MACH2自动换刀(英文)

zenyfei · 发表于 2007-12-29 16:01

Manual Automatic Tool Change
Making it all work
The statement “Manual Automatic Tool Change” sounds like an oxymoronic statement unto itself. Basically what it’s a way to convince Mach 2 that you have an automatic tool changer, when in fact you do not (not yet at least). The auto-change routine includes a pause and a prompt to ask for the proper tool. Somewhere in there it applies the proper tool offset and then resumes the program. When we though this up it cut the production time of our brackets from 3 hours down to 1:20 flat. Now that’s a manufacturing improvement, more so it allows an unskilled operator to “baby sit” the mill without a bunch of training. This “Manual Automatic Tool Change” series is broken into 3 sections: Prepping the tools Setting up the tool table Setting up everything else and making it work ( This section) Making it all work This is the third and final (maybe) section on the “Manual Automatic Tool Change”. In this section we wrap it all up and put everything into play.

Setting up Mach 2 for Automatic Tool Change
In Mach 2 open up the Logic panel and select "AutoTool Changer", click OK to save and close the box

Set the Safe_Z value to something you like, I use 12.00" Don't worry about the "Tool change location stuff" those number can all be 0.00

Setting Up The Macros
Find your Mach 2 macros (a Macro is just a small program that runs within another program), the default location is C:\Mach2\macros\Mach2Mill. You can always go through Mach to get them, but I'm a Explorer sort of guy. You'll need to adjust a couple macros, but before you do that you need to do a few things: Make a folder called Originals in the Mach2Mill folder. Make a COPY of ALL the macros and put them in the Originals folder Lets get to work, go back to the Mach2Mill folder and do the following: Open up M6Start.m1s and replace whatever is in there with the following lines. SafeZ = GetSafeZ() ' Load Safe Z Value Code "G53 G00 Z" & SafeZ 'Goto the safe Z location Code "M99999" ' Call Macro M99999 Open up M6End.m1s and delete everything that is in there (if anything). Create a new file called M99999.m1s and place the following lines in it. tool = GetSelectedTool() 'Load the tool number SetCurrentTool( tool ) 'Set the tool Code "G43 H" & tool 'Set the height Complete = Question ("Change to tool number" & tool) Make sure you do the following: Hit ENTER a few times after the last line of the macro Make sure you don't end up saving the macros with a .TXT extension The proper extension is .m1s or pronounced Mach Numeral ONE Script

Testing It
Make a small program with the following line in it: M06T<Programmed Tool Number> Load the program Things to notice: Z is at 13.75 Tool Off is actually off (not green) and set 0.00 Tool # box is 0

Run the program Here's what happens: The mill head moves to MACHINE Coordinates Safe Z (12.00) A small dialog box pops up with a number 0 in it. Although the Elapsed time clock is not moving it is still keeping time and will update to when you hit OK.

Hit OK (don't change the 0 in it, just hit OK) and here's what you get Things to notice: Z is at 10.3103, but the head did NOT move. Tool Off is actually on (green) and set 1.6897 Tool # box is 10 (whatever number you used) If there are more lines in the program, the program WILL continue on. Why is Z 10.3103? From part 2 of this series you remember When the Tool Height Offset is applied it SUBTRACTS the height of the tool from the Reference Line Height and puts the resulting value into the DRO (numbers on the screen). 12.0000 (Reference line) - 1.6897 (Tool Height) = 10.3103 Congratulations: You have now written you first program to use the Manual Automatic Tool Change.

Using It For Real
Here is a sniglett of one of my programs (Step 1) (Spot Harsh Cover Holes) M06T10 G00 Z1.0000 G81 X14.9116 Y1.4974 Z.70 R.80 F10.0 X14.9116 Y2.4697 X15.7071 Y3.3536 X16.3598 Y3.2652 X16.6352 Y4.0165 X17.2097 Y3.6187 X17.6075 Y3.0442 X16.8902 Y2.7348 X16.9445 Y2.1161 X16.2374 Y1.4090 G80 (Move Table to REAR for tool change) G00 Z1.75 G00 Y0.2 (*******************************) (Step 2) (Drill 6-32 Pilot Holes) M06T16 G00 Z1.0000 G83 X14.9116 Y1.4974 Z-.1 R0.85 Q.10 F3 X14.9116 Y2.4697 X15.7071 Y3.3536 X16.3598 Y3.2652 X16.6352 Y4.0165 X17.2097 Y3.6187 X17.6075 Y3.0442 X16.8902 Y2.7348 X16.9445 Y2.1161 X16.2374 Y1.4090 G80 (Move Table to REAR for tool change) G00 Z1.75 G00 Y0.2 (******************************) (Step 3) (Drill 5/16 Pilot Holes) M06T13 G00 Z1.0000 G83 X1.1250 Y1.7500 Z-.1 R0.85 Q.35 F8 X1.1250 Y4.2500 X3.3750 Y4.0000 X2.5090 Y3.5000 X2.5090 Y2.5000 X3.3750 Y2.0000 X4.2410 Y2.5000 X4.2410 Y3.5000 X8.8750 Y4.2500 X8.8750 Y1.7500 G80 (Move Table to REAR for tool change) G00 Z1.75 G00 Y0.2 (******************************) And so on... What happens it the machine starts out and asks for tool #10 (spotter) and zips down to spot a bunch of holes. When it finishes the holes it moves the table to the back and out of the way. M06T16 comes a long and we begin the tool change sequence, we swap the bit, hit OK and the program starts drilling holes. Again we move the table out of the way, and start another change cycle, and drill more holes.

Final Thoughts The sequence probably could use some cleaning up; leaving the number in the dialog box doesn’t thrill me, not to mention a few other things. But setting it up is fairly quick and doesn’t require a PHD. The more bells and whistles, the harder the setup. I’ve been thinking about revisiting this and adding a few features to the entire series Auto tool height sensor Auto Spindle shutdown during the cycle Auto Coolant shutdown during the cycle Auto table positioning (move table to the rear) And a few other things. I honestly don’t know when I’ll get to them; I think the Auto Tool Height sensor is coming first, maybe in a month or so. 网上找来的，或许有人感兴趣，有看得懂的话看一下吧，要是能翻译一下就更好咯。

设置好像不是很难，但是因为没有全部看懂，也就不敢妄下结论。