The Mighty Shiz: Tool setup for Y axis bracket

With the CAM work largely complete, the next step is to set up and measure the tools in their holders, update the tool library in Fusion with the key dimensions and set the tool length offsets in the CNC controller.

The first bit is fairly simple. I've already created toolholders for most of the tools I'm likely to use - a mixture of ER40 collet chucks, keyless drill chucks and Weldon style end mill holders. From the tool setup sheet, it's simple enough to identify the tools and holders required, mount the tools and measure up the stickout of the tool from the holder / chuck etc.

Setting the tools:

As I need 4 drills in this operation and have only 3 chucks, I'll use one of the ER40 collet chucks to hold the largest (10mm) drill. I also need an ER40 collet chuck to hold the 12.7mm chamfer mill. The 10mm long series end mill can use a Weldon style holder, as with the 6mm slot drill.

The ER40 collet chucks allowed me to make use of The Startled Man in anger:

Setting up the tool library:

I had to model up the 2 new 13mm keyless chucks I got from APT recently - by modifying a copy of the slightly different 16mm keyless chuck I got from Arc Euro. It's simple and quick in the Fusion tool library.

Finally, you select the toolholder and tool, editing the tool dimensions etc to suit the particular tool ie diameter and stickout. This is actually the face mill:

The feeds and speeds are taken care of in the tool library too. A good starting point is the manufacturer's cutting data for the tool itself. But this may be rather aggressive if it's targetted at modern high speed, high power machines, so it's probably sensible to sanity check what you end up with by cross checking with other sites.

When the tool is used by Fusion CAM to generate toolpaths, it uses these tool library settings to determine the spindle speed, feed per tooth etc etc. So it's rather sensible to get them right.

You can frig the settings manually on the machine if things are getting a bit too exciting by using the manual overrides for spindle speed and feed rate but if you changed one without the other, you could get some odd chip loads going on.

Setting up the tool length offsets etc in the CNC controller;

Obviously I'd forgotten the procedure for automatically setting the tool length offsets in the controller. It's sort of documented on this blog back in 14-16 May this year but this is the procedure, with a couple of additional observations I made last night after struggling initially.

Procedure for automatically setting the tool length offsets in the Newker CNC controller:

Change to G53 (type G53 in the MDI and press the green Run button). This means we are working in absolute machine coordinates, not one of the G54-G59 work coordinate systems. This is because the tool table functions for transferring coordinate values use absolute values. The box at the top of the display should then show "G53".
Fit tool T01 and select it using "G43 T01H01" in the MDI. The "-H01" selects the tool height (length) in the first row - ideally it should be used exclusively with the first tool. I’ve made a reference tool for this position.
Run the M882 macro from the MDI. This touches the tool onto the electrical contact (or closes the microswitch, electric touch probe etc) and then stops the tool at that touch position.
NB: Parameters 380 and 381 are the X and Y coordinates of the position where the M882 macro is run. So, if you have picked a position for the tool setting, note the machine coordinates and enter them in 380 and 381. It’s not clear to me what 382 (Z axis for M882) is supposed to do. One day I may figure that out.
Press the "Redeem" button. Within the resulting Tool screen, the T1 row should be highlighted in yellow as a result of the G43 T01H01 command above. Now press "A" (redeem) to enter the current Z (absolute machine) coordinate into the (current) T1 position. Alternatively, if you are at the main screen, you can press "H" to get the same result. With the "H" option, you are prompted to select the tool number to "redeem" (god knows which translation software came up with that one).
NB: note again that the "A" or "H" redeem functions populate the tool length (H1 here) in the tool table with the absolute machine coordinate, which is why you need to be in G53 absolute machine coordinates. Trust me, if you are in G54 or some other work coordinate system, the redeemed value will not work for you. I spent a lot of time proving that beyond any reasonable doubt.
NB: IIRC, there is a parameter (near #380) that sets the finishing Z position after running M882. Be aware that the (correctly) redeemed parameter may actually be different to where the tool ends up.
Now physically remove Tool 1 (T01) from the machine and load the next tool (eg T02) in its place, then select it in the system by issuing G43 T02H02 etc. You don't actually need the T02 part of the command but it's helpful to do so, as T02 (row 2) will be automatically highlighted (yellow) in the tool table if it has been told Tool 2 is active. The critical part of the G43 instruction is actually the H02 (tool length 2). This tells the system that H02 tool length should be accounted for in the Z coordinate from this point.
Run M882 again. This will position Tool 2 at the touch point and hold it there. The current absolute machine coordinate of the Z axis at touchoff is the tool length you need to enter as H02 in the tool table in the next step.
As above, within the Tool screen, press "A" (redeem) to enter the current Z coordinate into the (current) T2 position. As before, the T2 row should be highlighted in yellow as a result of the G43 T02H02 command above. Alternatively, at the main screen, you can press "H" to get the same result, taking care to ensure that Tool 2 is selected for "redeeming".
You should now have 2 different values in the tool table (for Tool 1 and Tool 2). The difference between the table values should be the difference in the tool lengths.
You should now check you have got sensible values by swapping the tools back and forth and issuing the appropriate G43 instructions to let it know what tool you have loaded. The critical part is the "H01", H02" etc. The "T01", "T02" etc doesn't get involved when the tool length is inserted into the work coordinate calculation. So if you insert Tool 1, you can type "G43 H01"in the MDI and hit the Run button. If all is well, you can jog the tool down to the touch level and the display should indicate zero Z coordinate there. Then fit Tool 2 and issue "G43 H02". The displayed Z coordinate should immediately change to suit the new tool length and if you lower the tool to the touch level, it should also indicate zero Z coordinate there. That's what you need to achieve.
Note that when set up correctly (still talking G53 machine cords here), the machine coordinate at touch off has the same value as the tool length in the tool table but opposite sign. When the display Z coord says zero, the machine coord reads the same as the tool length (negative value). When the quill is at machine zero, the display reads the same as the tool length (positive value).
Now choose a convenient and different height (move the touch switch / probe to a different height) and change the coordinate system to G54 (just type G54 in the MDI and press the Run button). The main display should show "G54" in the box at the top right. Now press "Setup" and type "Z" into the dialog box - this will zero the current (G54) work coordinate system Z coordinate at the new height, as if you had touched off on a workpiece.
Now check that it is working as it should. Change to Tool 2 again and issue G43 H02. This will activate the H02 tool length and the displayed G54 Z coordinate should change (by the difference between H02 and H01). If you take the tool to the touch level, the Z coordinate should read zero correctly - with this new tool. Alternatively, if you issue a G00 X0 Y0 Z0 command, it should take the tool to the same touch off position. If you have managed to get it working as described, you are getting there....
NB: In the MDI window, you can comment out a line by entering a left bracket at the start or part way long the line. No need for a matching right bracket on that line. This allows you to type several frequent lines into MDI and select them as appropriate by adding or deleting the left bracket.

Here's how you select Tool 11 and run the M882 macro:

NB: Note that the M882 macro takes the machine to X and Y coordinates that are defined in parameters 380 and 381 respectively, so if you are doing this work in a different table position from last time, be prepared for the table to move when you run the macro. Even better if you note the machine coords and update parameters 380 and 381.

If you have a turret machine like mine, with a limited quill movement (about 150mm in my case), you need to minimise the range of total stickouts between the various tools. So if you have a short cutter in a short holder and a long tool (eg drill) in a large holder (eg chuck), you have to ensure that you can get all of the planned machining operations done within the range of movement of the quill - and this also goes for any tool setting movements.

Here's my crude tool setting device in action. The height of the pad is roughly on the same level as the top of the 1-1/2"stock to avoid the problem just noted.

To check the tool offsets look sensible, touch off one of the tools in G54 and set X, Y and Z to zero (press "Setup" button, select the axis and enter zero for each axis). Then swap each tool out one after the other, using G43 to identify the current tool and then issue G54 X0 Y0 Z0 to check the tool also touches off on the reference piece.

This is for Tool 14: