Mach 3 tool changing

[Crawling Calvin]

Can anyone who uses Mach 3 with tool table explain to me how to do it. I understand how full size machines set "zero." I have had a few crashes with my mill and im going back to the old method of setting each tool individually

The way I am doing it is I am using a height setting tool on a 'fixed' location on the mill (the table) and it has a height of 2" which is compensated in Mach 3.
I home the machine before setting the tools so it understands how "long" they are from "Z0"
Then i set the tools individually on the setter and have the software note lengths.

I have it ignore the tool change macro but it does acknowledge the tool change and adjusts offset as necessary.

Some of the time this seems to work and others it ends up being a giant crashing disaster anyone who uses a mill with mach 3 and uses the tool table i'd really appreciate it if you could explain how since I am sick of crossing my fingers and HOPING the mill doesn't crash!

[Etype R]

Is your cam program outputting a g43 h# command with the tool change? That is the height offset code that goes with each tool.

T2
G43 h2

My machine uses centroid, but still has a tool height offset call out in the g code. I came a across this thread on mach 3https://www.machsupport.com/forum/index.php?topic=25107.0

[Crawling Calvin]

Mine outputs it as
T4 M6
G43 H4

[Etype R]

Is your m3 line after that?

Might want to remeasure all of your tools, make sure they are saved properly. I have set mine before, and forgot to hit the save button. Also a good idea to show your feed after a tool change and hit feed hold as the bit gets close to the work piece. Make sure what the control shows on the dro looks right.

[Crawling Calvin]

Originally Posted by Etype R

Is your m3 line after that?

Might want to remeasure all of your tools, make sure they are saved properly. I have set mine before, and forgot to hit the save button. Also a good idea to show your feed after a tool change and hit feed hold as the bit gets close to the work piece. Make sure what the control shows on the dro looks right.

Ill do that. I need to get a new tip for my 3D taster which is my normal touch off tool. Right now though one of the tools in my cutting library is a touch off. Im going to try and make a different tool the touch off and see what happens. That could be causing problems

[rob_b]

I don't have my limits installed yet so I use the following...

Pre-load all programmed tools into their holders
Select the longest tool (gauge line to tip)
Make sure no tool length offsets are applied (G49) (Stay in this mode during the entire procedure)
Touch-off longest tool to a gauge block
Zero DRO and check that longest tool has no length offset in the tool table.
Touch-off all remaining tools and record their Z values in the length offset of the tool table(these will always be negative numbers)
Run the program

Assuming all of your numbers are correct this insures that if there is some kind of length offset or G43/G49 hiccups your tool is always shorter than the DRO reads. All except the longest tool of course.

Once your tool table is set you can touch off on your work with any tool just make sure you...

T# M6
G43 H#

...first

[C*H*U*D]

The tool table is one of my favorite features of Mach.

I use a height gauge and granite block to measure all of my tool holders on my work bench. I have one tool holder loaded with a dial indicator...it gets measured at it's zero. Once all my lengths are set in the table, I load the dial indicator and run it to zero, then zero the Z in Mach and it's set.

Here are some videos that explain it better:

Mach3 Tool Tables Made Easy « Milling Around

[Crawling Calvin]

Originally Posted by C*H*U*D

The tool table is one of my favorite features of Mach.

I use a height gauge and granite block to measure all of my tool holders on my work bench. I have one tool holder loaded with a dial indicator...it gets measured at it's zero. Once all my lengths are set in the table, I load the dial indicator and run it to zero, then zero the Z in Mach and it's set.

Here are some videos that explain it better:

Mach3 Tool Tables Made Easy « Milling Around

The one thing that always got me with that was if the number is supposed to be negative or positive... when I get the tip for my Haimer 3D taster ill retry that method again

[Crawling Calvin]

Wow huge thanks for the help guys I got it! *knocks really hard on wood*

I set my tools in the machine using a 2" height setter and then made a random tool (not being used) #1 aka the master tool and used that my setter and minus buzzing into my vise jaws which was my fault I got my parts done



Its such a nice feeling to have the machine working pretty well overall minus the great vise jaw munch but that is 100% my fault

[C*H*U*D]

Originally Posted by Crawling Calvin

The one thing that always got me with that was if the number is supposed to be negative or positive...

None of them will be negative.

Measure all of your tools, and enter their total lengths into the table. Measure your Haimer at it's zero point, and set it to whatever tool # you wish...let's say #1.

Now load your Haimer and tell Mach it has #1. Bring the Haimer down until it Zeros onto the workpiece, enter 0" into the Z field of Mach, hit enter and you are done. Now when your program calls for a tool change, you'll see the difference in the offset right next to the tool number.

You can check all of this without running a program just to make sure you have it correct. Enter a bunch of tools into the table. Then zero your Haimer somewhere on a workpiece. Change to tool #2 and tell Mach it has #2. Bring it down to the same place and it should be at the same height as the Haimer when Mach reads 0.000". Continue with all of the tools.

I did that many times before I began to trust the table, but now I just enter everything and go. I still keep a hand over the E-stop until the first complete run, but haven't had it screw up yet.