Broke tool T1 - Need offsets remeasure. Knee mill. Ref tool F1/F2 question.

I broke tool-1 T1 in my setup. (DCAIO, few years old software). All my tools (10 or so) are listed w/ F2 offset measurements to the Ref tool. Do I just mount the ref tool to the original spot on the top of the vise, then load T1 and hit F2? I do not want to re-measure all...Just T1. I Also know the Knee is not in the same place... Sorry this keeps messing with my Mind.

if you already have tools setup in the tool library by using a reference tool following the procedure in the video...
and now you break a tool.. all you have to do is remeasure the new replacement tool against the reference tool.

1.) load the reference tool in the spindle, touch off the reference position. (i like to use top of the table or top of the vise)
2.) in the tool library, press "F1 REF" and then F10 to set the reference position. (all this does is tell the control to remember this position)
3.) load the new tool in the spindle, touch off the same position that you just used the reference tool to touch in step 2, then navigate to the tool # being used height offset and press "F2 Measure" this simply measure the extra distance traveled with the new tool compared to the reference tool to touch the same spot.
4.) the new height offset value will now be in the "H" value for the tool you are resetting, press F10 to save the changes. and you have just reset a tool height offset value.

all the other tools that were previously measured using the reference tool are still good, no need to remeasure them. you only have to remeasure just the new tool(s) against the reference tool.

when running a job for the first time or after resetting a tool(s), ALWAYS perform the "reality check" i mention in the video. and press feed hold during the first Z move down towards the work piece and look at the information on the screen ask yourself "does this make sense" the DRO will tell you how far above Z0 the control thinks the tool is.. so take a look.. is the tool really that far away from Z0? if not, double check part zero Z position and Tool Height offset values. If it does look good press cycle start to continue..

OK... So you confirmed my steps. I do need to F1 the Ref tool again, then F2 on the new Tool. Got it.

LOVE this tip btw/ "does this make sense" the DRO will tell you how far above Z0 the control thinks the tool is.. so take a look.. is the tool really that far away from Z0? if not, double check part zero Z position and Tool Height offset values. If it does look good press cycle start to continue..

sorry.. .posted too soon, What continually blows my mind is that I know my knee is set roughly near the spot I did the original 8 tool measures from. Say around a 1/2" off from where I set the original 8 or so tools in the library.

• If the Knee is close but different for this 1 T-1 tool re-measurement, the Z offset value for both F1 (ref) and F2 T1 measure would be new values (right?).
• To me .. (as confused): Thus new Z value w/ the Ref tool installed and new knee spot includes the difference (+/- .5") to the top of the vise as I move Z around.
• As soon as I press F10 I save this difference. (in my mind).
• and B) Then, onto T1 tool measure: z offset value for Tool1 when I measure and F2 /F10 it is also now different by up to a value of +/- .5" from the other 7?
• What happens with the 7 other tools that I did not do an F2 upon?

Maybe this is all dependent on a Knee scale to place it to the same spot for a measure? Sorry guys! trying here. I am going to go pop in the ref tool, and play w/ T1 in the shop over the next 10mins and see what happens. Maybe this is all just doing and watching. . . (gee what a concept...).
:confused:

Assuming you are using the usual knee mill procedure, measuring tools compared to a dedicated reference tool:
If you move the knee, then go to measure or re-measure one or more of your tools, then the Z Reference position (set with F1) will probably be different, but the resulting tool offset measurements (measured with F2) will be the same, except to the extent that the measured tool has actually gotten longer or shorter (e.g. because it was broken and replaced with one that is a different length).

The value of a measured tool height offset is the difference in length between the reference tool and the measured tool.

If T1 is 1/2" shorter than the reference tool, then when you set Z Reference on some surface somewhere, and then measure H1 on that same surface, you will get a height offset of -0.500. It doesn't make any difference what surface you use, or where the knee happens to be, as long as you set Z Reference using the reference tool immediately before you measure T1.

It definitely sounds like you are getting things confused. Hopefully, I can shed some light on the situation.

When creating the tool offsets in the Tool Offset library, all of the height offset values are the difference between the tool and the Z Reference value. The Z Reference can be set using either a "reference tool" or it could also be set to a definitive position on the machine that will never change location such as Z home. Z Reference needs to be set in order to determine the difference between the height of the tool that it's currently measuring and the Z Reference location. The only time that the Z Reference value is ever used is in the Tool Offset library. When running a program, whatever tool you call out in your program, the CNC software will automatically adjust between the differences in the height of those tools.

Now, I will use some values to see if I can make the point that I am making a little easier to grasp. Let's say that I am using a "reference tool" which when installed into the spindle has a distance of 5" from the Z home position. That means that Z Ref in the Tool Offset library is set to 5". The value that is displayed for Z Ref in the Tool Offset value may change based on what WCS you are in and where Part 0 is setup. That means that if the CNC software is in WCS #1 which had a Part 0 set for the Z axis at 6" from Z home the value displayed for Z Ref when you are in WCS #1 will be -1". Hope that clears up any issues with the value that you may see for Z Ref. If not, you can always press ALT+D at the main screen and the CNC software will switch to Machine coordinates which places all of the values on the DRO to the true location of where the machine is at. Perhaps that might make this a little easier to understand.

Now that Z Reference has been set, we can start measuring your tool offsets for your library. Let's say that we are going to be setting 3 tools in addition to your "reference tool". Of course, since you are using a reference tool, which we will call it Tool #1, the height offset for that tool is 0". Let's say that Tool #2 when installed onto the spindle goes down to a distance of 6". That means that the height offset for Tool #2 is -1". Let's say that Tool #3 when installed onto the spindle goes down to a distance of 4". That means that the height offset for Tool #3 is 1". Let's say that Tool #4 when installed onto the spindle goes down to a distance of 7". That means that the height offset for Tool #4 is -2". If you had more tools that you wanted in your library, you would continue on with the same process.

Now that all of the tools in your library are set with their height offsets, it's time to run a program. The first thing you will do is set Part 0. When you set Part 0 for the Z axis, the CNC software asks you which tool you are using so that it will now which tool to reference the height offsets in the rest of the program. Let's say you used Tool #2 at the beginning of your program and that was the tool that you used to set Part 0 for the Z axis. Then your program has a tool change in it which calls out Tool #3. The CNC software recognizes that the height difference between Tool #2 and Tool #3 is 2" and will automatically adjust your offsets for that difference. Then later on in the program, it calls out Tool #4. The CNC software recognizes that the height difference between Tool #3 and Tool #4 is 3" and it will automatically adjust your offsets for that difference.

Please let me know if are confused up to this point. If not, then we can continue on. The problem that arises with your type of machine is that the knee moves up and down and has the potential of not being at the previous height. With that type of scenario, if you have a broken tool and you need to remeasure the new height offset for that tool, the knee needs to be at the same exact location that it was at whenever you measured the Z Reference. If it's not, the height offset for the new tool will be correct because you measured it with a newly set Z Reference but if your program calls out any of the other tools, which were not remeasured, they will be off by the amount that the knee is off from the original time that Z Reference was measured. Another option would be not to redo the Z Reference but then the height offset for your new tool will not coincide with the measurement for the other tools because your knee is off.

With your type of machine, in order to make life a lot easier for you, especially in the future when you want to add new tool height offsets, it would be better to either mark the machine with the location of the knee when you set your Z Reference or have the Z Reference set to a definitive location which never changes like your Z home position. If you do the latter, everything will work out for you. The only difference is that your tool height offsets are going to be very large values because they will be the distance from home to the location of the Z axis where your tool touches the table or TT1.

I hope I have explained this in a manner that is understandable. I know that I was throwing a lot of information and values out there. Let me know if you are confused on any of those points that I made and I will do my best to clear your confusion.

If you maintain a dedicated Reference Tool, it is not necessary to return the knee to any particular position before measuring more tools.

It is only necessary to use the Reference Tool to set a new Z Reference, on whatever surface you want to use, prior to measuring tools.

Z Reference is the Z axis position where the Reference Tool touches the measuring surface.

When you touch a new tool to that same measuring surface, the Z axis may be higher or lower: higher if the tool is longer than the Reference Tool; lower if the tool is shorter than the Reference Tool.

The height offset for a measured tool need to be equal to the difference in length between that tool and the Reference Tool.

When you press F2 to measure the height offset of a new tool which you have brought down to touch the measuring surface, the control calculates the difference between the Z axis position at that moment, and the Z axis position which was previously stored as Z Reference. If the tool to be measured is longer, Z will now be higher, and the offset will be positive. If the tool to be measured is shorter, Z will now be lower, and the offset will be negative.

Perhaps this illustration will help:
http://www.cncsnw.com/ToolHeightKneeMill.PDF

I would like to apologize as I am incorrect in the following statement that I had made.

Now that all of the tools in your library are set with their height offsets, it's time to run a program. The first thing you will do is set Part 0. When you set Part 0 for the Z axis, the CNC software asks you which tool you are using so that it will now which tool to reference the height offsets in the rest of the program. Let's say you used Tool #2 at the beginning of your program and that was the tool that you used to set Part 0 for the Z axis. Then your program has a tool change in it which calls out Tool #3. The CNC software recognizes that the height difference between Tool #2 and Tool #3 is 2" and will automatically adjust your offsets for that difference. Then later on in the program, it calls out Tool #4. The CNC software recognizes that the height difference between Tool #3 and Tool #4 is 3" and it will automatically adjust your offsets for that difference.

I read the comments from cncsnw as well as looked at his illustration and he is exactly correct on the functionality of the Centroid software concerning the tool height offset. After re-reading the post, I realized what I had written which was incorrect and wasn't what I was wanting to say. I am going to chalk that up to a senior moment on my part. If the illustration that cncsnw sent is still confusing, I did find an amazing tutorial video on YouTube https://www.youtube.com/watch?v=iJcq_G8yRdc which may enlighten this issue.