Tool Library Offset -< Answered>

[ScotY]

Thank you!

[Crosshatch]

Thank you!

Just so you know, I'm on a Mill, not lathe btw (just writing this to make sure we are on same page).

I never had to use a reference tool in Mach3, not at least how I had it setup from memory.

-Jason

[ScotY]

Mill here also. I struggled with my lathe tool setup...that was confusing to me. This seems more straight forward.

I used Mach only briefly so not really familiar with it. The Z Ref feature sounds like it will make it easy to keep the tool library set up.

[Muzzer]

I've got a TT-2 type electronic tool touch setter on my mill (Chinesium, from ebay), bolted to the table and wired into the Acorn. The controller knows where to find it (using G30 coordinates) and the Z ref "auto" function is a great feature. If I ever move the table height (mine's a knee mill), I can acquire the current Z position by telling it which tool I have in the spindle (MDI "T5H5" etc) and get it to do an "auto Z Ref" move which automatically acquires and sets the new Z ref. If you need to set a new tool, you load it (select it from the tool offset screen) and do an "auto tool length" measurement. The rest happens automatically.

Definitely recommended!

[Crosshatch]

I will eventually take a look at this TT2 setter. Oddly enough, I snapped my new endmill yesterday. This had nothing to do with the topic of this thread, it was rather pathetic as how it snapped and it wasn't cheap!

Hoping to report back later today on some results.

Regards,

Jason

[Crosshatch]

Ok. I have news. first and foremost, Admins...please see my "Report" attached.

I have a 3-Axis Mill with Home switches.

So I spent a good time tonight preparing to AIR cut a test piece which was 1" higher than the actual workpiece with the intention to cut the part after a successful test.

Here is what is happening. My machine is home to the limit switches and the MACHINE DRO is set on three (3) axes to 0.000. The part is stationed in the vise and the setup key was used to define the edge of my workpiece in cordinate WCS #1 (G54) with goal of using T5H5. I had the offsets correctly accounted for and could in the MDI zero the part by commanding G01 X0.0 Y0.0 F25 to move the tool over the corner; the Z-axis was also set off the part using a 123 block and the zero (0) height was set off the 123 block as I did not yet want to cut the part. So far so good, cycle start the program and the machine heads to the max Z position and stops, waiting for the tool change to happen because of T5 G43 H5 T6 (shown below).

(T5 D=0.375 CR=0.015 - ZMIN=-0.855 - BULLNOSE END MILL)
(T6 D=0.25 CR=0. TAPER=45DEG - ZMIN=-0.785 - CHAMFER MILL)
G90 G94 G91.1 G40 G49 G17
G20

(TOP_FACE)
M5
M9
T5 G43 H5 M6
S6000 M3
G54
M9
G0 X5.8463 Y-0.9375
Z0.1
G1 Z0.04 F35.
G18 G3 X5.7962 Z-0.01 I-0.05 K0.
G1 X5.59
X0.
G17 G2 Y-0.6807 I0. J0.1284
G1 X5.59
G3 Y-0.4239 I0. J0.1284
G1 X0.
G2 Y-0.1672 I0. J0.1284
G1 X5.59
G18 G2 X5.64 Z0.04 I0. K0.05
G0 Z0.5
G17


Upon Cycle Start to resume the program due to the tool change (which was already in the machine and used to zero the z-axis) I hit the Cycle Start only to receive an error "907 Z axis travel exceeded" due to " Z0.1" highlighted in red.

Here is what is know, at the moment in the MACHINE DRO is at the following ordinates away from the switches: the X-Axis (+2.6170"), Y-Axis (-4.0690"), Z-Axis (0.000"). Because WCS #1 is used to offset the part, the absolute coordinates are: X-Axis (+0.7650), Y-Axis (-0.3900), Z-Axis (3.886") relative to the part in the vise.

Why is Acorn simply not traveling to the Z0.1 from the current height of 3.866" and instead giving the error because it exceeds the Home Limit of the Z-axis? I understand that Z0.1 violates the MACHINE WCS because the machine is at it's maximum height, hitting the limit switch and not being able to travel more in the positive direction. However, the part is defined in WCS #1 so shouldn't the machine travel down to Z0.1 in WCS #1 as per the G-Code which would NOT put the MACHINE WCS in the positive direction but rather in the negative and not violate anything? It's acting as if the G-Code thinks I am in the Machine WCS.




Please advise.

Regards,

-Jason

[Centroid_Tech]

Looking at your report, you have the software travel limit for the Z axis set to -6.375 but yet the Z axis Part0 in WCS#1 is set to -6.86 which is past your software travel limit. I also see that you have offsets in your Tool Offset library but it appears that Z Reference has not been set. You need to set Z Reference in order for the control to accurately take the height offset values into account.

[Crosshatch]

Looking at your report, you have the software travel limit for the Z axis set to -6.375 but yet the Z axis Part0 in WCS#1 is set to -6.86 which is past your software travel limit. I also see that you have offsets in your Tool Offset library but it appears that Z Reference has not been set. You need to set Z Reference in order for the control to accurately take the height offset values into account.

The Z Axis Part Zero is only -3.886" from the home switch which should leave me a few more inches before I reach the maximum depth.

For the tool offsets, I suppose I'll take the longest tool as the controller says. Can the surface be any arbitrary surface just to do the offsets even if that surface changes in the future?

Thr offsets I have now are simply the lengths of my tools from spindle nose to end of cutting flute, which is why I put them positive.

I'm still not sure how I feel about the limit, as I don't know how to fix that.

Regards,

Jason

[Centroid_Tech]

The Z axis software travel limit is a finite value. It should be the total distance that your Z axis can travel before it will hit something.

You can use the spindle nose as your Z Reference but based on the report that you attached, the Z Reference was never set. When you are in the Tool Offset library, press F1(Z Ref). Jog the Z axis until the spindle nose is at the desired location, typically the same location that you are using to measure your tools from. Then press F10(Set). Now all of the values in the height offset column for your tools will be in relation to the value in Z Ref.

[ScotY]

Jason,

What I did was use a 1-2-3 block and jogged the spindle nose until it just touched the block. Then set Z Ref. I then touched off my tools to the same block and set their offset values (all positive values). If I ever break a tool, I can just set the new tool offset using the same block without resetting Z Ref (as I understand it). I guess the Z Ref is like setting your zero point?

Since you are measuring your tools using a height gauge, the offset value should be the same as if you used the method I used above. I used a 1-2-3 block because my Z-limits won’t allow the spindle to drop all the way down to the table.

What I don’t understand is why you actually need a Z Ref position. I want one to make adding/changing tools easier so I don’t have to remeasure them all. But it would seem to me that provided all tools have an offset, the control should know where to position the tool.