Offsets.... ARGH!!!

[cjdavis618]

I have an SX3 mill that I converted and have been looking to setup the tool offsets for my mill. Finally want to take advantage of the tool change features to speed things up.

I have been able to enter the dimensions into the mill for tool hieght and also have my 1st tool which is the longest. But I have something that I can't seem to get past.

I can setup my mill with a dummy part (cardboard box), then set my Tool 1 to zero with that. (Tool 1 is a 2 Inch plunger indicator set to a specific depth of 6.153" length)

When I cycle the tool change to T2 which is only 2.947", it works like it should and drops to Machine coordinates of 5.980 But when I change from T2 to T4 as a test, the offset stays at the T2 length, even though Mach Tool DROs show the change.


Tool lengths and Zero positions on part top.
T1 - 6.153 (Machine Coordinates -3.0393)
T2 - 2.947 ( - 5.980 )
T4 - 2.154 ( - 5.980 ) (correct tool# and offset show in main screen DRO, but Cutting coordinates remain at T2 offset distance)

I used a macro that I found at Mach3 forums that allows me to go to a position on the table for tool changes, and also asks me to touch off a plate for auto zero, but I do not use that part. Once I click cancel on that, then insert the new tool, it returns to the next cutting coordinates, but doesn't apply the correct amount of offset.

What doesn't make sense though is that if the macro is screwing up the offset entry, why only on the 3rd tool and not the 2nd tool?

I have made sure that the gcode shows
M6 T2 G43 H2 for second tool.
(I've tried with and without G49, no change)
Then M6 T4 G43 H4 for 3rd tool change.

What am I missing?

Thanks for the help.

[rwskinner]

I noticed weird behaviour as well on Mach's tool offsets. For instance, I have tool 1 set up just like you and I zero tool 1. Now I use the mach screen and change to any tool and test and the offset works fine.

However, using G-Code, if I already have tool 4 in the machine, and the tool change in the G-Code ask for tool 4, I press Cycle Start and everthing gets whacked out. Is the H4 changing the offset again? It shouldn't since this should be the tool offset measure from the spindle nose.

If I make sure I select any other tool first (Tool 0 by habit now), the G-Code works fine.

It cost me a nice 1/4 carbide end mill when it rapid z into the work (aluminum). Ruined the work as well.

I don't care to see how often it happens, I just select tool zero before I hit cycle start and the problem went away.

[Torsten]

I have an SX3 mill that I converted and have been looking to setup the tool offsets for my mill. Finally want to take advantage of the tool change features to speed things up.

I have been able to enter the dimensions into the mill for tool hieght and also have my 1st tool which is the longest. But I have something that I can't seem to get past.

I can setup my mill with a dummy part (cardboard box), then set my Tool 1 to zero with that. (Tool 1 is a 2 Inch plunger indicator set to a specific depth of 6.153" length)

When I cycle the tool change to T2 which is only 2.947", it works like it should and drops to Machine coordinates of 5.980 But when I change from T2 to T4 as a test, the offset stays at the T2 length, even though Mach Tool DROs show the change.


Tool lengths and Zero positions on part top.
T1 - 6.153 (Machine Coordinates -3.0393)
T2 - 2.947 ( - 5.980 )
T4 - 2.154 ( - 5.980 ) (correct tool# and offset show in main screen DRO, but Cutting coordinates remain at T2 offset distance)

I used a macro that I found at Mach3 forums that allows me to go to a position on the table for tool changes, and also asks me to touch off a plate for auto zero, but I do not use that part. Once I click cancel on that, then insert the new tool, it returns to the next cutting coordinates, but doesn't apply the correct amount of offset.

What doesn't make sense though is that if the macro is screwing up the offset entry, why only on the 3rd tool and not the 2nd tool?

I have made sure that the gcode shows
M6 T2 G43 H2 for second tool.
(I've tried with and without G49, no change)
Then M6 T4 G43 H4 for 3rd tool change.

What am I missing?

Thanks for the help.

Not sure if that is the problem but the format seams confusing.
Try this

M6 T2
G43 H2 Z3. (Moves to Z3. at H2 offset)

M6 T4
G43 H4 Z3. (Moves to Z3. at H4 offset)

Hope that takes care of your problem.
The Z- Coordinate should be a clearance Plane above your part and Clamps
from where you can rapid to your X and Y coordinates.

[cjdavis618]

I finally got it but I worked at it all day I think. Thanks for the help. After I posted this, I broke out the Peter Smid books and started back at the basics. I learned that 2 things were very important. But it did help to split up the lines with the tool changes also.

So instead of M6 t4 g43 H4,
use M6 T4
G43 H4

It does seem to work better.


1. Having homing switches is a must to do this at all. (Sets machine zero to reference)
2. Knowing what your total work envelope is from spindle bottom to Mill table.
Without those constants, you cannot double check your measurements in the system to know what is wrong when problems occur.



Since I got that figured out, I got ambitious and setup my Wildhorse innovations touch probe today and just now figured out how to use Hoss's Touch probe buttons and scripts with it and still keep my offsets from screwing up my machine.

I'd call it a good day.
Now I am ready work.

I did find out for certain that since I used my longest tool as my "reference tool", I only needed to enter the actual length of the following tools. Mach 3 did correct the distance and put them where they were needed. All tools were entered with a positive measurement.

Here are the steps I used to do this. They are different based on what tool I referenced from. The part must already be secured to perform any of this.


Touch Probe:
1. Connect Wildhorse Touch probe to mill control Area. (using 1/8" jack in my case)
2. Make sure that the tip is secure in probe socket.
3. Seat probe in spindle (R8 endmill holder in this case, permanent)
4. Load mach 3 "Probe and offsets page" (Provided by Hoss here)
5. Ref All Home in offsets page. (Makes sure your machine knows it's zero positions)
6. Make sure that Tool offsets are off. (Hoss button macros cause issues with Tool offsets on, at least for me. They like to go right through a limit switch.)
7. Jog to part corner Within 1/4 to 1/2 inch of edge
8. Select zero task (Wait while part is referenced)
9. Click "Goto zero" (This allows the system to get to a position to enable offsets again)
10. Click Apply Offsets
11. Click Z zero button above "Tool Information". (Adds probe length to part offset.)
12. Load good G-code and start cutting program.

(Note, I have the Gcode start with a tool change to automatically apply the next offset that is needed with the correct tool)

Dial indicator:
1. Ref All home
2. Insert Tool 1 "Reference tool" into spindle. Longest tool in use. (Tool number can be any number, as long as you reference with the longest one.)
3. Load mach 3 "offsets page"
4. Make sure T1 is selected in Tool info, and Click Apply Offsets if not already on.
5. Jog spindle with indicator to part surface to reference for part Offset.
6. Lower spindle until you reach a REPEATABLE point on your indicator. (Critical that you know a measurement on the indicator to always zero with.
7. Click Z button above tool info area to reference part. (This will update the part offset.
7. Load good G-code and start cutting program.

Of course to do any of this, you will need tools in the tool table entered. And when you put data into mach3. Always hit the "ENTER" key so the data will stay. That has been my problem for the most part. Numbers that don't stay, do not work.




Hope this helps somebody.