Hey guys,
having an issue surfacing my baseplate. im getting an alarm that the machine cant travel far enough, i double checked all of my switches and travel distances and have almost an inch over the entire program. Has anyone had this issue yet? im using the 3/8 Em program.
Update, No issues with the 1/2 inch Program. seems to work fine
2 Likes
@Jpersons44 we’ll check the 3/8" program on Monday…could be an error in the code; if so we’ll fix and reupload. Glad you were able to get the 1/2" program running!
Cool thanks guys i looked throught the G code and everything looks good! but i must be missing something, super stoked on my machine although i may be needing to sand some epoxy out 
When it’s covered in chips and coolant, you can hardly notice imperfections
Mike,
You sure that got checked out? I tried doing the facing op tonight with the 3/8" post and it fails with a Machine Alarm that the G code motion target exceeds machine travel. Opened the 1/2" post and it runs fine from the same G54.
Well take a look, thanks!
We’re somewhat of a skeleton crew this week since many have taken the opportunity to enjoy some much needed time with family, etc. We’ve admittedly fallen a bit behind on tech support stuff. Back to normal next week!
3 Likes
Had this same problem, program worked after turning off soft limits. 3/8 program.
Was this ever addressed by Langmuir?
I tried running the 3/8 program today and got the same error. Don’t have a 1/2" collet so need this one to work!
@Drydoid I took a look at the 3/8" gcode and there’s a very small positive Y movement at the start of the code that is causing the issue for folks. This + movement is what throws the error because this program is ran from the machine zero position and no additional positive Y movements are allowed from machine zero. It works for some with soft-limits disabled since the movement is really small and isn’t enough to hit the limit switches in the +Y direction.
I’ve highlighted the code below that is causing the issue. It’s a simple fix, simply add a (-) symbol where shown with your favorite text editor of choice and it should run fine:
(MR-1 BASEPLATE SURFACING WITH 0.375" END MILL)
(T1 D=0.375 CR=0 - ZMIN=0 - flat end mill)
G90 G94
G17
G20
(3/8" END MILL FACING)
S7500 M3
G54
M8
G0 X0 Y0.0319 <--- add a "-" in front of this y coordinate (Y-0.0319)
G1 Z0 F65
X21.819
G17 G2 X21.819 Y-0.3003 I0 J-0.1661
Hope that helps!
PS. Edited for clarity and grammar
5 Likes
Thanks so much for posting this!
did anyone try the code adjustment? I am about to do the facing for .375.
can always run the Z high and do a dry run but it should be fine.
@bestduckingfarm Did it work ok for you? Another tool I use for gcode sanity checks is
Just copy and paste your code, or a section of it, into the window and get a quick simulation on the right. Works well for modifying Gcode to run from certain operations, etc.
1 Like
got an error when i tried to fix the program. has anybody had luck running the 3/8? i just ordered a 1/2 and will try that when it gets here.
I know this is an old thread. Changing the Y to a negative fixes the overtravel, but makes the next arc command invalid. The G2 line will have to be changed to G1 and delete the I and J address and values on that line only. This is only required on the first G2 line. The rest are ok.
Or offset G54 in the Y negative direction about .040.
Welcome to the forum.
What are you trying to do? If running the baseplate program, just run the canned Langmuir file.
No g code is required. If you have modifications outside the design, maybe some of our rocket scientists can chime in.
Hi Bigdaddy. Thanks for the welcome. I ran into a snag with the baseplate program but am past that now. I agree there is nothing wrong with their 3/8 program however the video guide instructs you to set G54 X and Y at home location. (Always a chance I missunderstood) The program has a positive Y command which causes an overtravel error. The edit suggested by arcnsparks causes the problem I described above with the first G2 arc command. I had hoped my post would help others. Have a great day.
1 Like
You just needed to turn off soft limits for the program and It runs just fine. It is intended to go in the positive direction.
1 Like