ProbeApp Official Release: Public Trial ***EXPIRED***

[Muzzer]

Ran a job yesterday and thought it would be a great chance to try out the probing app for real, rather than play with it.

I set up my workpiece X and Y using the probe app and this worked fine - nice and slick, very happy. Then I used it to set the top of the workpiece, using the Renishaw probe as before. But when I then changed tools, they all ended up almost 35mm off kilter. If I'd run the job, I'd have crashed the tool and toolholder into the workpiece. Something wasn't right.

I reprobed the Z coordinate using the CNC12 built-in work probing function (as I was accustomed) and ended up with the right offsets - I ran the job without crashing.

Not sure what I did wrong here. Hopefully it will be blindingly obvious.

The error is the same value as the offset shown for my Renishaw probe (T10).

This is a turret mill with a fixed (to the table) TT type electronic tool setter.

Report attached

report_38D269594F9C-0110180512_2020-08-03_18-40-59.zip

(627.37 KiB) Downloaded 118 times

[swissi]

Ran a job yesterday and thought it would be a great chance to try out the probing app for real, rather than play with it.

I set up my workpiece X and Y using the probe app and this worked fine - nice and slick, very happy. Then I used it to set the top of the workpiece, using the Renishaw probe as before. But when I then changed tools, they all ended up almost 35mm off kilter. If I'd run the job, I'd have crashed the tool and toolholder into the workpiece. Something wasn't right.

I reprobed the Z coordinate using the CNC12 built-in work probing function (as I was accustomed) and ended up with the right offsets - I ran the job without crashing.

Not sure what I did wrong here. Hopefully it will be blindingly obvious...

Muzzer,
I can't tell based on the information given and the two screen shots what went wrong here and I'll send you an email to get more information.

What I can tell you is that I have used the probing function you described hundreds of times with the ProbeApp and it worked as expected every single time.

The ProbeApp uses the Probe Tool Number and Height Offset as configured in CNC12, so the WCS Z0 point will be set based on the configured Height Offset of the Probe. Now when you change the tool, the Height Offset of the active tool will be activated and if the Z0 point of the active tool is different from the Z0 you measured with the probe, that can only mean that the tool height offsets in your CNC12 Tool Offset Library are not properly setup.

Look out for my email and let's get to the bottom of this.

-swissi

[carbuthn]

Muzzer & Swissi,

I have used the ProbeApp about 50 times, it has worked very well for me, but it sounds like Muzzer may be running into something that I experienced.

In my setup my probe (Hallmark ITTP) is assigned to Tool #10, I put it into my mill and used the tool setter in ProbeApp to measure the touch probe. I then went through all of the tool holder and used the auto measure to measure the offsets of each tool.

When I put a piece of stock into the vise I used the 3 axis probe cycle to measure the stock and setup zero location for X, Y & Z axis. I changed the Tool out in the quill, but DID NOT use the MDI to command the tool change (i.e. CNC12 still thinks it has the tool setter), when I lowered the new tool it didn't have the correct offset applied. When I ran a program that called for a tool change it new tool had the correct Z height and cut as it should.

Just a guess, but it sounds like what I saw, and not an issue if you tell CNC12 which tool you are using.
Chuck

[martyscncgarage]

Muzzer & Swissi,

I have used the ProbeApp about 50 times, it has worked very well for me, but it sounds like Muzzer may be running into something that I experienced.

In my setup my probe (Hallmark ITTP) is assigned to Tool #10, I put it into my mill and used the tool setter in ProbeApp to measure the touch probe. I then went through all of the tool holder and used the auto measure to measure the offsets of each tool.

When I put a piece of stock into the vise I used the 3 axis probe cycle to measure the stock and setup zero location for X, Y & Z axis. I changed the Tool out in the quill, but DID NOT use the MDI to command the tool change (i.e. CNC12 still thinks it has the tool setter), when I lowered the new tool it didn't have the correct offset applied. When I ran a program that called for a tool change it new tool had the correct Z height and cut as it should.

Just a guess, but it sounds like what I saw, and not an issue if you tell CNC12 which tool you are using.
Chuck

That statement seems to bite most a time or two. After a crash, we seem to get it.
GOT to tell CNC12 WHICH tool is in the spindle when you set Part Zero.

[swissi]

... GOT to tell CNC12 WHICH tool is in the spindle when you set Part Zero.

Unless you have a spindle with non-fixed tool holders it is even more important to make sure the correct tool height offset is activated when you set WCS Z0. In this example, tool 10 (Touch Probe) is loaded but no height offset has been activated:

S1.PNG (9.23 KiB) Viewed 3075 times

After a

Code: Select all

G43 H10

it will look like this:

S2.PNG (9.33 KiB) Viewed 3075 times

To make matters even more complicated, the CNC12 Tool Library does allow to change the Tool Height Offset and Diameter Offset number of a tool:

In the example above, Tool #11 has a Height Offset H99 and Diameter Offset D99. Never ever do this unless you have a very, very good reason to do so. However, even when you do it, ProbeApp will always get the correct H and D offsets of a tool as they are configured in the Tool Library.

The Tool Height Offsets between the Touch Probe and all the Tools must be correct, otherwise setting WCS Z0 with the Touch Probe will not work properly.

-swissi

[Muzzer]

Pleased to say that Swissi quickly got to the bottom of the issue. My mistake was having a non-zero tool length offset for my reference tool T10, which in my case is a Renishaw probe, also used for probing. If you lack the intellect to understand why it would be a bad idea, it's possible to measure the tool length of the probe on the tool setter and save that to the reference tool as a tool length offset.

So I manually reset the offset of T10 to zero in the tool length offset table, which of course now requires me to remeasure all of the tools. I suppose I could manually adjust them in the table to save the hassle but I often remeasure them before running a job after being away for a while anyway. Now the tool length offsets all work as intended and the probe app agrees with the CNC12 native probing functions.

As I seem to share the workshop and machines with a clumsy congenital idiot(!!), I like to double check the tool length offsets of the tools before running a job, not least as I often end up mounting new tools. It seems you can never have enough toolholders. So I run G43 H03 (for tool 3 etc) in MDI, jog the tool down close to the workpiece and then slowly jog it upwards until I can roll a broken 10mm tool under the tool. On a good day, this would show Z10 in G54 and give me confirmation that the offsets are sensible.

Perhaps Swissi can comment but the lesson seems to be - ensure the tool length offset for the ref tool is zero. It may be obvious to many but that one passed me by, so may be worth stating.

[slodat]

Ok.. now I'm confused. My touch probe has a non-zero offset in the tool library and this is how I am setting my part zero. It is working correctly this way. If my touch probe (T99) has a zero offset, how will this all work?!

[cncsnw]

It should not matter whether the offset value for the probe is zero or non-zero. If your tool measuring procedure involves setting Z Reference using the probe, then its offset will be zero. If you use some other way of setting Z Reference, then when you measure the probe, its height offset will be non-zero.

As long as the software which sets Z axis Part Zero using the probe accounts for the probe's height offset, then it will get the right answer.

[martyscncgarage]

It should not matter whether the offset value for the probe is zero or non-zero. If your tool measuring procedure involves setting Z Reference using the probe, then its offset will be zero. If you use some other way of setting Z Reference, then when you measure the probe, its height offset will be non-zero.

As long as the software which sets Z axis Part Zero using the probe accounts for the probe's height offset, then it will get the right answer.

For instance, on my mill, I have set the control to use Z home as the Z reference point. The probe will be like any other tool, it will have an offset value, in my case the distance from Z home. I use Z home because I have servos, when the machine homes, it uses the mechanical switch to get close and the Z servo motor index pulse to get precise.

Marty

[Muzzer]

Well, perhaps it's due to the way Swissi implemented his probing functions. My system always worked fine using the native Centroid functions and a non-zero offset for the probe - but running Swissi's probing app seems to require the zero offset. If you plan to use both interchangeably, it seems that you need to use zero offset to avoid issues, which could result in crashes.

I'm sure Swissi understands better than me but it sounds to me like something we need to explain and understand clearly.

Perhaps someone else would like to try setting WCS Z0 using the original work probing function (with a non-zero offset for the ref tool), then follow up using the probe app to measure the same Z0. Watch the Z coordinate in G54 and see how they compare before and after running the app.