Machsupport Forum
Third party software and hardware support forums. => Newfangled Solutions Mach3 Wizards => Topic started by: radioactive on May 23, 2009, 11:52:27 AM
-
While cutting a circle (0.86" diameter, 1" deep, spiraling downward toolpath) the tool moves along great except it pauses very briefly each time it crosses the X axis. Why does it do this? It does the same thing when I am cutting external threads on the same part. ???
I'm using the NFS wizards to create the toolpaths (2.83 I think) and version 3.042 of Mach 3.
-
Have you checked your backlash for the X and Y?
Brett
-
No, I haven't done that yet. I'll try to get that done this afternoon.
I don't think that is the issue because I seem to recall cutting a different part a few weeks ago where it didn't pause like this.
-
CV mode?
-
CV mode?
Me think also.
-
Show your code.
-
It appears as though I have 0.002" of backlash on the Y axis. X and Z were about 0.0004 and 0.0001.
Here's a tidbit from the code for the finish pass of the circle that pauses at the X axis each time.
(***** Circular Groove/Cutout *****)
M6 T3
M03 S4000
M9
G00G43 H3 Z0.1
G00 X0.805 Y0.1875
G41 P0.125
G01 X0.6175 F25
G03 X0.43 Y0 R0.1875
F25
G02 X-0.43 Y0 R0.43 Z-0.025
X0.43 Y0 R0.43 Z-0.05
X-0.43 Y0 R0.43 Z-0.075
X0.43 Y0 R0.43 Z-0.1
X-0.43 Y0 R0.43 Z-0.125
X0.43 Y0 R0.43 Z-0.15
X-0.43 Y0 R0.43 Z-0.175
X0.43 Y0 R0.43 Z-0.2
X-0.43 Y0 R0.43 Z-0.225
X0.43 Y0 R0.43 Z-0.25
X-0.43 Y0 R0.43 Z-0.275
X0.43 Y0 R0.43 Z-0.3
X-0.43 Y0 R0.43 Z-0.325
X0.43 Y0 R0.43 Z-0.35
X-0.43 Y0 R0.43 Z-0.375
X0.43 Y0 R0.43 Z-0.4
X-0.43 Y0 R0.43 Z-0.425
X0.43 Y0 R0.43 Z-0.45
X-0.43 Y0 R0.43 Z-0.475
X0.43 Y0 R0.43 Z-0.5
X-0.43 Y0 R0.43 Z-0.525
X0.43 Y0 R0.43 Z-0.55
X-0.43 Y0 R0.43 Z-0.575
X0.43 Y0 R0.43 Z-0.6
X-0.43 Y0 R0.43 Z-0.625
X0.43 Y0 R0.43 Z-0.65
X-0.43 Y0 R0.43 Z-0.6625
X0.43 Y0 R0.43 Z-0.675
X-0.43 Y0 R0.43
X0.43 Y0 R0.43
G00 Z0.1
G03 X0.6175 Y-0.1875 R0.1875
G40
G00 X0.805 Y-0.1875
-
See if some of the settings in this file help.
-
Do you have backlash compensation turned on?
-
ALso make sure you are running in CV mode(G64) not exact stop mode(G61). The wizard tends to assume you are in the correct modes(;-)
Just a thought, (;-) TP
-
No backlash comp is not on, I didn't think that a smoothstepper board supported this?
I'll check on the CV mode today (I think it is, but will check again)...
-
You never said you were using a SS. :)
-
Your right I didn't mention that.
I just checked and it is in CV mode.
The problem is occurring when the circle cut crosses the X axis so the Y axis isn't changing directions at this point and shouldn't be the problem.
-
Leave CV on, but turn off Distance and Feedrate on the settings page and uncheck all the options in General Config.
-
thanks I'll give it a try in about 60 secs, running a part right now
-
Distance and feedrate were unchecked on the settings tab. I cleared out the two options checked below under CV control and it still pauses as it crosses the X axis? Now what?
(http://i94.photobucket.com/albums/l110/jdnedde/Mill/config.jpg)
-
You have the Exact Stop checked!
Check the Constant Velocity instead. Make sure you don't have any G61 in your g-code.
-
What is the feed rate setting under the settings tab? And is it active?
-
Not sure why? I just went in and looked again and it is on CV (not Exact), I could of swore it was before as well??? No G61 is used in the code I'm running. Here's what the settings tab looks like... I'll try running it again and see what happens...
(http://i94.photobucket.com/albums/l110/jdnedde/Mill/setting.jpg)
-
Well it's working fine now. Somehow I got on Exact stop mode??? Will this setting change based upon a command in gcode? I'm guessing one of my other programs is doing this...
-
Yep, if you have a G61 in your G-code, then you find yourself in Exact Stop Mode.
-
Thanks for the help guys...