Transitioning from Negative Tool Offsets to Positive Tool Offsets on VMC

[cgrim3]

Hi all,

We are currently trying to transition from using negative tool offsets to using positive tool offsets on our machines. Please see the attached link.

Lesson 5: Everything about CNC Tool Length Offsets. Positive and Negative (G43 g-code, H offset) | HSM Machining

Resources and Software For High-Performance CNC Machinists

zero-divide.net

Positive tool offset is measuring the tool from the gage line. See image below.


Negative Tool Offsets look like this. See picture below:



We have a Zoller Venturion 450 tool setter where the tool length is measured outside the machine. The zoller tool setter measures tool length from gage line thus using positive tool offsets. However, I take it that in order to use positive tool offsets, you must have Renishaw probes to measure G54 Z since it is measured from the gage line of the machine to the top of the part and a renishaw probe can quickly do this.

However, we have some older Fadals, Makinos, and an old Kitamura that do not have renishaw probes so we have been using negative tool offsets for those machines (setting our tool offsets and G54 Z from a 123 block in the machine).

We would like to use positive tool offsets for these machines but do not want to buy expensive Renishaw probes for them. What is a quick workaround for this? I was thinking of possibly buying a Haff and Schneider 3D taster (see below). The procedure would involve picking up Z on the workpiece with the 3D taster (zeroing out needle on top of workpiece) and have a macro in the controller do the following: (Z value measured by 3D taster when needle is @ zero + gage length of 3D taster when needle is @ zero) = G54 Z value.


Does this seem like a good solution of measuring G54 Z without renishaw probes?

What is everyone's thoughts?

Thanks,

Chris

 

[Booze Daily]

Back in the old days I would put a 123 block on top of the stock, touch the face of the spindle off that, and put that -Z value in G54.

Then activate G54 thru MDI and touch all the tools off the 123 block. This gives gage length offsets.

When finished, move G54 down 3” to account for the 123 block and you’re done.

 

[EmGo]

Back in the old days I would put a 123 block on top of the stock, touch the face of the spindle off that, and put that -Z value

What ?!?! You didn't buy a Millabrator ? Cheapskate ! No wonder the world is going to the dogs !

 

[cgrim3]

Back in the old days I would put a 123 block on top of the stock, touch the face of the spindle off that, and put that -Z value in G54.

Then activate G54 thru MDI and touch all the tools off the 123 block. This gives gage length offsets.

When finished, move G54 down 3” to account for the 123 block and you’re done.

This is good and all but we have a super expensive Zoller Venturion Tool Setter we are trying to put to good use. We would like to use the Zoller Tool Setter to set all of the tools in the shop if possible.

 

[cgrim3]

Also, if my method of using a 3D taster works, how would I write the macro program on the Fadal for (Z value measured by 3D taster when needle is @ zero + gage length of 3D taster when needle is @ zero)

 

[rklopp]

I do what you are proposing but without a macro. I measure positive TLOs from the gauge line to the tool tip using a 40-taper pocket on a surface plate and a height gauge. I do the same with my Haimer probe, driving the probe down with the height gauge until it reads zero. I memorize that number, which, in my case is 6.9970" from the gauge line to the zeroed Haimer tip.

I plug in the TLOs in my offset table. I keep the Haimer in the last ATC pocket without any TLO for it. When I need to probe for G54 Z, I call up the Haimer, touch whatever is my reference surface, go to my offset page and G54 Z. I enter Z6.9970 and then hit Measure (this is on a Fanuc). No doubt there's a way to write a macro to accomplish the same and avoid the risk of fat-fingering the Haimer length. If in doubt, I can do a sanity check by referencing the Z axis and then using a tape measure to measure from the spindle face to the Z reference plane.

 

[SteveEx30]

What you propose is fine. You could use any plunge style indicator for picking up z.

I prefer having Z0 on the FCS plate so it never has to be picked up constantly. I never used top of part..
Even the old days, Z was on top of the 123 blocks on the table.

 

[angelw]

However, I take it that in order to use positive tool offsets, you must have Renishaw probes to measure G54 Z since it is measured from the gage line of the machine to the top of the part and a renishaw probe can quickly do this

Not so. Once you have the Tool Length Measured via your External Measuring device, and registered in the Tool Offset Registry, a totally manual method without a Measuring Probe is as follows:

1. Call any tool that has the Tool Length Registered, into the Spindle.
2. Toch off the Tool on the Top of the Workpiece.
3. Make the following calculation:
ZWSO = MC - TLO - ZA

Where:
ZWSO = Z Work Shift Offset value to be plugged into G54 to G59
MC = Machine Coordinate (It will be a Negative Value)
TLO = Tool Length Offset (It will be a Positive Value)
ZA = Z Allowance - the amount of material left on between the Touch Off Surface and Z Zero (This will be a Positive Value)

Example:
ZWSO = -450 - 120 - 1
ZWSO = 571

Plug the ZWSO value into the Z Offset Field for the G54 to G59 Offset being used.

The above can be achieved using a quite simple User Macro, where the Macro will:
1. Retrieve the Offset Value of the Tool called into the Spindle.
2. Read the Current Machine Position for Z when the Tool is Touching the Top Surface of the Workpiece.
3. Calculate the Z Work Shift Offset using the same algorithm in the above, manual example and plug it into the specified Work Shift Offset.

The Work Shift Offset Number and the Z Allowance is passed to the Macro Program via the Macro Call Block.

In use, you would manually move the Spindle Tool down to touch off on the Surface of the Workpiece, then execute the Macro Program.

Regards,

Bill

 

[rklopp]

I keep the Haimer in the last ATC pocket without any TLO for it. When I need to probe for G54 Z, I call up the Haimer, touch whatever is my reference surface, go to my offset page and G54 Z. I enter Z6.9970 and then hit Measure (this is on a Fanuc).

Correction lest anyone have a crash because of what I wrote before: The tool length offset table entry for the Haimer has a 6.9970 value entered, but the offset is not active when I am touching off a G54 Z0.

 

[customcentric]

I've been scouring the web and came across this thread. I have been using a Haas with a probe for several years. Just recently got a used Quaser MF400U to add 5-axis capability to the shop. It's my 1st Fanuc and boy, what an enjoyable experience it is trying glean useful information from the manual(s).

I don't have a probe on this machine. I've set up the tool table with positive offsets using a master tool, including my Haimer. I set G54 with machine coordinates just like always. When I go to run a program the z-axis attempts to move UP and alarms out with z-axis soft-limit code.

If I reset all the tools using the negative offset method, the program runs fine. What am I missing? Is there a parameter I need to change to use positive tool offsets?

Any advice would be really helpful...I'm almost at full brain-lock.

-Chris

 

[customcentric]

Disregard, I figured it out after re-reading this thread 5 times. Need to negate the length of the Haimer after I touch off G54. Just one evening beverage and it came to me.