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

All things related to the Centroid Acorn CNC Controller

Moderator: cnckeith

swissi
Posts: 573
Joined: Wed Aug 29, 2018 11:15 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: 985DADEB24D5-0309180716
DC3IOB: No
CNC11: No
CPU10 or CPU7: No

Re: ProbeApp Official Release: Public Trial

Post by swissi »

Muzzer wrote: Wed Aug 05, 2020 3:15 pm 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.
The ProbeApp is using the same functions as CNC12 to set tool height offsets so I just can’t see how this statement can be true and this is why:

Your machine is a knee mill. On a knee mill the machine bed is not fixed and can be moved up and down and that means that the Reference Tool Method needs to be used to measure tool height offsets.

In your case, the reference tool is the Renishaw Touch Probe configured as tool #10. There's a Tool Touch Off installed on the machine bed that’s being used to set the Z Ref point with the TP and to measure the tools height offsets.

So maybe I’m missing something here and somebody can shed some light on this but if the Touch Probe is the Reference Tool and it’s being used to set the Z-Ref point, I just can’t see any options in which the height offset of the TP, which is tool #10 in the Offset library, would be something else than 0. The Z Ref and the Height Offset Position of the TP are exactly the same point so there can’t be any offset between them just by definition.

In your case the Touch Probe had an offset and I just can’t see how the CNC12 internal probing cycles would be able to set Z0 properly if the height offset of the Touch Probe in the Offset library is incorrect. I need to get more information from you of how exactly you did set the Z Ref point and what CNC12 internal probing cycles you used to get to the bottom of this.

For Mill and Routers that have a fixed distance between Z top and machine bed top, this works differently (so slotdat no need to be confused :-)). On those machines you can set CNC12 parameter 3 = 2 which tells CNC12 to set a fixed Z Ref point on top of the Z axis. So if you have a Tool Touch Off on the machine bed, CNC12 will store the distance from the top of Z to the position the Tool or Touch Probe is triggering the TT and the tool height offset is the difference between the TP and tool height values. So in this case the Height Offset of the TP is not 0.

As the last posts have confirmed, the Z Ref and Tool Height Offset subject is very confusing and not well documented in the CNC12 User Guide and I’ll post a separate thread on this subject as an information and discussion platform.

-swissi
If you are using Fusion 360, check out my CNC12 specific Post Processor
If you are using a Touch Probe, Tool Touch Off Device or a Triple Corner Finder Plate, check out my ProbeApp

Contact me at swissi2000@gmail.com
slodat
Posts: 793
Joined: Thu Apr 12, 2018 11:16 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: none
DC3IOB: No
CNC11: No
CPU10 or CPU7: No

Re: ProbeApp Official Release: Public Trial

Post by slodat »

I have a mill and a router. I was referring to how I am measuring tools and setting part zero on my knee mill.

I used this http://www.cncsnw.com/ToolHeightKneeMill.PDF and http://www.cncsnw.com/OLMProc1a.htm as a guide to setup my mill. This was the best explanation I found.
cncsnw
Posts: 3763
Joined: Wed Mar 24, 2010 5:48 pm

Re: ProbeApp Official Release: Public Trial

Post by cncsnw »

Slodat,

If you are following the procedure at http://www.cncsnw.com/OLMProc1a.htm, then the height offset value for your probe (e.g. H99) will be zero.

While my procedure suggests using T200 and H200 for the probe, there is no reason you cannot use T99 and H99, or any other pair. Just be sure to set Parameter 12 to match.
swissi
Posts: 573
Joined: Wed Aug 29, 2018 11:15 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: 985DADEB24D5-0309180716
DC3IOB: No
CNC11: No
CPU10 or CPU7: No

Re: ProbeApp Official Release: Public Trial

Post by swissi »

So for those being concerned about Muzzer's statement:
Muzzer wrote: Wed Aug 05, 2020 3:15 pm 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 can confirm that the problem was caused by incorrect Tool Offset values in the CNC12 Tool Geometry Offset Library based on a misinterpretation how the Z Ref function works on a knee mill that has a non-fixed machine bed. I will do a separate post on this subject as it is the cause for problems for many users.

So if your Tool Geometry Offset Library is setup correctly, the ProbeApp will do exactly what it's supposed to do. If anybody else is having issues, please report them here.

Another issue that came up is having invalid probe parameters configured. The ProbeApp is doing a thorough check of the probe configuration settings when it starts up and will report an error message if some of the parameters are outside the expected values. So if you get an error message when the ProbeApp starts up, your probe configuration is incorrect.

As an example, starting from version 4.20 of the Acorn CNC12 version, there shouldn't be anymore negative Probe Input numbers. If your Touch Probe Input Parameter 11 or the Tool Touch Off Input Parameter 44 is negative (e.g -50007), you need to re-configure your probes properly in the Wizard.

Please keep posting issues, questions, opinions and experiences with the ProbeApp here.

-swissi
If you are using Fusion 360, check out my CNC12 specific Post Processor
If you are using a Touch Probe, Tool Touch Off Device or a Triple Corner Finder Plate, check out my ProbeApp

Contact me at swissi2000@gmail.com
martyscncgarage
Posts: 9912
Joined: Tue Mar 28, 2017 12:01 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: Yes
Oak CNC controller: No
CNC Control System Serial Number: none
DC3IOB: No
CNC12: Yes
CNC11: Yes
CPU10 or CPU7: Yes
Location: Mesa, AZ

Re: ProbeApp Official Release: Public Trial

Post by martyscncgarage »

Swissi, some basic documentation/videos would go a long way. Its ok to moderate your videos, vocals are better than no vocals.

Based on all your efforts, you should charge a reasonable rate for your work. I can appreciate the "donation model" but I think it would be better to see you fairly charge a flat fee.

You clearly put a significant amount of effort into this project and you are certainly doing your best to support it.
Thank you for your contribution!
Marty
Reminder, for support please follow this post: viewtopic.php?f=20&t=383
We can't "SEE" what you see...
Mesa, AZ
Muzzer
Posts: 728
Joined: Mon Feb 19, 2018 2:52 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: 38D269594F9C-0110180512
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
Location: UK
Contact:

Re: ProbeApp Official Release: Public Trial

Post by Muzzer »

I have to say I'm having the devil of a job understanding this.

If I understand the manual correctly, Zref shouldn't change once you've set it within the setup>tool>offset lib>Zref, yet mine changes when I run setup>part>auto. If I put a piece of paper on top of my stock before probing to set Z0, Zref changes by the thickness of the paper. I wasn't expecting this.

Furthermore, the value of the length offset in the tool length offset table doesn't seem to affect anything I can see, with the exception of Swissi's ProbeApp. Is the active ref tool length offset actually stored elsewhere? I've changed it to all manner of random values manually in the table and nothing seems to be affected, either in CNC12's part setup or tool length offset measurement.

- If I run part setup for G54 Z0 with CNC12, the length offset of the ref tool in the table doesn't affect Zref
- If I run part setup G54 Z0 with Swissi's app, for some reason Zref varies by the length offset value of the ref tool in the offset table, hence my original post.
- And as I said, Zref also varies with the height of the workpiece without me changing either the knee height or the TT height. This is regardless of whether I use CNC or Swissi's app.

I'll take a video screenshot if you think I'm making this up.
cncsnw
Posts: 3763
Joined: Wed Mar 24, 2010 5:48 pm

Re: ProbeApp Official Release: Public Trial

Post by cncsnw »

Z Reference is maintained, internally, as a position in machine coordinates (a distance from Z Home).

The number that is displayed in the Offset Library for Z Reference is in local part coordinates. Therefore that number will change whenever you change the Z axis part zero, even as it continues to represent the same machine position.
swissi
Posts: 573
Joined: Wed Aug 29, 2018 11:15 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: 985DADEB24D5-0309180716
DC3IOB: No
CNC11: No
CPU10 or CPU7: No

Re: ProbeApp Official Release: Public Trial

Post by swissi »

The confusing part with Z Ref and Tool Height Offsets is that there are different methods based on the type of machine you have.

So not to confuse others, the method I’m going to describe is for knee mill type machines that have a non-fixed machine bed. For this type of machine, the Reference Tool Method needs to be used.

Let’s start with the Z Ref function.

S6.PNG

The Z Ref[F1] function does set the reference point along the Z Axis at which the Reference Tool has touched the Reference Surface. The Z Ref value that’s being displayed is not in machine coordinates, it’s the actual offset of the Z0 point of the currently active WCS# and the Z Ref point. If you reset Z0 to another position, the displayed Z Ref position will change. I don’t know where in the manual you have read that the displayed Z Ref position should not change as this is definitely not the case.

In your case you are using the Renishaw Touch Probe (TT), which is configured on your system as Tool T10 with the height offset H10, to set the Z Ref point on top of the Electronic Tool Setter (ETS) which is positioned on top of the machine bed. That means the TP is your Reference Tool and all other tools will be measured by the difference of the length of the TP compared to the length of the tool.

So by using Z Ref[F1] to touch off your TP on top of the ETS, you have established the reference point along the Z Axis from which the length offsets of all tools will be measured. The displayed Z Ref value will be the distance from the Z0 point of the currently active WCS to the top of the ETS.

Now let’s move on to set the Height offsets of the tools:

S7.PNG

Because your TP, which is T10 H10, is the Reference Tool from which the length offsets of all the other tools is calculated, the Height Offset H10 MUST be 0 as this is basically the same position as the Z Ref point and the Z Ref point can’t have any offsets to itself.

If you now touch off all your tools with the “Auto Measure[F3]” function, the “Tool Geometry Offset Library” will record all the tool height offsets compared to your TP.

If you need to add another tool to the offset library at a later point, you have to establish a new Z Ref point first by using Z Ref[F1] to touch off the TP on top of your ETS. In theory you can place the ETS anywhere along the Z Axis to establish the new Z Ref point. If your machine bed is so far down that the quill can’t reach the ETS on top of the machine bed, you can lift the ETS up on top of the vise or somewhere else. As long as you establish a new Z Ref point with the TP on top of the ETS at that position, the measured tool offset done with “Auto Measure[F3] will record the correct offset.

So just to be absolutely clear: The Z Ref point is only used to establish a reference point along the Z Axis from which the length difference between the TP and the tool can be measured. The Z Ref point has absolutely no function during a job execution.

Now how does CNC12 know how to adjust the WCS Z0 point based on the length of the tool?

When you set the WCS Z0 point with the TP, CNC12 knows that the height of that point is relative to the length of the TP which in your case has a height offset of 0 because it’s the Reference Tool. From this point, CNC12 knows how to adjust the WCS Z0 point based on the height offset of each tool compared to the TP.

So let’s put this to the test.

Let’s assume this is the Tool Geometry Offset Library:

S12.PNG

If you set a WCS Z0 point with your TP, you will see that Tool T10 is active with the Height Offset H10 activated and the WCX is set to Z0:

S8.PNG

Now if you turn off Tool Height Compensation with G49, you will see that H10 is no longer active but Z is still at Z0 because the height offset H10 is 0:

S9.PNG

If you now load T1 with the Height Offset H1, you will see that the Z position has changed by the length of 3.215 because H1 is 3.125 shorter compared to H10:

S10.PNG

If you turn off Tool Height Compensation with G49, you see that T1 is still loaded but H1 height offset has been deactivated and the Z position went back to Z0.
S11.PNG

I hope this makes it clearer and I encourage anybody to jump in if you think something here is incorrect or if there are more questions.

-swissi
If you are using Fusion 360, check out my CNC12 specific Post Processor
If you are using a Touch Probe, Tool Touch Off Device or a Triple Corner Finder Plate, check out my ProbeApp

Contact me at swissi2000@gmail.com
Muzzer
Posts: 728
Joined: Mon Feb 19, 2018 2:52 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: 38D269594F9C-0110180512
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
Location: UK
Contact:

Re: ProbeApp Official Release: Public Trial

Post by Muzzer »

Hi Swissi
?
You say "Because your TP, which is T10 H10, is the Reference Tool from which the length offsets of all the other tools is calculated, the Height Offset H10 MUST be 0 as this is basically the same position as the Z Ref point and the Z Ref point can’t have any offsets to itself."

Yet as I said previously, I am able to set ANY value I like into the offset for T10 in the offset table and it makes not the slightest difference to anything. Have you tried it for yourself? In which case, where is the Z Ref offset actually stored?

It seems a bit sneaky / confusing that the Zref displayed is in the current WCS, whereas the calculation is based on machine coords. If you change working WCS, it doesn't change or invalidate the offsets of the other tools, or the process for acquiring them.
swissi
Posts: 573
Joined: Wed Aug 29, 2018 11:15 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: 985DADEB24D5-0309180716
DC3IOB: No
CNC11: No
CPU10 or CPU7: No

Re: ProbeApp Official Release: Public Trial

Post by swissi »

Muzzer wrote: Fri Aug 07, 2020 3:21 pm Hi Swissi
?
You say "Because your TP, which is T10 H10, is the Reference Tool from which the length offsets of all the other tools is calculated, the Height Offset H10 MUST be 0 as this is basically the same position as the Z Ref point and the Z Ref point can’t have any offsets to itself."

Yet as I said previously, I am able to set ANY value I like into the offset for T10 in the offset table and it makes not the slightest difference to anything. Have you tried it for yourself? In which case, where is the Z Ref offset actually stored?

It seems a bit sneaky / confusing that the Zref displayed is in the current WCS, whereas the calculation is based on machine coords. If you change working WCS, it doesn't change or invalidate the offsets of the other tools, or the process for acquiring them.
Did you read the whole post? Why do you even care where the Z Ref point is stored? I explained in my post how and when to set the Z Ref Point and what it is used for. Sorry but I just can't explain it any better.
Muzzer wrote: Fri Aug 07, 2020 3:21 pm Yet as I said previously, I am able to set ANY value I like into the offset for T10 in the offset table and it makes not the slightest difference to anything. Have you tried it for yourself? In which case, where is the Z Ref offset actually stored?
Yes I have tried it and if you follow the examples in my post you will see that your statement above is wrong. Just entering a H10 value in the Tool Geometry Offset Library doesn't show any visible effect in the table but it does change how CNC12 calculates the length difference (height offsets) between your TP and the Tools.

To prove that, do the following steps:
  • Make sure H10 in your offset library is 0
  • Set WCS Z0 with the TP on any surface
  • CNC12 will now display T10 H10 and the DRO shows Z0
  • Do a G49 in the MDI to turn off Tool Height Compensation and CNC12 will show T10 H-- and the DRO still shows Z0 because H10 is 0
  • Go back into the Tool Geometry Offset Library and change H10 to 20 and Save the new setting
  • Now repeat the above steps again and compare the results with the results from before
Please report back if you still think it doesn't matter what height offset the TP has.

-swissi
If you are using Fusion 360, check out my CNC12 specific Post Processor
If you are using a Touch Probe, Tool Touch Off Device or a Triple Corner Finder Plate, check out my ProbeApp

Contact me at swissi2000@gmail.com
Post Reply