Wierd tool offset issue <resolved, set tool # when setting Z 0>

[GDawson]

Good Afternoon,
We are running a CNC router with an acorn control and by and large it works excellent with one rather annoying quirk.. it often tells us we have a z axis over travel alarm when starting or restarting programs, when you look at the tool offsets they are correct, and when you look at the machine zero it also looks right, but it often sees any positive movement on the z as an overtravel event (router is set up as z home is 0 and all z movements are negative, tool offsets are all negative depending on the length of the tool and the thickness of the work, work offset is top of the work =0) so whats wierd is it sometimes runs no issue, sometimes z over travel, when this happens opening tool offsets tends to change your z to the tool one offset then you close out and re zero your z and its good.. so it acts like it is remembering an old offset and ignoring the current program and current zero, all very strange, any ideas?
Thanks in advance,
Greg

[grossmsj]

G43
I'm floundering through this as well. As I understand it, you need to be sure that CNC12 knows the proper tool offset when you set zero.
At the top of the screen you'll see either T1 H-, or T1 H1 if you are using tool 1.
In the first case (T1 H1) the distance from machine home zero plus the tool offset is used to calculate part zero. So if your tool offset is 3 inches and part zero is 4 inches below the bit, you have a proper zero 7 inches below the machine home zero.
If you set zero when CNC12 shows T1 H- it doesn't know the proper tool offset (H1). It will use 0 as the tool offset. So your part zero will be calculated as being 7 inches below machine home zero (the 3 inch tool height and the 4 inches to part zero). When the program runs and it encounters the line assigning the tool height offset (G43 line), it will be calculated as an additional 3 inches below that and is effectively beyond the z-travel distance.
If I see T1 H- when I'm setting zero I need to first open MDI and type G43 H1 to tell CNC12 to use the proper tool height offset.

edit: I'll add that I just don't understand why CNC12 doesn't know to use H1 if it knows T1 is present. I know I'm doing something wrong. I only know the fix, but don't know how to keep it from happening. I am using an ATC. I never had this problem before the ATC, so it's related to the tool change part of the G-Code.

[cnckeith]

Greg,
Hello.
can you post a fresh report.zip so we can see how the cnc controller is setup?
and a copy of the g code program you are running when experiencing the travel limit issue.
is the machine setup to home out on switches?
are you using a 3rd party app or custom tool change macro?
does the machine have a tool changer?
what method of tool measurement are you using? see this post. viewtopic.php?p=83490#p83490

[cnckeith]

we added a set tool number macro to the Router VCP as a stock button for upcoming v5.1. Not for ATC use!
if you want to use it now, you can add it to your VCP here is how.

download set_tool_number.zip, copy to c:\cncm\resources\vcp\buttons and unzip.

download set_tool_number.cnc and copy to c:\cncm\system

edit your VCP skin and add this line to add the button.

<button row="6" column="1">set_tool_number</button>

[cnckeith]

do you guys maintain a tool library? i.e. do you measure tool lengths and keep a offset library? OR are you just resetting z zero for each tool?

[cnckeith]

related reading
viewtopic.php?f=60&t=4686

and

https://centroidcncforum.com/viewtopic.php?f=63&t=1493

[tblough]

edit: I'll add that I just don't understand why CNC12 doesn't know to use H1 if it knows T1 is present.

Because you don't have to use H1 with T1. You can use H12, or H93, or any other height offset with ANY tool. This lets you do rough and finish passes with the same code by calling a different offset, or machining to depth in steps by using multiple offsets.

You also don't have to use D1 with T1 either. You can use different or multiple diameter offsets with any tool as well. Granted, these are advanced concepts and most users keep the tool number and height/diameter offsets matched, but it is important to know that it is not a requirement.

[grossmsj]

do you guys maintain a tool library? i.e. do you measure tool lengths and keep a offset library? OR are you just resetting z zero for each tool?

I'm using Swissi's Probe App for ATC Keith. I measure all the tools in the tool holders using my TT-4 before each job. I actually don't know if this also sets the tool offsets in the tool library.

Because you don't have to use H1 with T1. You can use H12, or H93, or any other height offset with ANY tool. This lets you do rough and finish passes with the same code by calling a different offset, or machining to depth in steps by using multiple offsets.

Good point Tom. That would be the plainest explanation, and I do believe I've read this in the past. I'm not at the level to take advantage of things like this. It most translates into plunging a bit through the table.

[cnckeith]

do you guys maintain a tool library? i.e. do you measure tool lengths and keep a offset library? OR are you just resetting z zero for each tool?

I'm using Swissi's Probe App for ATC Keith. I measure all the tools in the tool holders using my TT-4 before each job. I actually don't know if this also sets the tool offsets in the tool library.

Because you don't have to use H1 with T1. You can use H12, or H93, or any other height offset with ANY tool. This lets you do rough and finish passes with the same code by calling a different offset, or machining to depth in steps by using multiple offsets.

Good point Tom. That would be the plainest explanation, and I do believe I've read this in the past. I'm not at the level to take advantage of things like this. It most translates into plunging a bit through the table.

does your machine home out to a home switch?
is the TT permanently mounted (always at same z location)?

[grossmsj]

does your machine home out to a home switch?
is the TT permanently mounted (always at same z location)?
[/quote]

Yes, all axes home to home switches. Yes, the TT has its own return position. Where this gets problematic for me is I have a machine table zero, and a rotary system zero. And I will switch between table and rotary interchangeably almost every day. So this is a recurring problem of resetting zeros with the G43 Kabuki dance.