Wierd G-codes

[OLDMAN]

Okay; here's my problem?? I'm using V-Carve Pro and have managed to design the Leaf bowl and come up with the g-code scenario. Everything works fine until it gets into the program at the finish of the rough cut program and thinks go bonkers on me. All of a sudden the router will take off in a circular motion going off of the dimensions of the material as well as the actual size of the project selected. Here are just 2 of the line codes that I read at that point: N16140G2X3.2967Y2.4682I-0.0884J-0.0084 & another line reads N16780G2X3.8081Y2.7370I0.1250J.000. Scrolling down the g-code lines there are several more such line codes. Is this something that i have done wrong or is this written into the program intentionally??? Any and ALL suggestions will be greatly appreciated.

Thanks in advance
Paul

[PaulRowntree]

Paul, those are arc commands. Vectric programs use the incremental mode for arcs, and you should make sure that your controller software (Mach3 ?) is also running them as incremental mode, not absolute.
Incremental is said to be more accurate.
I believe that you can set Mach3 to use this by default on the Settings page I believe ... it should be a check box.

Which post-processor are you using? The Mach3 Arcs PP should use incremental by default, with a G91.1 near the top of the gcode file. This tells Mach3 what mode to use, regardless of its defaults. This is a snip from the top of a Mach3 file

Code: Select all

( File created: Sunday, July 13, 2014 - 04:59 PM)
( for Mach2/3 from Vectric )
( Material Size)
( X= 25.000, Y= 7.000, Z= 0.750)
()
(Toolpaths used in this file:)
(Profile 2)
(Tools used in this file: )
(1 = End Mill {0.188 inch})
N100G00G20G17G90G40G49G80
N110G70G91.1   **************************** HERE IT IS
N120T1M06
N130 (End Mill {0.188 inch})
N140G00G43Z0.9500H1

[OLDMAN]

Okay Paul: I found what you are talking about but I have another question about this setting. Should the distance mode be set at absolute or incremental along with the IJ being incremental? when I did this on the screen the message abnormal conditions continues to flash stating of course that the IJ is not set correctly.

[PaulRowntree]

I believe that the distance mode should be absolute (G90) and the arc mode should be incremental (G91.1). If you look at the gcode I posted, the line above the 'HERE IT IS' pointer contains the G90 command.

But I don't see why this is a problem. If you are using Mach3, the Vectric Mach3 post-processors include the right settings for both the distance and arc modes, and they will override the checkboxes used to define Mach3's default behaviour. I use the Mach3 Arcs inches PP

Are you running Mach3? What post-processor are you using ? Can you post the header portion of a simple toolpath?

[OLDMAN]

Paul: Running late tonite but will try and post your request tomorrow. I am running Mach3 as my post-processor in inches. Thanks

[PaulRowntree]

OK. Just found this thread http://forum.vectric.com/viewtopic.php?f=4&t=11075 that seems to be reporting a similar issue. Post #6 reports that moving the Mach3 license file automagically fixed the problem...

[OLDMAN]

Here is the program G-code I'm running. See attachment please:

[martin54]

OK. Just found this thread http://forum.vectric.com/viewtopic.php?f=4&t=11075 that seems to be reporting a similar issue. Post #6 reports that moving the Mach3 license file automagically fixed the problem...

Paul if I have read that other post correctly then their machine was stopping because mach3 had reached the line limit set in the demo version, the licence code file has to be placed in the mach3 folder which they hadn't done.

[OLDMAN]

Thanks: I will make an attempt to do that and keep my fingers cross.

[PaulRowntree]

Martin : you are probably right ... that would make sense.

Paul : The header looks 100% normal to me. I will try to run it at home. Do you see crazy behaviour in the Mach3 toolpath window?

[OLDMAN]

No, the only thing I notice is that during operation "abnormal conditions" button is constantly flashing telling mee that the IJ is incorrect. The program runs normal as far as I can tell from end results. Maybe if I contact ARTSOFT they will explain the reason. Thanks

[PaulRowntree]

OK. I haven't seen this on my machine, but here is a/the fix. Honestly, I don't know what 'normal conditions' are for Mach3, but check reply#5 in this thread

http://www.machsupport.com/forum/index.php?topic=6957.0

Cheers!

[martin54]

OK. I haven't seen this on my machine, but here is a/the fix. Honestly, I don't know what 'normal conditions' are for Mach3, but check reply#5 in this thread

http://www.machsupport.com/forum/index.php?topic=6957.0

Cheers!

Paul, I use mach3 but have to admit to knowing almost nothing about it, one of those things where you say you will spend some time & learn more but never seem to get round to because of all the other stuff you have to learn.
How did you go about setting your machine up & where did you find the info? I know every machine is different & settings will obviously vary but there must be somewhere that gives a clue. Most of my settings are still default values, a few I have changed after reading posts on various forums.

Most disappointing thing about the latest link you posted was although there seems to be a way to turn the warning off no one has actually explained what the warning is or why it is there.

[PaulRowntree]

Sadly, I am in the same situation, exactly. I think the documentation is opaque at best. It reads like a hobby program that has gained wider acceptance; the default screen layouts reinforce this impression. I set it up by goofing around with it for a couple of hours; since it was all new to me it was kind of exciting, but this is hardly the way a commercial shop or expert would look at it. It seemed to work fine with only a few adjustments of + and - directions etc. But my machine doesn't use slaved axes, home switches (yet, still promising myself to use Ger21's 2010 screen set), or even limits. I am so afraid of changing anything that I have refused to do the upgrades over the past 3 years. With only 1-2 exceptions, errors are always my own, so I don't see much need to upgrade.

[ger21]

No, the only thing I notice is that during operation "abnormal conditions" button is constantly flashing telling mee that the IJ is incorrect.

"Abnormal Condition" is the most confusing "feature" of Mach3. It doesn't mean that it's "incorrect". It just means you've changed something after defining a "Normal" state. Just go to the Operator menu, and clicj "Set Normal State" to stop the flashing message.

The "Abnormal Condition" LED causes far more confusion than any help it might provide to anyone.

In most cases, Mach3 should be configured for Absolute motion (G90) and Incremental IJ (G91.1).

I know this is late, but it may help someone down the road.