Probing Macros for Solidworks/Camworks use

All things related to the Centroid Acorn CNC Controller

Moderator: cnckeith

Post Reply
Deon
Posts: 52
Joined: Thu Jan 25, 2018 1:13 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: Yes
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: AllinOne cncm system ID: 0625181998 / XE3HFDFJBI
Acorn/Leadshine 4axis bench mill: 3403DE6C0783-01919192476
Acorn/Gecko G540 Sherline Lathe: 0479B7B00885-1107192659

Probing Macros for Solidworks/Camworks use

Post by Deon »

I am not sure how to word this. I am working with a person who wrote me a Post Processor so I can use SolidWorks/CamWorks CAM. It works and since CamWorks has a probing ICON I should be able to CAM the probe tool to do a function into the process.
Here is what I would like to do. I would program the probe in the CAM to find the stock center or a corner to set the WCS. Then do some removal of the stock in one side of the stock for operation1. The probe is called and the stock is re-positioned the cycle start is pressed, the probe finds the WCS from a feature to begin the removal of stock for operation 2. Then the same for Operation 3 and so on.

Is the Centroid control able to perform the functions needed? Or what info do I need to pass on to the person that is assisting me in trying to make it happen. Below is a reply I received form him that asks me for info and not sure where to direct him to. Thanks in advance.


Currently, CAMWorks Probing is designed around the Renishaw Inspection Plus probing system. I do not know which probing system you have nor which probing system the Centroid controller uses. I do know since your machine is a retro fit with this controller, I have concerns on if the machine and controller is configured to do probing. Additionally, the probing output essentially calls macro programs that are preloaded and configured on your machine. So that means you must have those macro programs preloaded and configured on your machine where it has all the necessary behind the scenes macros set and the probe wired and calibrated. Typically machine representatives come in and add this into the machine. Has your machine done that and have this ability? I would suggest hand writing a program to verify that and see if and how it runs. Just because the controller can do it, don't mean the machine can and is configured to do so.

I would need all the documentation that illustrates all the probing cycles that it offers, with a description of each parameter that needs set. Then we would review it and the compatibility between CAMWorks probing and then quote it accordingly. I'm not sure what this will take without seeing all the documentation on probing cycles and programs that run on this machine... but I've done probing on other machines where it can take a good day to write and implement into the post and I've done ones where it's taken 4-5 weeks. So what I'm saying is this could get rather involved.

For what it is worth, the functionality that CAMWorks is supporting for probing is that of a spindle touch probe, not to be confused with tool setters and it is currently only on mill machines. The probing cycles supported are:
• Single Surface (XYZ)
• Web/Pocket with or without island
• Boss with or without island
• Bore with or without island
• 3 point boss with or without island
• 3 point bore with or without island

In these above cycles are currently only supporting the ability to set the work coordinate fixture offsets (such as G54, G55, G54.1 P1, etc).

If you can gather up sample program that runs successfully and probes a part on your machine, a manual that illustrates each probing cycle and parameters, I can review it on my end to check for compatibility with CAMWorks.
Deon Daugherty
GOD, Country, Family
swissi
Posts: 509
Joined: Wed Aug 29, 2018 11:15 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: 985DADEB24D5-0309180716

Re: Probing Macros for Solidworks/Camworks use

Post by swissi »

Deon wrote: Thu Nov 18, 2021 5:14 am
For what it is worth, the functionality that CAMWorks is supporting for probing is that of a spindle touch probe, not to be confused with tool setters and it is currently only on mill machines. The probing cycles supported are:
• Single Surface (XYZ)
• Web/Pocket with or without island
• Boss with or without island
• Bore with or without island
• 3 point boss with or without island
• 3 point bore with or without island
I have done this for Fusion 360. It requires a Post Processor that actually supports the Probing functions. (Fusion 360 Probing Guide)

Are you sure your Post Processor actually creates probing output?

The Post Processor will just generate code that will call the Renishaw probing subprograms like this:

Code: Select all

(PROBE WCS Y-SURFACE)
N30 T10 M06
N35 G54
N40 G00 A0.
N45 G00 X9.117 Y-5.5
N50 G43 Z15. H10
N55 G65 P9832
N60 G65 P9810 Z5. F1000.
N65 G65 P9810 Z-12.
N70 G65 P9811 Y0. Q2. M1. W1. S1.
N75 G65 P9810 Z5.
N80 G00 Z15.
N85 G65 P9833
These subprograms do not exist for Centroid and I had to create them. I also had to modify the subprogram calls from the Post Processor a little to make them compatible with the way CNC12 works with parsed parameters. As an example, there's no way to differentiate if a parsed parameter is 0 because the parameter was omitted from the subprogram call or had an actual value of 0.

I do not have access to Solidworks so please do a quick test and design a rectangular part and create the probing cycles to set WCS X0 Y0 Z0 on the front left corner of the part and put it trough the Post Processor. Post the output here or email it to me (email address down in my signature).

BTW did you have a look at my ProbeApp? I found it is much quicker and easier to use the ProbeApp to set WCS 0 rather than creating the Probing Tool-paths in the CAM system.

-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
Deon
Posts: 52
Joined: Thu Jan 25, 2018 1:13 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: Yes
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: AllinOne cncm system ID: 0625181998 / XE3HFDFJBI
Acorn/Leadshine 4axis bench mill: 3403DE6C0783-01919192476
Acorn/Gecko G540 Sherline Lathe: 0479B7B00885-1107192659

Re: Probing Macros for Solidworks/Camworks use

Post by Deon »

Hi Swissi,

I do have you latest probe app. It works great when programing in CNC12. I just viewed the fusion tutorials on probing and that is what I am hoping to do. Especially for more than one operation. So, how or what did you have to do to the Centroid program to make this happen? I use the Royal Quick change tooling for my tool holders.

This is the Post output for finding X,Y,Z and got no error until I got to Probe OP 3.

; OPERATION NAME: PROBE OPERATION1

;TOOL 200, N-5000-3603-00-D Touch Probe
N10 G00 G17 G20 G94
N15 G40 G49 G80 G90
N20 H0 M25
N25 G00 X0. Y0. ;TOOL CHANGE POSITION
N30 T200 M06
N35 S0 M05
N40 G54 G00 G90 X0. Y0.
N45 G43 H200 Z1. M08
N50 G04 P3.
N55 G01 Z.1968 F.6
N60 Z.0984
N65 Z.1968
N70 Z1.
; OPERATION NAME: PROBE OPERATION2
N75 Z.1968 F3.94
N80 Z1.
N85 M09
N90 M05
N95 H0 M25
N100 G00 X0. Y0. ;TOOL CHANGE POSITION

Then Centroid does the removal of the unneeded stock.

; OPERATION NAME: PROBE OPERATION3

;TOOL 200, N-5000-3603-00-D Touch Probe
N7740 G40 G49 G80 G90
N7745 T200 M06
N7750 S0 M05
N7755 G54 G00 G90 X0. Y0.
N7760 G43 H200 Z1. M08
N7765 G04 P3.
N7770 G01 Z.1769 F3.94
N7775 Z-.1
N7780 Z.1769
N7785 Z1.
N7790 M09
N7795 M05
N7800 H0 M25
N7805 G00 X0. Y0. ;TOOL CHANGE POSITION
N7810 M00 ;MANUAL TOOL CHANGE - CHANGE TO: T12


This is where when graphing on Centroid I got errors. I will attach the entire file via email for your inspection.



Thank You,
Attachments
Inline Carb Adapter II.TXT
(56.12 KiB) Downloaded 4 times
Deon Daugherty
GOD, Country, Family
swissi
Posts: 509
Joined: Wed Aug 29, 2018 11:15 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
MPU11 & GPIO4D -w/ 3rd Party Drives: No
DC3IOB: No
CNC11: No
CPU10 or CPU7: No
CNC Control System Serial Number: 985DADEB24D5-0309180716

Re: Probing Macros for Solidworks/Camworks use

Post by swissi »

Deon wrote: Fri Nov 19, 2021 6:02 am ...
This is the Post output for finding X,Y,Z and got no error until I got to Probe OP 3.

; OPERATION NAME: PROBE OPERATION1

;TOOL 200, N-5000-3603-00-D Touch Probe
N10 G00 G17 G20 G94
N15 G40 G49 G80 G90
N20 H0 M25
N25 G00 X0. Y0. ;TOOL CHANGE POSITION
N30 T200 M06
N35 S0 M05
N40 G54 G00 G90 X0. Y0.
N45 G43 H200 Z1. M08
N50 G04 P3.
N55 G01 Z.1968 F.6
N60 Z.0984
N65 Z.1968
N70 Z1.
; OPERATION NAME: PROBE OPERATION2
N75 Z.1968 F3.94
N80 Z1.
N85 M09
N90 M05
N95 H0 M25
N100 G00 X0. Y0. ;TOOL CHANGE POSITION

Then Centroid does the removal of the unneeded stock.
...
The Operation is called "PROBE OPERATION" but if you look at the actual G/M-Commands that the Post Processor generated you will notice that there's no probing going on here. This is just called PROBE OPERATION because the "tool" is called PROBE. There's even a M08 command in there that's turning on the Flood Coolant which you probably don't want when the probe is in the spindle.

I never used Solidworks and I have no idea how Solidworks generates Probing Tool Paths but if you have used the Probing Function correctly, then it looks like that the Post Processor you are using does not support them as the generated output is just a regular tool path and does not include any necessary probing moves that would actually set WCS 0.

If somebody is out there that has a Post Processor for Solidworks that works with CNC12 and does support the Probing Functions, please chime in.

-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