lets set that as the max.

3> Since the Axiom4 Basic uses a consumer router, I have to re-set the z0 every time I change a bit.
is this what the fixture offset of E1 or G54 refers to? Sorry I'm rusty on this stuff still.

thanks,
Ben

[Dan B]

Hi Ben,

You can set the Z0 where ever you want. In my example I set it on the bottom. I could just as easily have set it on the top. It doesn't matter as long as you pick it up on the machine to match where it is in your CAD file.

I will adjust the post to 8000mm/min max "rapid" speed. That's an easy change.

The fixture offset (I will stick with the more conventional G54) allows you to have multiple parts on the table, and run separate paths for each. For example, let's say you had 4 parts to machine and each has a separate tool path. Mount the 4 blocks onto your table and proceed to pick up the first one. Now save that as G54. Now pick up the second one, and save that location as G55. Proceed with the next 2 as G56 and G57. Now in your code, post each of the paths with the corresponding offset. madCAM lets you do that right from the post-processor page. Then using a text editor (I highly recommend Notepad++) copy the paths one after another, removing the M30 and % from between them. Now when you run it, all 4 pieces will be machined,

I'll have your post ready this morning.

Dan

[Dan B]

Here is the post. Copy and paste this into a .txt file and save where you keep your posts.

//MadCAM_POST_2015-04-08 by Dan Bayn
*VERSION*
1.00
*FILE_NAME*
Axiom
*FILE_EXTENSION*
nc
*FILE_DEST*
c:\cnc-code\
*FILTER*
0.001
*OUTPUT_WIDTH*
4
*OUTPUT_DECIMALS*
3
*SCALE_X*
1
*SCALE_Y*
1
*SCALE_Z*
1
*AXIS_1_CHAR*
X
*AXIS_2_CHAR*
Y
*AXIS_3_CHAR*
Z
*CUTTER_REFERENCE*
TIP
*END_SECTION*
*CUSTOM_VARIABLES*
Fixture offset;fixture_offset;G54
*END_SECTION*
*FIRST_MOVE*
N"lnbr" G00"x""y""fixture_offset"S"speed"M3
N"lnbr" G00"z""coolant_on"
*END_SECTION*
*RAPID*
N"lnbr" G01"x""y""z"F8000
*END_SECTION*
*RAPID_APPROACH*
N"lnbr" G01"x""y""z"F8000
*END_SECTION*
*RAPID_RETRACT*
N"lnbr" G01"x""y""z"F8000
*END_SECTION*
*RAPID_FEED*
8000
*END_SECTION*
*TOOLCHANGE_TIME*
.33
*END_SECTION*
*APPROACH*
N"lnbr" G01"x""y""z"F"feedz"
*END_SECTION*
*FIRST_CUT*
N"lnbr" G01"x""y""z"F"feed"
*END_SECTION*
*CUT*
N"lnbr" "x""y""z"
*END_SECTION*
*TOOL_CHANGE*
*END_SECTION*
*TOOLPATH_CHANGE*
N"lnbr" ( TOOL #"toolnr" CONTINUES)
*END_SECTION*
*TOOL_STOP*
N"lnbr" M5
N"lnbr" M9
*END_SECTION*
*PROGRAM_START*
%O1
(This code is from madCAM for the Axiom)
(This is path #"pgmnr")
N"lnbr" G0G17G40G80G90M5M9
*END_SECTION*
*PROGRAM_END*
N"lnbr" M30
%
*END_SECTION*
*LINE_START_NUMBER*
1
*END_SECTION*
*COOLANT_ON*
M8
*END_SECTION*
*COOLANT_OFF*
M9
*END_SECTION*

Let me know if you have any issues.

Dan

[techtonix]

Hi Dan,

I had a chance to test out this g-code out on an actual cut file.
It seems that it causes the Z axis to move too fast which makes the stepper motor skip steps. I can hear it audibly when this happens, and it's not always consistent.
The result is that when say a 10mm Traverse safe distance is set, after hearing the noise, the bit be at maybe 5mm when traversing, or if it happens multiple times would be impacting the material block.
I have been testing this without a bit, so no damage has been done.
So can we slow down the Z movement a bit, maybe 1/3 the speed. Is it possible to smooth out or cushion some movements with acceleration?
This slipping seems to only happen when the Z head is returning back to the top in preparation to traverse to another location.

Also I went into the Post file and changed the *Rapid Retract* from 8000 down to 700. It helped a bit, but there are still some other Z axis moves that are much to fast that cause the stepper to skip. I had also changed the *Rapid* to 700 which fixed the problem, except the X and Y were then painfully slow.
Is there a way to Change only the *Rapid* Z?

thanks,
Ben

[techtonix]

Here is a Video showing the problem.
I can't quite figure out if it is the g-code (post processor) or the controller settings.

https://youtu.be/2a5lXbB381Q

[Dan B]

I don't think I can separate the retract in the Z so that it has a different feedrate. However, I do have another idea. What if we substituted the G01F8000 for a rapid move (G00)? You would have to test and make sure the controller isn't going to over ride the X and Y moves when under G00 control (like Fadals do). If you are not cutting objects with standing "islands" then this probably wouldn't be an issue anyway. If all your repositioning moves are above the material, then there should be nothing to worry about.

Try this post:

//MadCAM_POST_2015-04-20 by Dan Bayn
*VERSION*
1.01
*FILE_NAME*
Axiom
*FILE_EXTENSION*
nc
*FILE_DEST*
c:\cnc-code\
*FILTER*
0.001
*OUTPUT_WIDTH*
4
*OUTPUT_DECIMALS*
3
*SCALE_X*
1
*SCALE_Y*
1
*SCALE_Z*
1
*AXIS_1_CHAR*
X
*AXIS_2_CHAR*
Y
*AXIS_3_CHAR*
Z
*CUTTER_REFERENCE*
TIP
*END_SECTION*
*CUSTOM_VARIABLES*
Fixture offset;fixture_offset;G54
*END_SECTION*
*FIRST_MOVE*
N"lnbr" G00"x""y""fixture_offset"S"speed"M3
N"lnbr" G00"z""coolant_on"
*END_SECTION*
*RAPID*
N"lnbr" G00"x""y""z"
*END_SECTION*
*RAPID_APPROACH*
N"lnbr" G00"x""y""z"
*END_SECTION*
*RAPID_RETRACT*
N"lnbr" G00"x""y""z"
*END_SECTION*
*RAPID_FEED*
8000
*END_SECTION*
*TOOLCHANGE_TIME*
.33
*END_SECTION*
*APPROACH*
N"lnbr" G01"x""y""z"F"feedz"
*END_SECTION*
*FIRST_CUT*
N"lnbr" G01"x""y""z"F"feed"
*END_SECTION*
*CUT*
N"lnbr" "x""y""z"
*END_SECTION*
*TOOL_CHANGE*
*END_SECTION*
*TOOLPATH_CHANGE*
N"lnbr" ( TOOL #"toolnr" CONTINUES)
*END_SECTION*
*TOOL_STOP*
N"lnbr" M5
N"lnbr" M9
*END_SECTION*
*PROGRAM_START*
%O1
(This code is from madCAM for the Axiom)
(This is path #"pgmnr")
N"lnbr" G0G17G40G80G90M5M9
*END_SECTION*
*PROGRAM_END*
N"lnbr" M30
%
*END_SECTION*
*LINE_START_NUMBER*
1
*END_SECTION*
*COOLANT_ON*
M8
*END_SECTION*
*COOLANT_OFF*
M9
*END_SECTION*

Let me know how this works out.

Dan

[Mauri R]

techtonix,
Try this Code.
I changed the Rapids so it will split X/Y with Z and provide a lower F speed for Z.
Regards,
Mauri.

//MadCAM_POST_2015-04-08 by Dan Bayn revised by Mauri R
*VERSION*
1.00
*FILE_NAME*
Axiom
*FILE_EXTENSION*
nc
*FILE_DEST*
c:\cnc-code\
*FILTER*
0.001
*OUTPUT_WIDTH*
4
*OUTPUT_DECIMALS*
3
*SCALE_X*
1
*SCALE_Y*
1
*SCALE_Z*
1
*AXIS_1_CHAR*
X
*AXIS_2_CHAR*
Y
*AXIS_3_CHAR*
Z
*CUTTER_REFERENCE*
TIP
*END_SECTION*
*CUSTOM_VARIABLES*
Fixture offset;fixture_offset;G54
*END_SECTION*
*FIRST_MOVE*
N"lnbr" G00"x""y""fixture_offset"S"speed"M3
N"lnbr" G00"z""coolant_on"
*END_SECTION*
*RAPID*
N"lnbr" G00"x""y"F8000
N"lnbr" G00 "z"F4000
*END_SECTION*
*RAPID_APPROACH*
N"lnbr" G00"x""y"F8000
N"lnbr" G00 "z"F4000
*END_SECTION*
*RAPID_RETRACT*
N"lnbr" G00"x""y"F8000
N"lnbr" G00 "z"F4000
*END_SECTION*
*RAPID_FEED*
8000
*END_SECTION*
*TOOLCHANGE_TIME*
.33
*END_SECTION*
*APPROACH*
N"lnbr" G01"x""y""z"F"feedz"
*END_SECTION*
*FIRST_CUT*
N"lnbr" G01"x""y""z"F"feed"
*END_SECTION*
*CUT*
N"lnbr" "x""y""z"
*END_SECTION*
*TOOL_CHANGE*
*END_SECTION*
*TOOLPATH_CHANGE*
N"lnbr" ( TOOL #"toolnr" CONTINUES)
*END_SECTION*
*TOOL_STOP*
N"lnbr" M5
N"lnbr" M9
*END_SECTION*
*PROGRAM_START*
%O1
(This code is from madCAM for the Axiom)
(This is path #"pgmnr")
N"lnbr" G0G17G40G80G90M5M9
*END_SECTION*
*PROGRAM_END*
N"lnbr" M30
%
*END_SECTION*
*LINE_START_NUMBER*
1
*END_SECTION*
*COOLANT_ON*
M8
*END_SECTION*
*COOLANT_OFF*
M9
*END_SECTION*

[Mauri R]

techtonix,
I should have also changed the G00 to G01 on the three changes that I made.
Regards,
Mauri.

[Dan B]

That doesn't work. Look closely at your code.

%O1
(This code is from madCAM for the Axiom)
(This is path #1)
N1 G0G17G40G80G90M5M9
N2 G00X0.637Y-199.999G54S2600M3
N3 G00Z33.350M8
N4 G01F8000 <<<
N5 G01 Z31.987F4000
N6 G01Z25.637F1000
N7 G01X0.000Z25.000F1200
N8 X0.637
N9 X200.000
N10 G01F8000 <<<
N11 G01 Z31.350F4000
N12 G01X199.363Y-171.428F8000
N13 G01 F4000 <<<
N14 G01Z25.637F1000
N15 G01X200.000Z25.000F1200
N16 X199.363
N17 X0.000
N18 G01F8000 <<<
N19 G01 Z31.350F4000
N20 G01X0.637Y-142.857F8000
N21 G01 F4000 <<<

[techtonix]

hi Mauri,
In the first test, this seems to have worked -almost- perfectly.
I carefully monitored all 3 axis speeds and they do exactly as you have programmed.
I went into the post myself and calibrated the speeds a bit.

There was one little spot of inconsistency where a Y direction cut (3000) curves up into a Z (1500) retract. When this happens the Z goes up to (3500).
It seems like an error from the controller or a bad syntax, more than anything in the toolpath. I went back to the couple spots where this happens and there are no ramps upward in that area.
I will see if I can locate the exact lines in the code this happens...

here are my calibrations on your last code, do they look okay?
*END_SECTION*
*RAPID*
N"lnbr" G00 "x""y"F4500
N"lnbr" G01 "z"F1500
*END_SECTION*
*RAPID_APPROACH*
N"lnbr" G00 "x""y"F4500
N"lnbr" G01 "z"F1500
*END_SECTION*
*RAPID_RETRACT*
N"lnbr" G00 "x""y"F4500
N"lnbr" G01 "z"F1500
*END_SECTION*
*RAPID_FEED*
4500
*END_SECTION*

Thanks,
Ben

[Dan B]

Okay, I stand corrected. I'll bow out of this now and let Mauri take over. :-)

Dan