Hello Guest it is December 15, 2019, 07:27:26 AM

Author Topic: Proper Tool Changes  (Read 2645 times)

0 Members and 1 Guest are viewing this topic.

Proper Tool Changes
« on: April 28, 2010, 10:02:34 AM »
Hello All, I have a cnc Knee mill under Mach3 Control. And I am wondering what the best way to set up my tools / and do tool changes is?

My Set up is as follows:

The mill has 5 inches of cnc quill travel
There is a semi auto tool changer (Air wrench with manual buttons to loosen the drawbar
The quill must be at the top for a tool change.

My Major questions are:

How to you set up your tools in a knee mill situation
(do you see each of them each time based off the top of the part?
If so what number to you put in for the offset?
Do you use a Gauge tool that does no change like a solid rod of X length in a holder and then set all tools based on that?
Again what is the offset if this is the method?
If you use the Gauge method do you use that gauge to set the top of the part?
)

How to you do tool changes so that the mill goes to the top of the quill and waits for input to continue?


Offline Hood

*
  •  25,856 25,856
  • Carnoustie, Scotland
    • View Profile
Re: Proper Tool Changes
« Reply #1 on: April 29, 2010, 04:57:27 AM »
I have just done manual tool changes for years on the knee mill by placing tools in  moving to Z zero and then cranking the knee to suit
Now however that I have a power drawbar (and plan on a toolchanger when I get time) on the Beaver Mill I have made a tool setter, this hooks directly to Mach and what I do is:
Place a probe in the checker and bring the checker down onto it, I then set my Z zero in Mach.
Next I place the next tool in the checker and bring it down onto the tool, press a button on my screen, it asks for tool height offset number and then when I enter that it puts the offset into the tool table, I repeat for all tools I will be using.
Once thats done I then put the probe in the spindle and touch off my material and zero the DRO, after that any tool I place in the spindle is offset to that zero position.
Pic of toolchecker and screen can be seen here. http://www.machsupport.com/forum/index.php/topic,10331.80.html
Hood

Offline BarryB

*
  •  267 267
    • View Profile
Re: Proper Tool Changes
« Reply #2 on: May 02, 2010, 10:15:24 PM »
I'm only a beginner at milling, but I'll yell you my ghetto tool change technique.  My spindle is
manual, so I have to muscle each bit it.  However to guage the height of the bits I use a brass pipe with a flat end.  I've been keeping the length of each bit the same, regardless of their diameter by shoving the pipe on it like a sleeve when tightening the collet.  I don't think it's the most elegant solution, but it works.
Re: Proper Tool Changes
« Reply #3 on: May 02, 2010, 10:46:12 PM »
If you're doing manual tool changes, unless your knee is CNC'd, don't even bother setting up the tool table - just change the tool, and zero it to the work using the knee, then hit CycleStart.  If your knee is CNC'd, I have a set of macros that I wrote to use the knee for doing tool-length compensation, though this requires using custom macros in your G-code (M843 instead of G43, and M849 instead of G49) for turning tool length compensation on and off, due to limitations in Mach3 (That will be fixed in v4).  I have another set of macros I use for setting up the tool table, using probing.

Regards,
Ray L.
Regards,
Ray L.

Offline BR549

*
  •  6,916 6,916
    • View Profile
Re: Proper Tool Changes
« Reply #4 on: May 03, 2010, 11:51:02 AM »
THere are MANY different methods for tool changing/guaging (;-)

My Major questions are:

** How to you set up your tools in a knee mill situation
(do you see each of them each time based off the top of the part?
If so what number to you put in for the offset?

With this method your top of material is a known value say Z0. When you change tools move over the material and touch off and reset Z DRO to zero each time.

OR just move over the material and move Z to zero and MOVE the knee to touch off.

**Do you use a Gauge tool that does no change like a solid rod of X length in a holder and then set all tools based on that?
Again what is the offset if this is the method?
If you use the Gauge method do you use that gauge to set the top of the part?

(;-) "My preferred method".

NOTE: this depends on IF ALL you tool lengths can be used inside of the Quill 5" envelope and NOT hit a Zlimit

  Use a MASTER guage to reference all other tools too, then use the master to set the initial TOM.

The tool offset is simply the difference in height from the master to the tool being checked. Then register each tool in the tool table.

NOW mach can use this data to automatically adjust the offset in your Gcode providing you are using Tool height offsets . YOU must code this into the gcode.

You can do this  ON the machine or OFF the machine(;-)

Manually (off the machine) requires a fixture to MEASURE tool heights. then you take the values and inoput them into the tool table.

 ON MACHINE lets the machine do all the work measuring AND registers the tool in the tool table automatically.


**How to you do tool changes so that the mill goes to the top of the quill and waits for input to continue?

You would set up code in the M6start macro to tell mach to go to MACHINE POSITION (G53) " Z0" ( assuming you ref your Z to up(top)  =0.000. Then when an M6 is called the machine will move up to the top of travel in Z. You can also tell it to move out to a known X/Y location as well.

ALL in ALL a simple process ONCE you decide what is BEST or Easiest for you.

Hope that helps