Manual Automatic Tool Change

 Setting Up the Tool Table

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 ( This section)

  • Setting up everything else and making it work

Setting up the Tool Table

Before we begin with the pictures we need to get some terminology down.

Reference Line:  Is an imaginary line that runs parallel with the table just under the quill.  It is your Z reading when no offsets are applied; in my case it’s 13.75”  (Gotta’ love the Full Head Z).

Tool Height Offset:  A positive number that represents the height of a tool.  This number is subtracted from the Reference Line height to get an actual working height.

For example: 

When I execute a G00 Z0 with no cutter in the spindle and no offset applied it drops the nose of the collet right to the table.  A less technical way of saying “The reference Line is at Z 0”.

  • Z DRO Start Position:  Z 13.75
  • Z DRO End Position:  Z 0
  • Applied Height Offset:  0.00

If there is a cutter in there kiss it good-bye, as it will be planted through the table.

Now, when I mount a cutter say 2” long into the collet, it extends PAST the reference line by 2”.  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).  Now when I execute a G00 Z0 with the offsets APPLIED it will drop the very tip of the cutter to the table.

  • Z DRO Start Position WITH offset:  Z 11.75    (The original Z 13.75 - Tool Height 2.0)
  • Z DRO End Position WITH offset:  Z 0
  • Applied Height Offset:  2.00

As far as the Mach 2 DRO reads it moved from Z 11.75 to Z 0.

That’s it; basically you’re telling Mach how long a tool is, nothing magic.  The reason it’s a table is so you can keep a bunch of tools on file.  Mach 2 allows for 255 tools, I use 20 or so, and of those only 10 on a regular basis.  But, oh how those 10 make a difference.

 
All we need to set the height of a tool.

1/2 R-8 Collet, 1/2 double sided end mill, 0.125 precision ground flat stock.

We use the 0.125 P-Ground flat as a shim, you're welcome to use whatever you want.  We actually pick this up in 36" lengths and cut them into usable lengths, they make great parallels too.

 
Start be Referencing Your Machine and LOCK the QUILL.

VERY IMPORTANT STEPS

 

Mount the cutter into the collet, ensuring it makes solid contact with the collet.
 

This is what the Mach 2 numbers will look like of my machine when "Ref'ed" .  Z 13.75 is the important one.

I did a fair amount of customization to the Program Run screen to tune it for the way we work, if you would like the screen design just let me know and I will send it to you.  Your screen will look quite a bit different, but the important numbers are the same.
 
Rapid the cutter down to the table, just above the 0.125 shim
 
Lift one end of the shim and slowly (less than 1 IPM)  lower the cutter the rest of the way, this way it will push it down to the table.

Don't get your finger pinched.
 
Gently set the cutter on the shim, actually I can slide the shim out, but I feel the cutter drag across the top.
 

With the end mill sitting on top of a 0.125 shim here are the Mach 2 numbers.  Once again focus on the Z Axis.
 

Change to the Tables screen (F5), it should look more or less like this.
 

Click on the Tool Table button on the right side of the screen.  Enter the name of the tool (whatever you want) and press Save Table.  Then press Select Tool Number and OK
 

Click in the Touch Correction box and enter the thickness of your shim (0.1250 for us).

Also notice the tool number has changed to #1
 

Turn the Touch Correction ON, it will flash yellow.

This is the part people forget.
 

Click on the Touch button in the middle of the screen.  that will do the following:

  • Calculate the current offset- touch correction
  • Apply the offset
  • Reset the DRO 

Just because I'm superstitious I open the tool table and click Save Table, I really do this because the value is cached as a parameter and not saved to disk until you press the Save Table button.  Under certain conditions, (I've found them) the program will revert to the SAVED value from the disk, so to avoid any problems I save the table after EACH TOOL is added/updated.

Our touch correction is STILL on, we just caught it in between flashes.
 

The updated table.
 

Back to the Program Run screen (F1), we can see the following:

  • Tool # 1 is selected
  • Tool Offset is 2.2690" and is applied (green led)
  • Current position of the cutter is 0.125 (right where we left it on top of the 0.125 shim)
  • Touch Correction is off (the flashing light is annoying) 
 

We actually use our Tool Table starting at #10, we leave 0-9 for just quick jobs.  For tools 0-9 we actually cleared out all the values before we started taking screen shots.

If you look over our tool table you'll notice one value stands out as being odd.  The #6 pilot has an offset of 5.6" which is pretty darn long for a little tiny bit.  Well, in the last section you'll remember that we "shanked" a pretty small bit, i.e. a new #6 pilot, the old one was lost in a tragic milling accident and we needed to use the chuck to complete the run.  We simply stopped the program, chucked up the bit, reset the table and did a "Run From Here" start.
Conclusion:

At this point just repeat the procedure for each tool, it's actually goes pretty quickly.  About 3-4 minutes per tool if you take you time.
Final Thoughts:

Although we didn't go over it, repeatability in the collet is half the battle, applying consistent torque to the draw bar is the key to success along with using the same collet for a tool after it's been setup in the table.

We always set tool height at X0 Y0, we do this for consistency. 

When we setup for a production run we do the following:

  • Pull all the tools and collets needed for the run.
  • Inspect and replace tools or collets as necessary.
  • Reset the height of all the tools for the run in the Tool Table, reference the Z Axis between each tool 

This little procedure takes us about 30 minutes for our most complex part, we'll then run about 18 hours straight with out a single issue.  If for some reason we break the run into 2 or more days and we shut down the machine we repeat the entire procedure again.  It's not that we don't trust the repeatability of the referenced machine, it's just a good practice to get into, not to mention good insurance against an avoidable mistake.  I know it seems like a pain in the ... but to get consistent results you need to have a consistent methodology.