[Runner4404spd]

setting up mach 3 with cnc mill. when setting up the z do you call the home position zero or +14.75?

[SCzEngrgGroup]

setting up mach 3 with cnc mill. when setting up the z do you call the home position zero or +14.75?

Z=0 is typically the top of the workpiece in work coordinates. The home position for Z is the uppermost extreme of travel, and can be assigned any value you like in machine coordinates. It's really up to you to determine how to define and manage the difference between machine coordinates and work coordinates.

Regards,
Ray L.

[TOTALLYRC]

setting up mach 3 with cnc mill. when setting up the z do you call the home position zero or +14.75?

In Mach3, if you have home switches and you have the auto zero set, when you referance the axis, z home = 0, at least the way I have it set up. If the home switch is 0 and at the top of the column, then your z moves are all negative.

Mike

[Cruiser]

Runner, Are you asking for setup of basic macnine or for part, fixture, vice optional offset.

[Runner4404spd]

i am asking about the general machine setup. the reason i ask is because i'm having a problem with the tool change option. basically when i program a tool change with a T1 M6 sometimes the z axis wants to go down and sometimes it wants to go up? i don't really understand why its doing this. i am thinking its looking for some home position but i don't understand why. i would just expect for the spindle to stop and i would have to position the tool in such a way as i can swap it.

i was reading through the tool change setup on IH website and it seems i have my machine setup wrong. i currently have machine zero set at the top of the z axis off the z axis home/limit switch. i am running the IH kit on my IH mill but i built it myself.

[Cruiser]

OK, I think what you want is this !
Take your tool holder out so nothing is off end of spindle, then touch off using standard (touch off block) and set the end of spindle to table and set this dimension into dro "z". Now standard measure (i use 3" standard from micrometer) should show in z readout. turn off auto zero on the z homing and home it again and read the distance from table top to home switch and write it down so you can enter it in the appropriate block on auto homeing so it will be writen into dro every time you home the machine. If done correctly you will be able to turn on machine, home the machine and without a tool in spindle command GO Z0 and it will run down and kiss the table top, within whatever tollerances you applied. Now Z zero is table top and you can measure vise, fixt, matr'l, whatever and set the machine propperly.

[ger21]

Either your M6start or M6end macro is probably telling the machine to go to SafeZ. probably the M6end. If it looks like this:



REM The default script here moves the tool back to m6start if any movement has occured during the tool change..

x = GetToolChangeStart( 0 )
y = GetToolChangeStart( 1 )
z = GetToolChangeStart( 2 )
a = GetToolChangeStart( 3 )
b = GetToolChangeStart( 4 )
c = GetToolChangeStart( 5 )
SafeZ = GetSafeZ()
if SafeZ > z then StraightTraverse x, y,SafeZ, a, b, c
StraightFeed x, y, z , a, b, c



Then try changing it to this:


x = GetToolChangeStart( 0 )
y = GetToolChangeStart( 1 )
z = GetToolChangeStart( 2 )
a = GetToolChangeStart( 3 )
b = GetToolChangeStart( 4 )
c = GetToolChangeStart( 5 )
StraightTraverse x, y, z, a, b, c