Struggling with Probing

[Steve Geth]

Hi all,

I set up my CNC knee mill with two probes. A material/ part probe and a tool setter probe. I am having a hard time grasping the setup for Z probing and tool length offset and hoping someone can explain what I am doing wrong.

Here are my steps:

Home the machine.
Set the tool offset for the probe (tool #16) to 0.
Move the axes over a hard block that is the exact height of the tool setter.
Using a simple one line code, Z- until the probe is triggered.
Press F1 (Fagor Control), then Z, then Enter, then Esc to set the tool length for the probe.
Move the axes above the mounted material and run a Z probing program that does a material touch off and sets G54.
ISO G54 to make the tool active.
T1 cycle start to move the axes to the tool change position
Change to the first cutting tool, cycle start to accept the new tool
Run a probing program that moves the axes such that the tool is above the tool setter, slowly moves down until triggered, I hit F1, then Z Enter, then escape to set the new tool length.

Fundamentally, everything works, but the numbers that I see are confusing me.

With the material probe (tool 16) from Z 0 to the hard block I get Z-1.97 (which I set as the tool length). I then move to the mounted material and Z down and get Z- 1.52 to the material surface and G54 reads .450 which makes perfect sense indicating that the material is .450 higher then the hard block and tool setter. I then ISO G54 to make the tool active and the Z DRO changes to 0 which also makes sense.

Now, I change to tool #1 and run the tool setter program. When the tool setter is triggered, I again hit F1, Z, then Enter, then Esc to set the new tool length. The tool length for that tool now shows Z- 2.65. When I look at the Z scale on the spindle, it shows -2.20 I recognize that 2.65 less .450 is 2.20.

My confusion is this: My thinking is that whatever the value is for the tool length of a given tool in the tool offset table, I should be able to start at Z 0, (Z fully retracted) go to ISO and enter that -Z number and cycle start and the tool tip should be at the material surface. Is my thinking incorrect?

if I were to do the above starting from Z0, the tip of the tool would be at the tool setter height, not the material surface which is .450 higher.

Please let me know if I am doing something wrong, or not thinking this correctly.

Thanks,

Steve

 

[13engines]

Not familiar with Fagor but can offer some generic advise.

When using a tool setter, you will always have a value in G54 Z (or whatever Offset you're using) while doing your work.

The only thing I can see that may be throwing you for a loop is you should not have any Z value active in a work offset, as it seems to affect your tool measurements. You want your tools measured under the exact same circumstances as your probe. After you've measured you're probe and all your tools, then measure the stock with the probe and leave whatever value it gives in the G54 Z register. You're now free to go about machining the work. All tools should behave offset wise.

Sorry if I didn't understand your problem correctly, but hope some or all of this helps.

 

[Steve Geth]

Not familiar with Fagor but can offer some generic advise.

When using a tool setter, you will always have a value in G54 Z (or whatever Offset you're using) while doing your work.

The only thing I can see that may be throwing you for a loop is you should not have any Z value active in a work offset, as it seems to affect your tool measurements. You want your tools measured under the exact same circumstances as your probe. After you've measured you're probe and all your tools, then measure the stock with the probe and leave whatever value it gives in the G54 Z register. You're now free to go about machining the work. All tools should behave offset wise.

Sorry if I didn't understand your problem correctly, but hope some or all of this helps.

I think I understand. I should have the material probe in the spindle, probe the hard block (which is the same exact height as the tool setter probe).

Remove the material probe, and one by one measure each of the tools to the tool setter. Then, when all tools have been measured, reinstall the material probe and probe the material surface, and set the G 54 for Z and then activate. Does that sound right, or am I misunderstanding?

Thanks.

 

[rjwalker1973]

When you set your tools like you are now and run a program does the tool go to the programmed position in Z? As in if you tell tool 5 to go to g54 z1.0 will it go to 1.0 above where you have z0 set?

 

[Steve Geth]

When you set your tools like you are now and run a program does the tool go to the programmed position in Z? As in if you tell tool 5 to go to g54 z1.0 will it go to 1.0 above where you have z0 set?

That’s an excellent question. I am extremely new at this, as in just getting started. I had not thought to try that, but will do so when I am back at my machine on Thursday. I have touched off tools from the material surface using a piece of paper, the old-school way, and that works just fine, but I am trying to implement the use of the probes and since I don’t have a tool changer, ultimately would like sub routines that do the tool setter touch offs during
the part program. Thanks for your help.

 

[sinha]

I think I understand. I should have the material probe in the spindle, probe the hard block (which is the same exact height as the tool setter probe).

Remove the material probe, and one by one measure each of the tools to the tool setter. Then, when all tools have been measured, reinstall the material probe and probe the material surface, and set the G 54 for Z and then activate. Does that sound right, or am I misunderstanding?

Thanks.

This is fundamentally correct.
Now, verify if the tools are placed to correct heights when using the same WCS and incorporating length offsets.

 

[sinha]

That’s an excellent question. I am extremely new at this, as in just getting started. I had not thought to try that, but will do so when I am back at my machine on Thursday. I have touched off tools from the material surface using a piece of paper, the old-school way, and that works just fine, but I am trying to implement the use of the probes and since I don’t have a tool changer, ultimately would like sub routines that do the tool setter touch offs during
the part program. Thanks for your help.

After every new offset setting, it is a safe practice to check if the tools do come to the expected position. This may take a few minutes, but will ensure that there would be no crash due to an inadvertent error in offset setting.

 

[Jatrox]

They are separate procedures. Same action but info is stored and used differently. Set all the mounted tools first. That info shouldn't change. The G54 (or whatever you use) will change with every piece of stock you mount. A good habit for newbies is, after setting G54 run a tool down to 1" above the stock and check it with a gauge block to confirm correct position before running the program.

 

[sinha]

That info shouldn't change

Wear value may need slight adjustment for some tools, over a period of time.

 

[Steve Geth]

They are separate procedures. Same action but info is stored and used differently. Set all the mounted tools first. That info shouldn't change. The G54 (or whatever you use) will change with every piece of stock you mount. A good habit for newbies is, after setting G54 run a tool down to 1" above the stock and check it with a gauge block to confirm correct position before running the program.

Got it, thank you..

 

[13engines]

I think I understand. I should have the material probe in the spindle, probe the hard block (which is the same exact height as the tool setter probe).

Remove the material probe, and one by one measure each of the tools to the tool setter. Then, when all tools have been measured, reinstall the material probe and probe the material surface, and set the G 54 for Z and then activate. Does that sound right, or am I misunderstanding?

Thanks.

Yes that sounds good.
I'm not familiar with your Fagor setup and how things are handled when you move the knee up or down. But like I said earlier, as long as the probe and all tools are measured under the same circumstance, they should always directly relate to one another. So after establishing a new Work height Z offset, all your tools should still play nice. The trick is to not get caught out by having a left over Z setting somewhere that affects a new reading or tool setting.

 

[Steve Geth]

Yes that sounds good.
I'm not familiar with your Fagor setup and how things are handled when you move the knee up or down. But like I said earlier, as long as the probe and all tools are measured under the same circumstance, they should always directly relate to one another. So after establishing a new Work height Z offset, all your tools should still play nice. The trick is to not get caught out by having a left over Z setting somewhere that affects a new reading or tool setting.

The knee is a whole other issue. It is currently not a part of the axes controlled by the CNC. Since I only have about 4" of quill travel, I may add this as an additional axis someday, but for now I will manage. I understand everything all of you knowledgeable folks have posted, but your last sentence regarding a left over Z setting somewhere has me confused. How would I know if this is the case and where would I look? If I have only used G54 for Z so far and none of the other available work offsets and I set a new G54 based upon a new piece of material, could there still be a "left over Z setting somewhere"?

 

[sinha]

I have only used G54 for Z so far and none of the other available work offsets and I set a new G54 based upon a new piece of material

If every new workpiece is different, you may use G54 for all of them, after re-defining it.
However, if there are sets of similar workpieces, it would be more convenient and time-saving, if a different WCS is defined for each set. If there are more than six sets, additional WCSs (G54.1 on Fanuc), an optional feature of the control, can be used. Of course, one has to keep track of which WCS to use for which set.

 

[Steve Geth]

If every new workpiece is different, you may use G54 for all of them, after re-defining it.
However, if there are sets of similar workpieces, it would be more convenient and time-saving, if a different WCS is defined for each set. If there are more than six sets, additional WCSs (G54.1 on Fanuc), an optional feature of the control, can be used. Of course, one has to keep track of which WCS to use for which set.

I thought that this is what was meant with the statement. So, for now with individual and separate work pieces, It seems that it wouldn't apply, but as I develop skills and do more advanced things it can/will come into play. Thanks..

 

[sinha]

The advantage with G54 is that it is also the default (on Fanuc, and possibly on other controls also). So. if you forget to explicitly command it in the beginning of the program, the program would still run as intended.

 

[13engines]

It's really hard to say anything for sure without seeing and knowing what your system looks like. In your original post it seemed like your numbers where being affected by your early entry of the workpiece height into the G54 Z register. Let's just say that my comment was to suggest that anytime you start a new work height measurement, zero out G54 Z before entering the new. one. I don't even know if your probe automatically enters the number for you like it would on a standard CNC machine, or if it only stops the machine and you read a number off the screen and enter it manually. All these differences and unknowns sort of affect the comments a person can give.

 

[rjwalker1973]

The advantage with G54 is that it is also the default (on Fanuc, and possibly on other controls also). So. if you forget to explicitly command it in the beginning of the program, the program would still run as intended.

On our Haas's it is the last used workoffset. If you last used g55 it remains the workoffset until you change it. I thought it was modal on Fanuc as well?

 

[sinha]

On our Haas's it is the last used workoffset. If you last used g55 it remains the workoffset until you change it. I thought it was modal on Fanuc as well?

It is modal, but a modal data applies to the same program. Once the control is RESET, manually or by M02/M30, all modal codes revert back to the default ones on Fanuc. The only exception is G20/G21 where the last-used code continues also in the next program or the next machining session. There is no default code in this case.

If the last used WCS remains active even in a new program or a new machining session, it is a good design, I would say. It would have prevented an accident on one of my machines several years back when a program was terminated in the middle and re-started from that point without inserting G56. The execution started with G54 !

 

[rjwalker1973]

It is modal, but a modal data applies to the same program. Once the control is RESET, manually or by M02/M30, all modal codes revert back to the default ones on Fanuc. The only exception is G20/G21 where the last-used code continues also in the next program or the next machining session. There is no default code in this case.

If the last used WCS remains active even in a new program or a new machining session, it is a good design, I would say. It would have prevented an accident on one of my machines several years back when a program was terminated in the middle and re-started from that point without inserting G56. The execution started with G54 !

our lathes subspindles use g55 and the younger guys could not figure out why when they was replacing a tool on the main(g54) spindle they wasn't touching off correctly. It was because it was still in G55. You have to go into MDI and manually input G54 to reset the workoffset so it will take the tool touchoff correctly. Thats why I preach best practice of calling your workoffset and the spindle callout (g14/g15)at the beginning of every tool. One guess why I do that

 

[Freedommachine]

The knee is a whole other issue. It is currently not a part of the axes controlled by the CNC. Since I only have about 4" of quill travel, I may add this as an additional axis someday, but for now I will manage. I understand everything all of you knowledgeable folks have posted, but your last sentence regarding a left over Z setting somewhere has me confused. How would I know if this is the case and where would I look? If I have only used G54 for Z so far and none of the other available work offsets and I set a new G54 based upon a new piece of material, could there still be a "left over Z setting somewhere"?

I would like to touch on a few things that others have mentioned and add a bit more.

1.) Tools that are fixed in holders should not change in length unless you remove the cutter from the holder. (Yes, tool wear is different, but lets forget about that for now.)

Lets say I set up a 1/4" end mill in an ER16 holder. I will call that tool #2, touch it off and enter it's length on the tool offset page - let's call it + 3.000".

Now, I set up a different job on the mill that requires me to crank the table down to an unknown distance - as long as I have not removed that end mill from that ER16 holder - I will be able to run that tool again in my new program without resetting it's length.

2.) Building on the information above; the length of your material touch probe never changes; unless you physically change it by replacing the stylus. Setting the probe length is technically a calibration; once it's length is known, do not change it.

3.) Your tool length offsets should be positive numbers; they should reflect the actual, physical gauge length of each tool.

4.) Because the knee moves up and down, the actual distance from Z home, to the tool setter, will change frequently. This is the number that you will want to update each time you move the knee.

Each time the knee is moved for a new job, begin by probing that block like you were doing but, instead of updating the probe length; you will update the distance from z home to the tool setter trigger point.

Does this make sense?

Where does your machine store the offset location data for that tool setter?

We can cover how to find the actual gauge length of the probe next.