[PeterGo]

Hey Everyone,

I have finished setting up my CNC replacing my Chinese cnc controller with an AXBB-E. Everything works I can stop/start spindle and control its speed. Jog the machine etc. However, I am having an issue with running g code. I can execute G0 commands but not G1 commands if I run G1 X10 Y10 Z0 F300 it does not do anything. I think this has something to do with the feed rate somehow. I have not encountered this issue before. I should mention I am using Mach 4. Any help would be much appreciated.

Peter

[76special]

Did you solve this? I've just encountered the same issue. It will happily run a test square on G0, but will stop on any G1 line

[joeavaerage]

Hi,
I've been using Mach4 for seven years, if it could not do g1 moves it would be totally hopeless, its the MOST basic move there is.

Post your code so we can see ir.

Craig

[76special]

I know right? I'm very new to this and still in my builds commissioning stage, so I'm assuming I've cocked something up.
example of my test file (50mm square) below:
%
( File created using Intuwiz Software Service )
( https://www.intuwiz.com )
( More information: https://www.intuwiz.com/rectangle.html )
( File created: 2022-03-16 08:54:09 UTC )

G00 X0 Y0 F70
G01 Z-1 F50
G01 X0 Y50 F50
G01 X50 Y50
G01 X50 Y0
G01 X0 Y0
G00 Z0 F100
M30
%

Changing the G1 to G0 works fine.
I tried a simple move in MDI with same results.
'G1 X50 F100' nothing
'G0 X50' works fine

The log for that is
2022-03-16 21:39:08.201 - Logging Enabled.
2022-03-16 21:39:10.821 - API: mcCntlCycleStart(inst = 0) (unknown caller)
2022-03-16 21:39:10.942 - Attempt transition from "Idle" on event "Cycle Start" machapi.cpp:3085
2022-03-16 21:39:10.943 - Transition from "Idle" on event "Cycle Start" was rejected by a guard function! machapi.cpp:3085

As per the OP I'm think its a feedrate issue.

[mactec54]

I know right? I'm very new to this and still in my builds commissioning stage, so I'm assuming I've cocked something up.
example of my test file (50mm square) below:
%
( File created using Intuwiz Software Service )
( https://www.intuwiz.com )
( More information: https://www.intuwiz.com/rectangle.html )
( File created: 2022-03-16 08:54:09 UTC )

G00 X0 Y0 F70
G01 Z-1 F50
G01 X0 Y50 F50
G01 X50 Y50
G01 X50 Y0
G01 X0 Y0
G00 Z0 F100
M30
%

Changing the G1 to G0 works fine.
I tried a simple move in MDI with same results.
'G1 X50 F100' nothing
'G0 X50' works fine

The log for that is
2022-03-16 21:39:08.201 - Logging Enabled.
2022-03-16 21:39:10.821 - API: mcCntlCycleStart(inst = 0) (unknown caller)
2022-03-16 21:39:10.942 - Attempt transition from "Idle" on event "Cycle Start" machapi.cpp:3085
2022-03-16 21:39:10.943 - Transition from "Idle" on event "Cycle Start" was rejected by a guard function! machapi.cpp:3085

As per the OP I'm think its a feedrate issue.

What do you have above the posted code

Try a period after the F70. F50.

You don't use a Feed rate with a G0 move

[joeavaerage]

Hi,
Machs Gcode interpreter parses all Gcode to reduce to lowercase ALL letters, strips out leading zeros and strips out whitespace.
Mostly any code presented to Mach will be interpreted correctly, but I wounder if that is the case here.

For instance G01 X0 Y50 gets interpreted as g1x0y50. May I suggest try re-writing the code to see if it makes any difference.

The second question I have is this in metric units or inch units? Adding a g20 or g21 at the start of the code would be a good idea.
Are the native units of the machine different to the units of the Gcode? It shouldn't make any difference when you use g20 or g21 but it may
help eliminate a problem.

This is a snippet of code that I ran this morning (using Mach4), so I know it works:

(BOSS)
(T2  D=1.5 CR=0. - ZMIN=-1. - FLAT END MILL)
G90 G94 G91.1 G40 G49 G17
G21

(2D CONTOUR1)
M5
T2 M6
S24000 M3
G4 P6.00
G54
M8
G0 X-0.081 Y-2.148
G43 Z15. H2
Z5.
G1 Z2.5 F200.
G2 X-2.148 Y0.081 Z2.382 R2.15 F400.
X0. Y2.15 Z2.267 R2.15
G1 X1. Z2.232
G2 X3.15 Y0. Z2.114 R2.15
X1. Y-2.15 Z1.996 R2.15
G1 X0. Z1.961
G2 X-2.15 Y0. Z1.843 R2.15
X0. Y2.15 Z1.725 R2.15
G1 X1. Z1.69
G2 X3.15 Y0. Z1.573 R2.15
X1. Y-2.15 Z1.455 R2.15
G1 X0. Z1.42
G2 X-2.15 Y0. Z1.302 R2.15
X0. Y2.15 Z1.184 R2.15
G1 X1. Z1.149
G2 X3.15 Y0. Z1.031 R2.15

Craig

[76special]

Solved it!
Joe - I was looking at your 3rd line in the above code, the 'safe start line', and noticed it was different to the basic one I'd used (straight from themach4 manual).
I looked up the extra codes and saw G94 'Feed per Minute which looked promising.
Adding that did the trick. The problem & solution are repeatable, so I'm all sorted.
Thanks everyone

[mactec54]

Solved it!
Joe - I was looking at your 3rd line in the above code, the 'safe start line', and noticed it was different to the basic one I'd used (straight from themach4 manual).
I looked up the extra codes and saw G94 'Feed per Minute which looked promising.
Adding that did the trick. The problem & solution are repeatable, so I'm all sorted.
Thanks everyone

You should not need a G94 to make it work, his code also has the dot at the end the F--- . line also which should make your one work, without the G94 which is not normally used in normal programing

[dazp1976]

What do you have above the posted code
Try a period after the F70. F50.
You don't use a Feed rate with a G0 move

Now that is a good point.
Been looking through some of my codes and all F have a period.

Occasionally do on the axis values too. As if the axis in question is told to stay in place for a few lines while the other axis move.

[dazp1976]

Maybe something in the post script saying to ignore F commands?.
Just fishing.

[metalmayhem]

g94 should be default upon start up . I don't know about mach 4 but a lot of controls will read f50 (without decimal) as f.0005

[joeavaerage]

Hi,
the period at the end of the F command is a red herring. I have code produced by CAM that sometimes produces a period at the end, and sometimes not.
Any handwritten code certainly does not have a period at the end and yet all code works with or without the period. This works for Mach4, whether it applies to
other CNC software is more than I can say.

G94/G95 is modal. To my knowledge G95, Feed per Revolution, is only ever used in lathe operations, so unless you have a lathe profile I would not expect that Mach would ever end up
in G95 mode. Your machine has however. You could put a G94 in the 'Initialization Codes' of the Configure/Control/Defaults tab, thus you could be assured that at each
start-up Mach is in Feed per Minute mode..

I don't know what screenset you are using but the screenshot attached is of wx6 one of the standard screesets supplied by NFS with every Mach4 build. Note that in the middle
of the string there is a G94.

Craig

[metalmayhem]

Hi,


G94/G95 is modal. To my knowledge G95, Feed per Revolution, is only ever used in lathe operations,

Craig

feed per rev is also used in many mill tapping cycles , depending on the control . I doubt g94 needs to be added to the initial start up codes for a milling profile . Mach 3 starts up with that along with a number of other codes and I'd assume mach 4 would as well .
turning should should start up with g95 but it appears mach 3 turn defaults to g94 .

[joeavaerage]

Hi,

feed per rev is also used in many mill tapping cycles , depending on the control . I doubt g94 needs to be added to the initial start up codes for a milling profile

Yes, I can see that feed per rev would be extremely useful for tapping. I've used Mach3 for several years and Mach4 for a further seven years and in that time I've never had Mach start
in G95 mode. Then again the screenset I use specifically codes a G94 so I have never had to use an initialization code.

Craig

[metalmayhem]

thats my point , g94 shouldn't need to be added , it is there by default .
with mach turn it should default to g95 but it doesn't

[joeavaerage]

Hi,
which is why I asked OP what screenset he is using, if he has made his own then quite possibly a g94 is not included when it should be.

Craig

[76special]

I used a copy of the wx4 screenset and the G94 wasn't in the initialization Codes. I've added it, and it works fine now without needing to included it in the gcode itself.

The controller I'm using is a wiXhc and it originally didn't want to play nice with the GUI version of Mach4 (wxMach.exe only).
It took a bit of fiddling in notepad to get it working properly and figured I'd just butchered something in the process (I'm building an ESS/HG08 in parallel as a long term replacement)

Thanks again for the help, its making the learning curve a lot easier

[joeavaerage]

Hi,
you are the only person I've ever heard of who has stuck with that XHC controller. You need to ditch it and get a controller which supports MachGUI,
you're only getting a fraction of what Mach4 has to offer with wxMach.

Craig

[76special]

Yeah I hear they don't have good rep, but it works fine under MachGUI since I fixed the config files, plus, its got loads of IO's.
I've do have a half-built ESS/HG08 as a backup.
Cheers,
Roly