Centroid Community CNC Support Forum

Hey all revisiting this post after a couple of months away from my Sherline build, was getting my new Tormach machine up and running I just bought.

Just did my 1st Intercon program and I'm getting another 907 X axis travel exceeded error when running the program. I never did resolve the last issue of this I had back in October as I found the Tormach and had to move on that So back to this. I have not yet successfully run a part up to this point. : (

Here is the intercon file.

What options do i have to get on the phone or better yet a Zoom with someone to get me up and running once and for all? I need to get beyond my setup issues make sure everything is set up correctly (hardware,software,wizard) and get everything working so I can burn some parts.

cnckeith wrote: ↑Mon Oct 18, 2021 2:34 pm i would

1.) manually jog the machine to "test' the work envelope (software travel limits) all four corners, to make sure it is set correctly.

2.) command the machine to move to the WCS being used in the g code program x0,z0 to verify it is as the proper location.
"G54"
G1 X0 F20
G1 Z0 F20

3.) now graph the gcode. now if you still get travel exceeded message at this point the g code program is trying to move from the zero in step 2 to outside the work envelope in step 1.

Here is where my tool 1 ends up when entering z0,x0 right were it should be.

Post a report so we can see where your WCS is relative to your machine coordinates. Also post the intercon file from the icn lathe directory.

cnckeith wrote: ↑Fri Oct 22, 2021 1:22 pm please see the operator manual for g code explanation. with a lathe you'll need to put a G98 in front of the G1 to tell cnc12 not to sync with the encoder (or turn the spindle on so it can move) https://www.centroidcnc.com/centroid_di ... -v4.20.pdf

from your description of the work envelope and WCS test (zo,x0) it sounds like you are good to go, now its time to get the part program correct.

How is it that this new program created with Intercon is having the same issue if you're suggesting its a programing and part setup issue?

here are screenshots of Intercon pr9gram settings

So, is Z+ really towards the tailstock as in your photo with the masking tape label on the headstock? If so, your tool change position is 5" into your headstock.

Also, I think your finish feedrate of 1000 inches per minute might be excessive. Try something like 5 or 10.

Other than the comment about your finish feedrate, ignore that last post of mine. Your tool change position is probably correct but we won't know for sure until you post the Intercon program and a report. With those two things and what tool number is your reference tool, I can load your report on a machine and duplicate what you have.

I am guessing that Z+ moves the tool carriage right (away from the headstock) even though the masking tape label is on the headstock.

Without a report, we can only speculate about where and how the machine is homed, and what the travel limits are.

One picture shows the G28 return point set at Z-5.0, X-3.0. That is measured from machine home. If the machine does not in fact have 5" of minus travel on Z, or 3" of minus travel on X (according to the software travel limits), then any G28 is going to cause a "907 ... travel exceeded" message.

Of course, without knowing the line number that was listed in the "907 ... axis travel exceeded" message, we can also only speculate about which move in the program is causing the problem.

Perhaps you could post a Report, and also tell us what the full text of the 907 error message is.

tblough wrote: ↑Fri Dec 31, 2021 3:53 pm Other than the comment about your finish feedrate, ignore that last post of mine. Your tool change position is probably correct but we won't know for sure until you post the Intercon program and a report. With those two things and what tool number is your reference tool, I can load your report on a machine and duplicate what you have.

I had posted the Intercon file above in my 1st post (revisiting this post) but here it is again, also the current report and screenshot of tool change position.

and by the way, every file i load and try and run isthe same result, these would be the sample files from C:\cnct\ncfiles so not my programming.

As far as the feed rate I thought I entered in 10ipm LOL, just getting used to how CNC12 does things. I will change that,

As I mentioned in a previous post the Intercon file is in the icnlathe directory. The. .cnc file is the compiled g-code. We would like the Intercon source file to help you debug.

The machine homes to switches at the plus ends of both axes.

Software travel limits are set to:
-12.700" on X (radius amount)
-8.500" on Z

WCS #18 is currently selected.
The #18 WCS origin is at:
X-12.363
Z-7.006

So, when a tool with no offsets is at part zero, it has about another -0.337" available on X (-0.674" diameter); and -1.494" available on Z.

The program calls up tool #1 (T0101).

Offsets #1 are -4.946" on X, and -0.033" on Z. So, to put Tool #1 at part zero would require moving X to -17.309" in machine coordinates, or 4.609" beyond the travel limit.

This looks like either an error setting the part zero on the X axis, or an error measuring the offsets for Tool #1.