Tuesday 16 May 2017

Tool setting saga - getting there...

This is starting to do my cake in. The guy(s) who designed / wrote the controls knew what they wanted to achieve and they knew how to set the system up when they wrote the manual (in Chinese) but without someone to show you, it's a nightmare to figure out.

It seems I have a solution finally. To my mind, the requirements for a usable arrangement are:

  • Must be able to set up a tool table, so that the program can call up the different tools - and once loaded into the spindle (they will have to be changed over manually between operations on my machine), the tool lengths should be correct (read from the table) without having to touch them off again.
  • I don't want to be having to write lengths and coordinates down from the screen and type them into another page by hand. I want this to be semi automated. 
  • The "tool setting" macros need to be understood well enough to do much of the touching off. It would be too damned annoying to know they are there but not have a clue how to use them.
  • When a new tool is loaded or a cutter is changed in a tool holder, I want to be able to set it up easily, working to the same coordinates as the existing tools.
  • Ideally I will be able to use some form of master tool - and ideally a tool setting device with electrical contacts. I suppose a simple microswitch might do. Although I have a Renishaw probe, I suspect it is too large to fit in the spindle and in my current state of ignorance and newbyness, it wouldn't last very long so would be best kept for later when I've grown up a bit.
The method that seems to work so far for populating the tool table:
  • 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 seem to use absolute values. The box at the top of the display should 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.
  • 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. 
  • 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.
  • Now physically remove Tool 1 (T01) from the machine and load Tool 2 (T02) in its place, then select it in the system by issuing G43 T02H02. 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 is the tool length you now 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.
  • Check you have got sensible values by swapping the tools back and forth and issuing the appropriate G43 instructions. 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 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. If you have managed to get it working as described, you are getting there....

No comments:

Post a Comment

Final assembly and test of the spindle nose adaptor - RESULT!!

After the recent distraction caused by the 3D scanner, resurrecting the 3D printer and buggering about with the throttle bodies for my Honda...