LinuxCNC stopping/freezes at G1 code but G1 works via MDI

More
01 Oct 2017 01:11 #99710 by lrsmith
I'm trying to setup a Sherline Mill using LinuxCNC and I have a pretty simple program that should work but everytime I run it, it hits the G1 code and just stops, still running but doesn't do anything. If I go through the MDI and enter the Gcode one at a time it works. I'm on LinuxCNC 2.7.11

The initial Gcode is below and it will hit line N21 and then just stop there and not continue.

%
(1001)
N10 G7
N11 G18
N12 G90
N13 G20

(PROFILE)
N14 T1 M6 G43
N15 G54
N16 G97 S500 M4
N17 G95
N18 G90 G0 X2.05 Z0.2656

N19 G0 Z-1.434
N20 X1.41

N21 G1 X1.25 F10
N22 X1.17
N23 Z0.
N24 X1.2831 Z0.0566

N25 G0 X1.33
.....

Please Log in or Create an account to join the conversation.

More
01 Oct 2017 04:28 #99721 by rodw
I'm only a novice but it looks like N20 is missing a G code. Should this
N20 X1.41
Be something like
N20 G1 X1.41?

Please Log in or Create an account to join the conversation.

More
01 Oct 2017 16:14 #99737 by lrsmith
It should still be in 'G1 mode' and do a move at feed-rate from line N21. I did try this as in, typing each line in on the MDI command it it behaved as expected. It should return an error if the g-code is bad but it loads, and runs up to that point and doesn't throw any errors,warnings, etc. It just hits line N21 and seems to freeze/stop.

But I was wondering that and I did modify the code and explicitly added the G1 commands and passed in the F parameter to each but it still behaved the same way, stopping at line N21.

I also tried stepping through each line, rather than run it all at once. It gets up to N21 and I cannot step past it, again no errors, warnings or any other messages

Please Log in or Create an account to join the conversation.

More
02 Oct 2017 00:30 - 02 Oct 2017 00:33 #99756 by jmelson
Do you have limit or home switches on the machine? Did you home the axes? If not, then you can have a random machine position left over from previous use of the machine. if that random position is near the soft limits, it will not go past that position. You SHOULD get a warning, right as you press R, that some limit is exceeded. But, it is possible for that dialog box to end up BEHIND the main Axis screen. I'm just guessing, as I have never seen this behavior, except in relation to the soft limits.

Oh, one other possibility is there is some odd character in the G-code file that is being interpreted as an end of file.
You can use the od program to see the binary character codes in a file.

So, do :

od -c <g-code file name>

and see if there are any odd characters near the N20 line.

Jon
Last edit: 02 Oct 2017 00:33 by jmelson.

Please Log in or Create an account to join the conversation.

More
02 Oct 2017 03:15 #99759 by lrsmith
Jon,

I'm using it with a standard Sherline Lathe, so no limit switches, etc. I did home all the axes and selected the Sherline lathe from the HAL setup. I didn't think to check for invisible chars I'll give that a check.

Thanks
Len

Please Log in or Create an account to join the conversation.

More
03 Oct 2017 22:17 - 03 Oct 2017 22:18 #99871 by andypugh
G95 (feed per rev) mode is active. That is typical for a lathe, but won't move at all without a spindle encoder.
Last edit: 03 Oct 2017 22:18 by andypugh.
The following user(s) said Thank You: lrsmith

Please Log in or Create an account to join the conversation.

More
06 Oct 2017 17:42 #100020 by lrsmith
It was indeed the G95 code. Thank you

Please Log in or Create an account to join the conversation.

Moderators: Skullworks
Time to create page: 0.114 seconds
Powered by Kunena Forum