Tool Height Setting Probe - Mach3 - solution

[HiltonSteve]

Well got the Gerrys 2010 screenset, installed it as per the manual, and got to say that it looks much nicer than the original Mach screen. A lot easier to navigate around, took me about 5 mins to get my head round it.

Still not bothered with the homing switch's and I have got the auto tool length setting working just fine without them, I will be putting them on at some time soon though. Set up and tested my soft limits and they should give me enough protection at this stage.

Quick question - In the Auto Zero settings, can I set the tool using my height probe on the bed of the machine, put the height of the probe into the plate thickness box (41mm in my case) and then put the distance from the bed to the top of the job (Z0) in the material offset. This is more or less the same method that I have used on larger CNC machines in the past, only difference is the G54 Z offset is not used and the figure in the material offset box is used in its place. The simple auto zero button seems to achieve this but not played enough yet to see if the material offset workaround will work or not.

Theory behind this is quite simple, if i tell the machine how far the top of the work is from the bed by measuring it then the machine only needs to know where the tool is in relation to the bed. For a lot of my jobs I tend to be cutting rough sawn hardwoods which first need facing to give me a flat surface to work on and I usually set my z0 lower than the top surface as it is so uneven. This means setting zero on the top is no good to me.

JAZZ, let me know where you want the £6.64 sending and I will sort it tomorrow.....

[JAZZCNC]

Quick question - In the Auto Zero settings, can I set the tool using my height probe on the bed of the machine, put the height of the probe into the plate thickness box (41mm in my case) and then put the distance from the bed to the top of the job (Z0) in the material offset. This is more or less the same method that I have used on larger CNC machines in the past, only difference is the G54 Z offset is not used and the figure in the material offset box is used in its place. The simple auto zero button seems to achieve this but not played enough yet to see if the material offset workaround will work or not.

You know these four letters. . . RTFM.!! . . . . But here's a snippit.! (Example 2 )

" Material Offset: Use the Material Offset option to zero the Z axis to a position offset from the plate
bottom. Check the box to enable this option. If unchecked, the offset value is ignored.
Example: Say that you have g-code that cuts profiles .74” deep into a .75” thick panel, and you'd like to use
the same code on thinner material, say .50”. There are two ways to use the offset.
1) Set the offset to the difference between the material originally coded for (.75”) and the material your
using (.5”). You'd set the offset to .25”, and zero with the plate on the material. Z zero will be set
.25” above the material.
2) Set the offset to the thickness of the original material, .75”, and zero to the bed of the machine. Z
zero will be set .75” above the bed. This will allow you to cut the profiles from any material
thickness not greater than the original.
Note: Negative values are allowed for the material offset. If a negative value is used, a message will be
displayed to notify the user, followed by a 3 second pause, before the probing operation begins."

Send the £6.64 along with my consultencey fee's to RSPCA for chimps.!!

[Ger21]

Still not bothered with the homing switch's and I have got the auto tool length setting working just fine without them, I will be putting them on at some time soon though. Set up and tested my soft limits and they should give me enough protection at this stage.

If you don't have Home switches, just Ref the Z at the top of travel. This will allow the macros to keep from crashing the Z axis into the top of travel if you enter some settings that won't work. In order to use the toolchange position, park position, and tool change auto zero, you need a repeatable home position. Switches make everything easier.

Quick question - In the Auto Zero settings, can I set the tool using my height probe on the bed of the machine, put the height of the probe into the plate thickness box (41mm in my case) and then put the distance from the bed to the top of the job (Z0) in the material offset. This is more or less the same method that I have used on larger CNC machines in the past, only difference is the G54 Z offset is not used and the figure in the material offset box is used in its place. The simple auto zero button seems to achieve this but not played enough yet to see if the material offset workaround will work or not.

Theory behind this is quite simple, if i tell the machine how far the top of the work is from the bed by measuring it then the machine only needs to know where the tool is in relation to the bed. For a lot of my jobs I tend to be cutting rough sawn hardwoods which first need facing to give me a flat surface to work on and I usually set my z0 lower than the top surface as it is so uneven. This means setting zero on the top is no good to me.

The short answer is yes. The G54 ofset is still used, bbut the zero position is offset by the Material Offset amount.

I use the material offset so that I don't need to worry about the actual thickness when I program my parts. I just program to cut .75" deep, and it doesn't matter if the part is .78 or .68, it always cuts right to the bottom. I zero to the spoilboard and use a material offset of .75".

Of course, if doing V-Carving you need to zero to the top, but if you're just cutting out parts, the material offset can make things much easier.