Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: Sage on October 17, 2008, 09:13:24 AM
-
I generated some G-code which causes the "Abnormal Condition" warning light to flash on the Mach control panel. If I clck on the warning light it lists the problem as "Exact Stop vs CV mode".
The code runs ok.
I created an offset in lazy cam on something that had square corners. It insisted on rounding the corners so instead of fighting with it I accepted it's code any way and then fixed it up myelf by hand to remove the arcs it generated and replaced then with straight moves. Not sure if that led up to this problem.
Is this warning something I need to be concerned with.
Sage
-
You must decide whether you are running in Constant Velocity mode (CV) or in exact stop mode - and you can switch between the two in General Config.
Exact stop means what it says. At the end of each line of code, the axis all come to an exact stop. The next line is computed and then all axis start again.
If you require square corners then you must run in Exact Stop.
In Constant Velocity mode, the next line is already calculated, and as the axis are slowing down at the end of the line to come to a stop, the next line is introduced and the axis simultaneously accelerate into the next line.
You can see, therefore why square corners are not possible with Constant Velocity.
You must, therefore, set your computer to do whichever you wish before you start. Constant velocity is the default setting (I think)
-
That abnormal condition button is a royal PITA as far as I am concerned, its kind of like the wee boxes that pop up in windows and say Are you sure you want to do this. They just get the user panicking as they think there is something wrong. In Mach your default setting will be set to CV but because your code has a G61 in it it changes to Exact Stop mode and Mach sees that as an abnormal condition which in reality it is not. Your code may then have a G64 which will change things back to CV and may bring up another warning if you tell Mach that ES is the norm.
Hood
-
Oh and jim, square corners are possible with CV if your code arcs round at the cutters rad ;)
Hood
-
Thanks guys. That's good insight as to what Mach is "thinking".
After trouble shooting step by step (inserting m1's here and there) I found a couple of places causing different "abnormal condition" warnings. (I'm a rookey at Gcode so go easy on me).
The one about CV seems to come and go. The last time I ran the program it was being generated while the code was drilling. Maybe the look ahead nature of the program execution is confusing the real line that is causing the problem but there are no arcs being cut until quite a while down in the code from where the light comes on.
The other one seems to be caused by a bit of code something like this. (I think it's acceptable - no?)
G91
G0 Z-.020
G90
The light turns on for the G91 line and goes out on the G90 line. Under normal feed rates it just flashes briefly going un-noticed mostly.
The error reported in this case is "G90 / G91 State".
I'll attached the code. I'd appreciate your comments.
You'll probably want to change all the feed rates to 10 instead of 1 unless you like watching paint dry.
The CV error is visible near the beginning of the program during BOTH of the drilling sequences.
I left some M1's in the code to stop during the "G91 / G90" problem in the outline milling subroutine at the bottom.
Sage
-
Best thing to do is remove the button from your screenset then you wont get it blinking at you, I dont have one on my screen so never have to look at it telling me I am abnormal ;D
Hood
-
I have been ignoring that screen since the first day it winked at me.
So what or when should someone pay attention to it?
The question may sound dumb, but, if all works for me.....no problems ..... just don't even take time to read it anymore!
RICH
MODIFIED POST / COMMENT: Change to my thinking, i will pay attention to it, read it, and use it as a tool to refine my skills and
knowledge of what i am doing. ???
-
Rich, I never even knew that button had been added to the screen until maybe 6 months after it had been as I used my own screenset. I decided I better look at the standard screen to see what everyone was talking and worrying about, decided there and then that I would not add it to my screenset ;D
Hood
-
Hi, Rich
Art posted this, Not sure if theres a complete list anywhere.
Also, two new features are added. The Diags screen shows a mathmatical
formula of your work coordinates showing how your end coordinate is being
derived, Work Offsets, tool offsets anf G91 offsets are all shown in a talley
baord to show what offsets are in effect.
A new condition monitor has been placed on the main screen. It will not
activate any monitoring until set.
To set your "abnormal condition" monitor. You need to have your machine in the
state you consider most normal. This is in terms of the status of various things
like "are the axis homed?", "Is the unit OffLine or online?", "is it set to mm's
or inches?"," Is IJ Mode incremntal or abs"...etc..
In other words have your machine in the condition you consider to be
"Normal". Then, double click the "Condition" monitoring Icon on the main
screen. Your system from this point forward will flash "Abnormal" if certain
things are changed. Lets say you set the monitor when you were in mm's. If yu
now execute a G20, or switch to Inch mode in any way, the abnormal light will
begin to blink.
Abnormal does not mean you have a problem. It is just a way to see, at a
glance, that your machine is not in a state that you normally use. Its a visual
warning that you maybe should reset whatever is different when this job is done
so next time you use it you dont get surprised with starting a job in mm's, when
your used to inches because the last job changed it on you. To find out
specifically whats changed, just click once on the "Condition" Icon. A tip box
will come on for 3 seconds to tell you whats different..
Remember, an "Abnormal Condition " alert does NOT mean your broke or have
anything to fix, its just telling you that something important to you may have
changed. To shut off the current warning, just double click it and reset it to
believe that current conditions are "normal". Current "Normals" are saved in
the profile, so each profile can have a different meaning as to what it
considers Normal..
My thanks to John Prentice and Olivier for their work in both "Condition
Monitoring" and calculation formulas onscreen as telltales to the user. I have
shamelessly stolen both ideas, and implemented them in the core code as I think
they are excellent troubleshooting aids.... :-)
Thanks, Art
www.artofcnc.ca
Chip
-
Good info Chip,
With intent understood it makes for easier acceptance.
Wonder if it will be automaticaly added to the lathe screen later on.
Maybe it should be an "option" to implement via configuration.
RICH
-
Hi, Rich
The Abnormal Condition Button was added over a year ago, Mach3 R1.90.091
would be nice to have a complete list of what sets it off.
You could add the Button to the lathe .Lset screen set with Screen4.
Chip
-
Thanks for all that insight. Now that I understand it I guess it makes some (very limited) sense why it's activated in my particular program when nothing else has ever done it.(in my limited experience).
So now I'll ignore it.
I am now beginning to be suspicious about my installation of Mach on this test laptop. The code presented sometimes loads and comes up with an error about "the start of an arc is not consistent with the end point" (something like that). Then the program sits on the bad line of code and nothing works. The only way to get rid of the error seems to be to clear the code and shut down Mach and restart it and then the code usually loads and runs fine.
This and the other "abnormal condition errors" seem to come and go. Some other strange things as well. Only on this program.
I noticed tonight that the code loads and runs fine on my actual CNC setup. No flashing lights or hangups.
Has anyone tried my program to see if it triggers any of these problems?
Sage
-
Hi, Sage
If your IJ's Mode isn't configured properly, You will get this type of error.
People and Programed G-Code leave Mach in the last state Run.
Preambles need to be put in the top of your code to set Mach to interpret/read the code.
Do some reading on G90, G91, G90.1 and G91.1, These are some of the settings used to set Mach in a correct State.
Chip
-
Ok I'll do some reading. RTFM as they say. Since you say it saves the previous state this may explain why it could load fine sometimes and complains at other times (for me anyway) after runnning some other program in between. But it doesn't really (I don't think) explain why loading it multiple times in a row it can load once bad an the next time fine.
I posted the code at the beginning of this thread. Would you have any specific suggestion what should be set up to ensure proper loading?
It's a simple program. I can't see any possibly confusing parts.
Sage
-
Sage,
My take on it and using your code example.
Mach knows that my machine when started will always be in absolute distance mode.
Load a program and you now are doing incremental moves. Stay with me.
If an operator, and say just the same program over and over, Mach flags to the operator,
"somethinig wrong, see your supervisor".
Now a different analogy, just me and i now that things are fine, so don't bother me Mach.
---------------------------
I mentioned the lathe, because, sometimes i'm changing all kinds of settings for whatever reason.
Should i decide to actualy do some cutting, I'm always going in to the settings and rechecking my configuraton.
So in light of the above, and if i can come around to trusting it, it could be of real value.
RICH
-
Hi, Sage
Things can be aggravating at times, Looking at your G-code, If you Stop part way through the code you can get stuck in G91 Inc Mode, Giving Errors when re-starting or re-loading the Same G-code.
Try adding this code in the top of your G-code.
(Program to make Howell Lifter Bushings - Sheet25)
(Climb Milling)
(#14 Drill to suit 3/16 reamer)
(Mill with 1/8 4 flute center cutting mill)
(Resets Mach3 to a Default Mode)
G80 ; Pre-Amb Code Set Cancel Can-Cyc Mode
G20 ; Pre-Amb Code Set INCH Unit Mode
G90 ; Pre-Amb Code Set ABS Mode
G91.1 ; Pre-Amb Code Set IJ Inc Mode
(#14 Pre-drill for Reamer)
M5 M9
G0 Z0.1000
Chip
-
Chip:
Between what you and Rich wrote the light suddenly went on. When troubleshooting the program I quite often stop it right in the middle and go to edit code then go back to try again. I can see now that doing that can be a problem. I think I usually have some pre-amble code at the beginning as I usually adopt code from LazyCam which does generate some. This time (and becasue I'm actually leaning a bit) I just used LazyCam to get the geometry and wrote the rest myself.
From now on I'll pay better attention to the pre-amble code. Thanks.
This begs another comment though. I would have thought that Mach should clear everything back to some pre-set configuration parameters when you clear the G-code and reload a new program, OR at the minimum when you clear the code and specifically push the reset button or something like that. This does not appear to be the case. I tried all that.
So unless you have endless pre-amble code to cover every possible setting that could have been manipulated by another program, how do you ever return to a fresh start condition? I'm not even sure re-starting Mach clears some stuff. Maybe I missed something in the configuration.
Sage
-
Go up a few posts and look at the graphic. Where it has the G80, add G90 and anything else you might need and then check box above that says "use INIT string on all resets". That should do the trick. Mine, for example has G80 G90 G49 G0
HTH
Mark
-
Ok Chip,
Now you got me taking a peek at the Wiki and screen designer stuff. :)
Think I'll just pack my suitcase for a short stay on this journey! ;D
RICH
-
Think I'll just pack my suitcase for a short stay on this journey! ;D
RICH
Good luck with that. You better pack two. ;)
-
Hi, Sage, Rich, Mark & All
As Mark stated it, It will work fine.
But it won't allow you to use G90, G91.1 or G9...'s on the same line in the Initialization String, only re-sets the G91.1.
Not trying to complicated setting in Mach3 for New User's Hear,!!!
Hears a Macro to use in the Ini-String Line, I think it will Re-Set Most Situations that we can get into with G-code.
' ( M1111.M1S Macro )
' ( Needs to be installed in C:\Mach3\Macros\Mach3Mill Folder)
' ( Basic Default Location or as needed )
' ( Change it as your need )
' ( For MM Units Replace G20 with G21 )
' ( For CV Mode Replace G61 with G64 )
Code "G17" ' Set X,Y Plane
Code "G20" ' Set INCH Units Mode, MM "G21"
Code "G40" ' Cancle Cutter Radius Comp.
Code "G49" ' Cancle Tool Length Offset
Code "G50" ' Re-Set All Scale Factors To 1.0
Code "G61" ' Set Exact Stop Mode, CV "G64"
Code "G69" ' Cancel G68 Rotate Coordinate System
Code "G80" ' Cancle Canned Cycle Mode
Code "G90" ' Set ABS Mode
Code "G91.1" ' Set IJ's INC Mode
Code "G94" ' Set Feed Per Minute Mode
Code "G52 x0 y0 z0" ' Re-Set Temp Offset Mode
Code "F10" ' Set Default F Speed To 10
Code "M30" ' Program End and Rewind G-Code
Just a Beginner, Compared to So-So Many Great People Hear.
Chip
Edit: Changed the Execution Order a bit, Tested it some more, Using ver 3.042.015, Let Me Know what you find.
-
Great work guys. Being a rookie I do all kinds of sins starting and stopping not so good Gcode in order to perfect my programs. I've seen some strange things happen. I usually just restart everthing to get out of the situation. SOmetimes it works , sometimes it doesn't fully help.
It looks like this macro should make things more predictable. I'll give it a try.
Keep the improvements coming. I'm learning all the time.
Thanks
Sage
-
Thanks Chip,
When someone reads the manual ( sure..... Rich, shows you have read every page ;D ), like the definition shown on page 5-21, I wonder how many people will comprehend the impact of what they read and only remember that all works so leave it unchecked. In fact this probably applies to a lot of the boxes, until, something more is needed, added, or someone asks a simple question. With all the screens and boxes your eye becomes "blind" to the print. So because of you all, this thread has been very informative.
RICH
PS: Maybe we should pick a box a week and post a question around it?
-
PS: Maybe we should pick a box a week and post a question around it?
Good idea Rich. ;)
Brett