2.0 measures the tool before you start the program and then measures the new tool only at tool change in which case, yes the PP can be modified to show new tool number.
I think this would be the relevant section in the PP:
±--------------------------------------------------
- Commands output at toolchange
±--------------------------------------------------
begin TOOLCHANGE
“G0[ZH]”
“G0[XH][YH]”
“M05”
“M06 T[T]” <<== Is this not representing the tool number? [T]
Yes, it’s been a while I’ll check the exact command when I get home and post it. You need to add a M0 message and it will display in the dialogue. I think it’s “M0(Insert Tool [T])”. After the M06 line, I’ll confirm with you later.
@stleroux
Sorry I was off on the line for displaying tool number. Here’s how I have it and it will display tool number in dialogue pop up. Again if you’re using v2.0 it will show up at the right time. If you’re using the original macro that measures both tools at tool change it will show tool number on the first popup, instead of the second one. Not sure why I thought it was M0, sorry.
±--------------------------------------------------
- Commands output at toolchange
±--------------------------------------------------
begin TOOLCHANGE
“G0[ZH]”
“G0[XH][YH]”
“M05”
“T[T] (MSG, Insert Tool [T])”
“M06 T[T]”
Hope this helps!
Cheers,
Mike
Any luck sorting out the problem with bit setting? If you send me a screen shot of the program_start and tool_change dialogue boxes in the controller settings I’ll have a look and see if there’s anything that stands out.
Cheers
Hey Mike, been busy with work. I’ll be in the shop tomorrow and will get the pictures and anything else. I appreciate your help.
@BNB187 Hi Mike,
Thanks for the info. I will try this out later today.
One more question if I may. Can the touch plate be placed on the table surface or would that make it too far for the system to reach when probing? Or does it have to be located on the spoilboard?
Again, thanks for your patience.
I pocketed a spot for my probe in the spoilboard, but only about 1/8” deep. It’s really going to depend on where your spindle is mounted and bit stick out. Easiest thing would be to run the spindle down with your shortest bit over the probe where you want it to be placed. Farthest Z will travel is -133 on the absolute coordinates assuming machine is homed. The macro is written to use -133 as max travel when seeking the probe.
Excellent. I will test that.
One another note. Note sure if you would know.
Since we changed the PP, would I have to resave all the VCarve project (GCode) files I have already created to include this new line of code? Or is this something the system would do automatically. To my way of thinking, I will need to resave. If you are not sure, I will test and repost the answer.
I agree likely have to re-save files.
Hi Mike,
Awesome work on the macro. I love it. And thanks for your patience in answering all my questions.
Further enhancements requested, if I may 
Here is what I noticed when using the OF along with your macro.
- Secure material to waste board
- Probe XYZ using touch probe in bottom left corner of material
- Load file to carve
- Click on the Play button
- Router moves to designated area to do length probing
5.1. Popup prompt comes up with the following message(s):
- Remove Dust Boot
- Attach Probe Magnet
- Click Continue
5.2. Probe happens
5.3. Another pop prompt opens with the following message(s):
- Remove Probe Magnet
- Attach Dust Boot
- Click Continue
5.4. Router moves back to X0 Y0
5.5. IOT relay turns on router
This is where things get a little weird.
5.6. After the IOT relay turns on the router, the standard OF prompt comes up and tell me to Insert tool #xxx. This prompt only appears for a fraction of a second and then is replaced with another prompt with the following message(s):
- Insert tool #xxx
- Click Continue when spindle is up to speed
*** PROBLEM ***
Router is already running at this point
- Since this is the first tool, I click on Continue
- The first cut happens
- Once the cut is finished, the IOT relay turns the router off and the router goes back to X0 Y0
- The router then goes to the prescribed probe location
9.1. While router is being moved to probe location, a popup message appears on the screen with the message : Insert tool #yyy (This has the Green OK button on it, which leads me to believe this is a prompt coming from OF)
9.2. The previous message disappears as soon as the router reaches the probe location and a new prompt appears with the following message(s)
- Insert tool #yyy
- Remove Dust Boot
- Change Tool
- Attach Probe
- Click Continue
9.3. Probing completes properly
9.4. New popup comes up with following message(s)
- Remove Magnet
- Attach Dust Boot
- Click Continue - After clicking on Continue, the router goes back to X0 Y0
- IOT relay turns router back on
- This prompt comes up :
- Click Continue when spindle is up to speed
All future tool changes work fine repeating steps 9 through 12
I realize it is probably nitpicking but can the following be changed?
-
In step 5.1., can the order of the messages be changed?
- Remove Dust Boot
–>> Insert tool #??? <<-- This would be the first tool used in the job - Attach Probe Magnet
- Click Continue
- Remove Dust Boot
-
In step 5.6., can the message “Insert tool #xxx” be removed?
-
Is this possible to remove the message from step 9.1.?
-
In step 9.2., can the messages and the order of the messages be changed to:
- Remove Dust Boot
- Insert tool #yyy
–>> Change Tool <<-- Remove line - Attach Probe
- Click Continue
I also realize this would be a perfect scenario and I would try to make these changes myself but unfortunately, I do not have the time to learn a new programming language at this time.
Maybe this is something that should be looked at by the OF team??
Not sure if anyone else has experienced these little anomalies or if I am just being to picky.
I am trying to make this as child proof as possible as my wife will be doing most of the work on the machine
Sorry for the long winded post.
@stleroux most of the items you’re asking about can be resolved with some more changes to the PP. Work is a bit hectic right now. I’ll put together something for you on the weekend. Having said that there are some things that can’t be resolved using this macro as it works outside of the actual Gcode.
1 Like
@BNB187, that will be awesome. Looking forward to doing some more testing.
Let me know if I can assist in any way.
Thanks
IN POST PROCESSOR,
±--------------------------------------------------
- Commands output at the start of the file
±--------------------------------------------------
begin HEADER
“%”
“T[T] (MSG, Insert Tool [T])” <<<<<<<<<<<<<<<Remove or put a + in front of this line<<<<
“G0 G17 G21 G90 G40 G49”
“G0[ZH]”
“G0[XH][YH] M03[S]”
“M0(MSG, Click ‘Continue’ when the spindle is up to speed)”
To resolve this either remove or put a + in front of the line above. Then it will just prompt to click continue when spindle up to speed.
I can’t resolve this. This is happening because there is no click continue in the message (M0). So, it carries this message forward to the next M0 command which is issued outside of the Gcode file by the macro. I don’t know of a way to take the tool number in the Gcode and have it appear in the macro other than to do it in this manner. I played around with it a while back and tried to store the tool number as a variable and recall it but wasn’t able to make it work in this fashion. Effectively, the macro is a separate mini gcode file. I may look into a bit more in the future but I don’t have much time at this point, too busy making customer pieces. Alternately, you could have it pause before the macro starts but it’s really not going to make any difference as the next message will be the same but without the tool number.
So, this kind of goes back to the previous section. Because the insert tool # is coming from the gcode file it is simply carrying forward the message to the next M0 command. I don’t have a way to reorder this.
As for OF getting involved I’m not sure that will happen unless they decide to release a bit setting tool themselves. I don’t think that they place a lot of importance on this. Personally, I thought it wasn’t really a big deal before I tried it. Now, it’s something I wouldn’t want to live without. The results are 10 times out of 10 perfect for depth cut.
Also, it is possible to get rid of #12 as well if you so desire. I took it out pretty much immediately as this will also appear when cutting separate tool paths with the same tool. This can also be achieved by merging tool paths in VCarve Pro, but desktop doesn’t have merge.
IN POST PROCESSOR
±--------------------------------------------------
- Commands output for a new segment - toolpath
- with same toolnumber but maybe different feedrates
±--------------------------------------------------
begin NEW_SEGMENT
“G0[SAFEZ] M03[S]”
“M0(MSG, Click ‘Continue’ when the spindle is up to speed)” <<<<Remove or put a + in front<<
“G4 P20” <<<< Add this line
“G4 P20” is a 20 second pause. I put this in as a safeguard, I try to turn the router off at the switch for safety when doing tool changes. This pause has saved me numerous times if I forget to switch it back on. Will move to X0Y0Zsafe_height and pause for 20 seconds before continuing the file, giving me the opportunity to switch on router if I’ve forgotten after tool change. Whatever number comes after P will be a pause in seconds.
Hope this helps.
Sorry missed one bit. The Change tool can be removed from the macro in the controller settings tool_change dialogue box if you like.
@stleroux
One other thing I do is to put the tool numbers in the file name. For example:
Filename_1525_1125_1001.ngc
I find I often don’t even look at the popup so by doing this I can see the next tool number on the screen if I miss it or have forgotten. I keep a list of the tool database nearby for reference. In this example 1525 would be a 15 degree 1/4 shank vbit, 1125 would be a 1/8, endmill, and 1001 would be a 1mm endmill.
Cheers, Mike
@BNB187 Thanks for the updates.
I will have a closer look at this in the next few days.
@OnefinityCNC Hopefully this is something that is coming in the next few weeks as part of the upcoming updates???
@BNB187 Mike I have been using the macros for awhile now and they work great thank you for sharing. I see you have been making some changes to the post processor for vectric is there somewhere I can get the latest?
Hi Mike,
I love the concept, I have 3 questions… and excuse me since it’s only my second day playing with my woodworker cnc.
-
Has version 2.0 been tested with firmware I received on my 1F, firmware v1.0.8
-
Prior to any carving, I first home all X,Y, and Z with the probe to let the machine know where my stock material is on the waste board.
-
How do I set up the IOT relay?
So after mod’ing the controller with your macro, I will continue to do as I usually do, but have the advantage of changing my second and third bits etc, with the prompts and the bit setter, is that right?
I ask this because the initial x,y,z probe has already collected bit height.
Thanks again Mike, Kudos, really awesome concept!
Jenn
1 Like
- I have not tested 2.0 with 1.0.8, I’ve been using the original version as I have the laser and 2.0 is a problem with the laser. No problems with the original version. I don’t anticipate any issues with 2.0 as it is pretty much all the same commands as the original version just in different places.
2)Yes, probe x,y,z or manually set your zeroes. There were some issues with Z height when probing x,y,z in the past so I always probe x,y,z with a precision pin and then insert bit that I want to use and probe just Z.
- IOT relay is pretty straight forward Pin 15 for positive from relay and one of the ground pins for the negative on the breakout board. Here’s a link for a thread here Tool Enable - M15 - IOT Relay - & Breakout board (auto turn off/on router) - #3 by CruversWorkshop
The initial probe does NOT gather the data for the tool height differential calculation in this case. This is done when the tool touches off on the probe after you press play on the file you’re running. 1F post-processor has a line that cancels tool length offsets so this is the only way that I could see that would work.
Sorry for the delay I’ve been tied up with a landscaping project at home.
2 Likes