Software limits

[Ryan Patterson]

I'm trying to better understand how software limits work, and I feel like I may be running into some limitations—or perhaps I’m just not setting things up correctly. Here’s what I’m seeing:

1. Positive Software Limit Range:

It seems like the low limit must be at or below zero. On my machine, zero is at the home switch trigger point on the X-axis. I would like to set the working X range from 1" to 36", where 1" is just past the home switch. This would help avoid collisions with fixtures or a tool rack that extends into the machine's travel.

The machine still needs to reach the tool rack (which is outside the normal cutting area) for tool changes, but I’d like to prevent job files from moving into that area—unless it’s part of the tool change macro. Is there a way to define positive-only ranges or create an exclusion zone that allows motion only when explicitly commanded (e.g. via a macro)?

2. Tool Lengths vs. Software Limits (Z-Axis):

It doesn’t seem like tool length offsets are considered in the software limits. For example, if my Z-axis travels from 0 to -6", and I install a tool with a 2" offset, I’d expect the software limit to prevent motion beyond Z = -4" (i.e., accounting for the tool length to avoid a crash). But currently, it seems I can still jog to Z = -6", even with the tool offset active.

Is there a way to have software limits dynamically account for tool length offsets? Or are soft limits always based solely on the machine coordinate system, regardless of tool data?

Thanks in advance for any insight—just trying to make sure I’m understanding this correctly.

[Ken Rychlik]

On the homing, you can customize the x and or y to move an inch or whatever and reset machine home there. Then the negative 1" limit would function as desired. I change limits before a tool change and change them back after all within the m6 macro. The section below moves and resets machine home for the x for instance.
M91/X L1
G91 G1 X4 F200
M26/X

23601 changes axis one pos limit I think 23502 changes axis 2 minus limit. It should be in the manual. The last digit of the 2360x is the axis number

Mine looks like the below to change it for accessing the back tool rack.
#23602 = 68 ;Change Y + limit to move to tool change area

I don't have an answer for the z soft limit so maybe someone will chime in with that.

[Ryan Patterson]

I do understand that I could shift the X and Y more into positive to allow for the negative travel limit. More curious why this would be restricted in this way

The way you are handling the tool bar limits I suppose one could also adjust the Z limit in the tool change macro based on the tool height being set.

[cncsnw]

Software limits are intended to prevent you from moving far enough to trip the hardware limit switches; or, in the absence of limit switches, to prevent you from running beyond the machine ways or ballscrew length.

They are not intended to prevent you from crashing a tool tip into the table, or a boring far into the lathe chuck, etc..

Granted, that would be useful in some situations. But that would be a very different thing from the current software travel limit function; and for lathe controls, it would be a major can of worms.

[Ryan Patterson]

Thank you for the explanation — that makes sense and helps clarify the current intent of software limits in Acorn.

I’d like to suggest this as a potential feature for a future update or add-on. Without accounting for tool length offsets, the lower Z limit becomes less meaningful for many users. In my experience retrofitting machines with controls like Syntec, Fanuc, and ShopBot, all of these systems incorporate tool length when enforcing Z-axis limits. It’s a helpful safety layer, especially when working with automated tool changers or shared fixturing areas.

For my own projects, I believe I can work around this by dynamically updating the Z limit after each tool change, so it’s not a blocker for me personally. Just sharing this in the interest of helping make the platform even more robust for others out of the box.

Thanks again for the info and all the hard work that goes into the system!

[CentroidFrog]

Something you could look into using for tool changes is M297/M298.
M297 disables software travel limits and M298 enables software travel limits.
These are on page 298 of the mill operator manual:
https://www.centroidcnc.com/centroid_di ... manual.pdf

Be aware:
M298 is enabled by default.
M297, once called, is enable until the current job finishes, you exit MDI, or you issue an M298.
Limit and Home SWITCHES will still operate as normal.

[Ryan Patterson]

Something you could look into using for tool changes is M297/M298.
M297 disables software travel limits and M298 enables software travel limits.
These are on page 298 of the mill operator manual:
https://www.centroidcnc.com/centroid_di ... manual.pdf

Be aware:
M298 is enabled by default.
M297, once called, is enable until the current job finishes, you exit MDI, or you issue an M298.
Limit and Home SWITCHES will still operate as normal.

I think the issue may be misunderstood a little. I do not want to disable the limits. I want them to work and be updated with new tool lengths. For example, the nose of the spindle without a tool in the tool holder Z can go down -4.5 in. . So you may think that you could use a lower limit of minus 4.5. this lower limit will not protect anything once I put a tool in the tool holder. So if my tool length is 2 in. My lower limit can no longer be- 4.5. it needs to be set to -2.5.

It is going to be easy enough to adjust the limits based on tool height in a tool change macro. Just suggesting that it be a default out of the box adjustment.

[CentroidFrog]

The machine still needs to reach the tool rack (which is outside the normal cutting area) for tool changes, but I’d like to prevent job files from moving into that area—unless it’s part of the tool change macro. Is there a way to define positive-only ranges or create an exclusion zone that allows motion only when explicitly commanded (e.g. via a macro)?

Apologies if I misunderstood, I was referring to a possible solution to this.
Using M297/M298 in the tool change macro could allow a tool change to occur outside of the soft limits.
And once the tool change macro is done the soft limits can be re-enabled.
Allowing tool changes to happen outside the soft limits, while keeping job moves inside the soft limits.

[Ryan Patterson]

Thank you for the clarification and that is a good suggestion.

My apologies if I sounded ungrateful.