Manual tool change problem

curtisa wrote:

There are ways of getting tool length compensation going in Axis following a manual tool change, but it is a little fiddly.

The way I've done it is to add a touchplate to my mill and remap the M6 command into a subroutine to make Axis measure the length of each tool every time a tool change is performed. Method is outlined here:

forum.linuxcnc.org/forum/10-advanced-con...h-off?start=30#48235

This works even if your collet/tools isn't designed to use preset-height cutters. It just measures the length of each tool and adds or subtracts that offset from the initial touch off.

This is exactly what I have been looking for. Im currently setting up my jobs in fusion using multiple setup, therefor running a separate program for each tool change. I'll look over the thread to see If I can implement using my touch plate. Thank You!

Hello - thanks for all the replies.

I assume that the Z-axis DRO on the screen display is the actual tool tip position
If that is so, all intermediate positions of the display appear to be OK
impossible to measure or check as the tool keeps moving even with single step mode in operation
The first tool change always seems to occur at whatever level Z is set to at the start of the run
I can get around this by issuing a dummy tool change at the start of the program with the TLO set at around 2

Is it possible to set the AXIS GUI in some sort of pause mode during a run that will enable manual control (either by jogging or issuing MDI commands) and possibly using the touch-off command
I can only get it to do it by effectively killing the run - that leaves me with the problem of restarting it at the correct line - not good.

There is a definite bug in the M6 routines when different tool lengths are involved -
clicking on the tool change continue button instantly moves the display to the new tool position, but omits to move the actual mill Z-axis - the clue is in the "instantly".
It would be good to fix this, but where is the source code? I have found a load of code in github.com/LinuxCNC/linuxcnc/tree/master/docs/src/code but which is the relevant bit?
If I fix my own version, do I need to compile it? If so, how? Or do I just remap the M6?

The manual says about remapping the M6 code - "Note than when remapping an existing code, we completely disable this codes’ built in functionality of the interpreter".
Obviously if I am going to remap the M6 it would be good to see what the original version is doing so I can replicate it - another good reason to find the source code

Once that is fixed, I think there is a need for a new M6 that copes with different tool lengths.
If the headstock is moved to the new tool length (which is the case if the above bug were fixed) there is a risk of crashing the previous tool into the material (or other parts of the mill) if the new tool is shorter.

Tool change should be a 2 step operation where different tool lengths are involved -
first - move to the TLO position for current tool - remove tool
second - move to the TLO position for the new tool - fit new tool, save tool data for next tool change first stage

Parameters for the above operations appear to be -
#5400 - tool number
#5403 - Z tool offset
#5422 (also called #<_z>) - current Z position


My drills vary in length from 1.5" to 4.25", the drill chuck adapter adds a further 1.8" to that
I am doing a lot of drilling operations in the mill, hence the problem with the tool lengths

Jog & MDI appear to be inactive during M6 - this is explicitly stated for M0 & M1, but not mentioned for M6
So how do you jog (or do an MDI) in the middle of a program execution?

Do you have the ini file entry in the [EMCIO] section
eg.
TOOL_CHANGE_POSITION = 200 200 0 (x y z)
TOOL_CHANGE_QUILL_UP = 1
?

Talking about a milling machine or router
Years ago I was not really happy with M6 because of fixed toolchange position. I have collet manual toolchange, it could be done anywhere within working area. A touchplate or toolsensor is required for my solution, first setup reference tool, then setup z offset. Use g43 in gcode.
If you or someone is interrested, tell me. I need some time to modify the files for general use, need to remove some my_machine specific parts.

No - neither are set. I can't imagine why anyone would try to change a tool with the tip at Z0. Even a collet needs a bit of wiggle room (at least mine do) and a drill chuck needs even more, particularly if the drill size is near the maximum for the chuck.

I think most Linuxcncmachines have G53/machine coordinate system Z0 at the most faraway position from the table,workpiece. Very good idea to avoid crashing the machine. If you are working with toollength compensation, G43, it needs to be activated with the first z-move after toolchange. After the last move in z, toollength compensation must be deactivated with G49, for toolchange. Most machines refuse toolchange, if you don`t. That time z retracted to G53 Z0 (z+ direction), has nothing to do with the tooltip at all, it is the position of the Z-slide. then there should be enough space for your tool.
The attched picture is from the manual, Important User Concepts, 6. Machine Configurations.

My Taig mill is very small by most standards - very much Model Engineering rather than commercial
Max travel is X11, Y5, Z5 which immediately imposes contraints on what I can do
Add to that the fact that none of my tooling is fixed and can move up and down in the chucks
I have always used it with Z0 set to the top of the material, moving Z to 0.5 for tool change with a half inch block between tool tip and material
That way I adjust the tool within the chuck to suit. Changing the tool at higher altitude would be impractical as I would have no way of adjusting it relative to the material.

I have a Sieg X3 bigger but not a giant. This is what I do and it works quite well. Much of this is base on advise from this forum. Set home to be the front left corner of the table for the X & Y. Z home is with the spindle all the way up. Just a little below the upper Z limit. When I create the part in Fusion 360 I usually use the back left corner as the origin. That way I can touch off the X and Y on t he part or the fixed jaw of the vise depending on what I am making and how many I'm going to make. I put each operation in a separate file and name them PartnameSpot, PartnameDrill, PartnameMillSlot, and so on. Then I setup the material in the vised and touch off the back left corner using an edge finder. Load the file for the first operation. Put the bit in the collet/chuck. Touch off the tip of the tool to the top of the material using the touch plate I made. Then run the job. Then load the next file and tool and touch off the Z. Run the part. Just make sure there are no values other than zero in the tool table in LinuxCNC. That value would be added to the Z touch off value and for me usually resulted in cutting air.

Before I had the edge finder I would use a steel pin and eyeball when it touched the X & Y.. And before the touch plate I used the paper method on the Z Although loosening the bit and letting drop onto the part may have been more accurate.

John


When it comes time to cut the poart

Now I understand. I think you can avoid M6. In MDI Just load the desired Toolnumber, maybe T1, with M61 Q1, and touch off to material.
M61 Q1 in your gcode or whatever tool used for touch off.

For toolchange:
retract z to 0.5
M5 ,stop spindle
If desired, do a debug message (debug, change tool...)
M0 ,pause a running program temporarily
Change tool
press s on the keyboard to resume
Program S,F for the new Tool and M3 to start spindle
Do the whole job with this T number.

From what I have read doing manual tool changes using tools held in collets and chucks that are not of a fixed length does not work if your job is all in one file. You can't jog the machine to touch off during tool change prompt. That is why you use one file for each tool.

I don't worry about what the tool number is. The only thing that seems to matter is that if create a part in Fusion 360 and used 10 different tools for the job I will have 10 files and must have room for 10 tools in the tool table. It doesn't matter what the tool table says they are as long at the length is zero. I load the file, put the tool in the collet/chuck. Touch off the Z to the top of the material. Press run. The Z moves to the top and a popup comes up telling me to insert tool # whatever. I already put the tool in so I click OK. The machine performs the operation. When it finishes the Z moves back to the top. I load the next file and tool, touch off Z and press run. If the next job uses the same tool or I had hit EStop and I am restarting the same job LinuxCNC knows that the tool that is currently being used is the same as the last program run and will not prompt for the tool change. It will just go about doing the job.

John

Hello - thanks for the replies but I would rather run the complete operation in a single file with multiple tools. It would seem that I am getting confused by the display. When I turn the mill on it is actually doing something different. I made the mistake of setting tool offsets as negative values which moved the mill to the wrong height. I have now changed them to positive values which now seems to give the correct distance between relative tool tips as judged by the change in tone as the Z-axis switches from rapid to slow feed rates at 0.118" above the theoretical material (no actual material or tool in the mill yet) - measured with tape measure from bottom of headstock to bed, so only approximate values. All well and good, the only problem now is that it is trying to do the tool change way below the material level! I must have something configured wrong, but what? attached are my .ini file, a sample test program and the tool table (renamed with a .txt extension as this will not allow me to attach a .tbl file).
I am now intending to set the tool change at the top of the Z-axis slide (it already does if the tool offsets are negative) and make sure that all drills are seated hard against the top of the tool chuck (which will give them a pedictable length), end mills will have to have a collar Loctited to them to give them a predictable length when fitted in a collet chuck.
Cheers