Green "Tool Reset" prompt, but we have no button to push for that, or a tool changer.

[tomdbiggs]

Hello to all,

I'm getting started with CNC, but if someone can help with this, I'll be on my way happily cutting parts out of 1/2" ply material.

Here's the issue:
We have an old Milltronics Controller that has been upgraded.

Machine pictured here:
http://picasaweb.google.com/lh/photo...eat=directlink

So the old console does not have a tool reset button. Instead, of hitting this button, we were told by Milltronics tech support, to hit "Alt-F8" as the workaround. This worked fine, but we were running it in Verify (F9, "Verf") mode. When we went to Run mode (F4) we got the "Cycle Start" green message, and we hit the white Cycle Start button on the ancient console. Next we got the tool change message, prompting us to change the tool and then hit the "Tool Reset" button on the console. This time, if we try the Alt-F8 workaround, it does nothing. This is puzzling since it worked for the Verify mode. Is this a setting in the Parms (for which I have full access being co-owner of our company) or is there a code related workaround. It seems like this may be something others have experienced, and if so, please tell me what you did to solve it. Also, just as a note, our machine is a 3-axis, with moveable 4'x8' bed. There is no tool changer, and no sensor indicating to the controller that the tool bit is in place or not (I'm not sure if there is such a thing, but the Milltronics guy seemed to imply this).


Also, if there is anyone from Milltronics tech support reading this, is there a way to forward me a copy of the document where keyboard functions that perform the functions of the ancient controller are located. Logically, if "Alt-F8" replaces "Tool Reset" then there should be other keyboard commands that perform other functions. If there is some kind of document floating around that goes into this in greater detail, please tell me how I can obtain a copy of it. Also, is there a guide to programming GCODE for my machine?

[dlenardu]

I'm not sure what the work around is, but first how many tools are you using per program?

If you are only running one tool then when you write the program and you do the "tool chg" hit f3 and toggle over to "tool call" then you do not have to use tool reset button. If you are using more than one tool then you may have to write a separate program for each tool. I'm sure someone else may know a better way but that will get you going for now.

[tomdbiggs]

We only use one tool, unless we have to drill holes in addition to the profiles. I managed to test the method of pushing F3 at the prompt for the tool change, but nothing happened. I hit the Estop button, and reset and tried running it after the line in the code where it asks for a tool. This seemed to be a workaround. Note: It involves hitting F1-Start, and then F2-Block, where it asks the code number (in this case N6).

This seems like a weird workaround, and I'm pretty sure the previous owner of this machine did not have the issue. Since we updated the Parameters to the default settings to solve a corrupt parameters file, I suspect we have a setting to adjust that we are not aware of.

[dlenardu]

No, you have to change the tool change to a tool call in the program itself. Are you using conversational? If so when you program your tool change, the "change" will highlight, press f3 and then it will toggle to a "call" When you do "call" it assumes that the tool is already in the machine. If you are using Gcode take the M06 or M6 out of the program line, the M6 or M06 tells the machine it needs to do a tool change as long as you have the tool in the machine before the program starts up and you are using the correct tool offsets you will be good.

[jpawelk]

Please see the attachement regarding the keyboard operations. Thank you

[tomdbiggs]

So we are using gcode not conversational. We are unable to hit F3 on our controller to make a change a call. We can try taking out the N6 "tool change" line altogether but it seems odd to do this since the previous owner used the program we are using to test the machine. But since there is no way of changing a parameter to overuse this then we turn to the gcode as the solution. Is there a way to modify line N6 to be a tool call versus a change so we are able to switch tools if we need to without calling up a new program? If not is there a line of code we may subtitute that pauses the machine so that a toolcan be switched?

[dlenardu]

You could put in a m00(program stop) and then a m05(spindle stop) then put all of your info for the next tool. then you would have to hit cycle start to resume the program after you put in the new tool.

[jpawelk]

First of all, toggling between a tool change and tool call is only in the conversational programming. If you are programming G/M code, please disregard any and all comments on this. The actual problem that you have is an incorrect tool change macro. A custom M6.prg needs to be created. The tool change macro line will need to be changed. (This is a POWER parameter) It will need to be edited so that it is B:\RAM\M6.PRG
You will need to create the new tool change macro and save it to the B:\RAM directory. (You can create this file using notepad on your pc. Then place the file into a folder named RAM onto a blank, formatted floppy disk. Take the disk and insert the floppy disk into the floppy drive. Press F10(UTIL), F3(FILES), F1(LOAD), locate the file named "parameters". Place the cursor on this and press F2(SET). (It should highlight) Then press F1(START). This will load the tool change macro to the correct location. Escape to the main and cycle power and then you will NO LONGER HAVE THIS PROBLEM!
The tool change macro needs to look just like this:

G32
M5
M0(Change the Tool)
P260=P268
P370=P268

Please let me know if you have any questions.

Jason

[Kurach]

tomdbiggs,

Hope you have the answers your looking for already but in not here is a list of "F" comands.

Using a external keyboard......
Alt F1 = Spindal off
Alt F2 = E-Stop
Alt F3 = Spindal On CW
Alt F4 = Feed Hold
Alt F5 = Spindal On CCW
Alt F6 = Cycle Start
Alt F7 = Coolant Mister (toggles off and on)
Alt F8 = ?
Alt F9 = Flood Coolant (toggles off and on)
Alt F10 Reset
Alt F11 Chip Removal

This is how it works on our machines. (VM17) & (RH20)

Hope this helps.

Respectfully,
Kurtis