I have tried a couple of carves with took changes. I am using Carbide Create Free now. I have been setting my retract height to 1/4-1/2" so it can speed things up. However, when the machine pauses for the tool change, it only retracts to that short height, making it impossible to change the tool. Is there a trick where I can add code to make the Z go up several inches to accomplish the tool change?
V-Carve has a setting you can use to set the height when it stops for a change - but I donāt know how to make Carbide Create do that. Most people create different files for each bit - so you can move the machine around and re-probe for Z when you change files/bits.
When the spindle/router retracts for the tool change, just raise your z-axis enough to be able to change your bit then re-zero your Z-axis and you should be right to go.
2 Likes
You can raise the Z-axis from the control panel or with the joypad.
You will need to probe the Z axis after the tool change anyway since the new tool height is very likely to be different from the previous one.
I am new to cnc, I am using Carbide Create, mainly because I am a Mac user and refuse to buy a PC just for my cnc. Anyways, I have create a design that will require multiple tool paths with bit changes, my question is, when I create the gcode, how will the machine know what tool path to do first or in what order? is it simply the order in which you create the tool paths? thx.
you must separate each tool into their own file.
2 Likes
THX! I will do that.
joy stick does not work in the middle of a tool change
Hey Fred,
this is a known missing feature. While youāre in program mode, jogging is not available. This also applies when the machine encounters a M6 (tool change) event in your g-code program.
The ability to jog during pause or tool change is a feature that is requested under
- Tool change jogging plus notifcation/ETA of toolchange
- Hereās a key element missing from the BB controller
- here
- here
However you can modifiy the behaviour at tool change. Should you just want to raise your Z higher during a tool change event, or alter the behaviour at tool change in another way (e.g. bitsetter-like tool change at home position), you can insert g-code in the ātool-changeā field of the General Configuration Tab. The code in this field is executed when a M6 (tool change) command is encountered. Regarding what to insert there, I cited some information here the other day.
Welcome to the forum!
1 Like
New to forums, first post, this looks like an old thread but only one I see on topic. My first carve I screwed up twice and I think this answers question. I have 4 tool changes in my gcode. Did it in VCARVE and didnāt know to do separate files for separate tool paths. My first pocket worked great. Then the spindle moved in front of the piece and told me to change the tool and probe z, but height was too low to fit probe block between wood and spindle. So the collet was in front of my piece and too low both times. First time I didnāt even get probe to touch. It did the emergency stop and I screwed around with the second tool until I got it in. The. It restarted the code at the top and I had to probe XYZ, went to wrong spot and it destroyed that piece. So I repeated my first tool path on a new piece of wood and the first tool path worked fine. I did get the block under the tool on the tool change but it didnāt raise back up after I started router and hit continue. Broke my bit in half.
First carve frustration.
I have yet to figure out how to set my resting Z higher for tool changes without creating separate files.
One way I found to cheat it for most bit changes is unscrewing the collet nut and wiggling out the collet too. This gives room for most bits I use. If you do t get enough height to set your Z I create a separate file. I am learning every day. Like it a lot.
I canāt think of an argument for not creating separate files for each tool path.
1 Like
Hey Dan,
why donāt you simply use forum search engine functionality and read one of the many answers to this most frequently asked question, e.g. here:
or many practically identical answers? One of the many answers to this question is even only two posts above yours.
Anyway, thereās no reason to fear inserting a simple but comfortable g-code example into the ātool-changeā field of the General Configuration Tab, as described here. G-code is not rocket science 
, and with a tested example you can break nothing. You can mill air to test the example and see if itās comfortable enough for you.
I would try the second example, it is made for the Onefinity Touch probe height.
It is made for the case where you touchprobe on your workpiece top (=part zero is on workpiece top). Should you touchprobe on the machine bed instead (=part zero is at wasteboard height =at workpiece bottom), simply remove the āG0 X0 Y0ā line. Probing will then be done at machine home position.
1 Like
Thanks. Most appear to be adding lines in gcode. Sounds good but I am not that good with doing stuff like that. But I am learning. Thanks. Dan
1 Like
Hey Dan,
Itās not that complicated: On most computers, it is Ctrl-A (select all), Ctrl-X (cut), Ctrl-C (copy), and finally Ctrl-V (paste).
EDIT: Sorry, I forgot that maybe not everybody has a keyboard and a mouse connected to the Onefinity Controller, or runs the Onefinity Controller User Interface from a remote computer (which would have the additional advantage that you can see the CAMotics 3D toolpath simulation and can also easily make screenshots of the Onefinity Controller User Interface), but instead most users are probably used to work with this ugly stupid on-screen keyboard on the touch display (which on top of being an on-screen keyboard, is missing important system keys 
). Of course, such a distasteful thing can discourage users from doing anything at all. But, you donāt forcibly need to add a keyboard and a mouse, the on-screen keyboard will also do it.
Of course, instead of clicking into the ātool changeā field of SETTINGS page, then typing Ctrl-A (select all), Ctrl-X (wipe it out), going to the new browser tab that you previously opened on Onefinity Controllerās chromium window or on your remote computer, where you opened the page with the example, marking the example, typing Ctrl-C (copy to clipboard), and then back on the Onefinity SETTINGS page in the first browser tab, pasting it with Ctrl-V (paste clipboard content), of course, instead of doing this, you could very well, as you suggested, simply look which lines perhaps are already there (as shown below), and then just add the additional ones from the example. This should even go with the on-screen keyboard 
You actually thought more practically here than I did in my joke above
Making the ātool changeā routine usable
For example, if the content of your ātool changeā field on your SETTINGS page already contains the following (it usually should, as of up to version 1.0.9):
(Runs on M6, tool change)
M70
G21
S0
M0 M6 (MSG, Change tool and attach probe)
F100
(probe to minimum z soft limit, which is -10)
G38.2 Z-10.0
G92 Z15.4
g0 Z30
M0 (MSG, Remove probe, start spindle)
M72
then what Razi Ullahās excellent example would change is just the following (add the text in bold letters and press āSaveā on the flyout menu):
(Runs on M6, tool change)
M70
G21
S0
G28
M0 M6 (MSG, Change tool and tighten collet)
G0 X0 Y0
M0 (MSG, attach probe)
F100
G91 ; (added by Aiph5u, this was missing!)
G38.2 Z-10.0
G92 Z15.4
g0 Z30
M0 (MSG, Remove probe, start spindle)
M72
What will this little change do? Much!
Instead of being stuck over your workpiece at tool change, with too little room to be able to change the bit, the added G28 command will move the router to the machine origin, which is at home position, and ask you to change the bit THERE. Isnāt that comfortable? Plenty of room to change the bit, and no need to lean over the machine. Then, after you have confirmed that you are done with changing the bit, the G0 X0 Y0 command will move the router from the machine origin to the part origin (also called workpiece zero), which means the position where you probed your workpiece at the beginning, and allow you to probe Z again. Probing Z is necessary after every tool change, since usually the bits have different lengths, so this is to make the machine know the new tool length. And after youāre done with this, the machine will restore all settings and positions with the M72 command that it previously saved with the M70 command at the start (including your possibly chosen imperial measurements mode ), and voilĆ , the machine resumes the program and goes on with the next part with the new bit. A beautiful tool change within the program, isnāt it?
Note that this example assumes you have your workpiece zero on top of the workpiece and that you probe the top of the workpiece. Even as often there may be the case that instead you defined a 3D model with the workpiece zero on the bottom of the workpiece, which means, as you surely know, this has to be Z-probed directly on the machine bed. The Onefinity Touch Probe is used upside down in those cases. In this case you can still use nearly the same ātool changeā example, you would simply remove the line āG0 X0 Y0ā (or better just make it temporarily inactive by prepending a semicolon ( ; ) at the beginning of the line), and the Z probing will then simply be offered at home position too, where you already changed the bit.
One thing that you could change too, is to increase the ā-10ā value on the G38.2 (Probe) command to a higher negative value.
This value does nothing more than to tell the machine for how much Z travel it should move downwards in order to find the touch probe before aborting. By increasing this value you can get plenty of reserve to avoid the annoying āProbe not foundā error, but dependent on at which height the workpiece zero of your g-code program is, you will have to select the value that accomodates your needs.
Finally, what you can still adjust later, after youāve tested this example, is from where you want the Z to start probing, perhaps from a lower position. If you know e.g. that your workpieces are usually rather low in height and how long your longest bit in the program will be, you can add an additional command for moving Z to a lower position prior to start probing. You can get help for this later here in the forum.
References
- How to understand and to use the content of the ātool-changeā field of the SETTINGS page, is to be found here ā.
EDIT: There is an updated example of the ātool-changeā routine in the newer posting below
3 Likes
Hey Jim,
sorry that noone answered to your post (I was absent at that time).
For the answer, see above.
Welcome to the forum!
1 Like
ā¦ah and I forgot:
Welcome to the forum!
How do you confirm that you changed the bit? Will it ask that question? I put the changes in, now I will make a program and test that out to make sure I entered it correctly. It sounds like it will be very nice to change bits.
Thank you very much for your reply.
Hey Steve,
a popup window with two buttons, āContinueā and āStopā
sure.
