It would be great if the (MSG,) command could be supported. I imagine something like:
(MSG, Don’t forget to move the vacuum hose)
M0
…
i.e. the M0 causes a Pause, I look on the screen and see the reminder to move hose, before I press continue. Maybe include a de-facto M0 [Pause] until the message has been disposed.
I understand your request, personally I don’t need another forced “defacto M0” pause in the software to remind me to perform a common sense action when operating my CNC. Perhaps the request would be to add this as an “optional pause” checkbox while going through the machine setup screen. But even then the request will take resources away from development of other upgrades the development team is working on to provide us as customers with a better product.
Most folks start with a checklist of some sort, written or printed out to follow until muscle memory kicks in for standard operation of equipment.
Hopefully folks wont take my reply the wrong way.
1 Like
I will note that if one wants more prompts, setting the machine to think it has a BitRunner results in a speed setting dialog which I use as a chance to replace the dust shoe at need.
1 Like
I think what the original request was referring to would be optional. No one is going to force you to stop and do something.
It would be helpful to be able to add a “note” toolpath, so-to-speak, in some instances. I might do most of an operation with clamps in place in addition to double-sided tape but just before the cutout, having a pause where the machine stops and a little note pops up that I can set about what i want to do would be handy.
1 Like
That would be fine if thats possible in the software. It was not clear when I read the post that was the case. I only replied to the post due to the numerous request discussions over CM prompts for certain operations and the request to remove them to reduce the time for certain operations.
Adding a “note” tool path option is different in my mind than what the OP asked for and I can see the benefit of this option in many cases during the workflow.
My thinking about the optional pause on note is to answer the question “When is the message going to disappear?” Presumably with OK button. If it doesn’t pause, and another message pops up before the previous message has been disposed of, will it go over the previous? Hence the thought of, why not pause the machine until the message is disposed of? But I agree that I’d rather put a M0 into the gcode to pause instead of a mandatory pause because of the note.
I’ve had the Shapeoko for about 7 years now, and there have been numerous times when I thought it would be nice if some specific message could pop up. Whether it is a reminder to do something which is not part of my general workflow, or for one job which I do about once a year to ensure the clamps are held in a specific way…
I will note that Carbide Create does have a specific Notes feature which has a checkbox for show on open — make opening the Carbide Create file as a check a part of your workflow?
1 Like
My post was not intended to offend you (or anyone). I don’t have any issues with your request, it seems I may have incorrectly interpreted the request due the defacto M0 statement. If user selectable, perfect.
I use this feature all the time for reminders and instructions for shared files.
Please note I’m suggesting this feature for CM, not CC.
1 Like
I’ll put this out there. CM is already able to display text notes. Any line in a .gcode or .nc file enclosed in parentheses is treated as a comment not sent to the controller.
I leave myself on screen reminders this way all the time by prefacing them with M1.
Here is an example of something I do at the very end of a program. I have a 3D toolpath that for whatever reason always cuts a little deeper than I want. One way around that is to split the project into separate programs and do that one last on its own.
The way this gets parsed the machine pauses after the G53G0Z-0.200 move and displays the RAISE Z message. I press start and it finishes the M2 cycle.
I also put some comments at the top of the .gcode file which can be read in CM Preview.
I do this manually in a text editor. Can also be done via post processor in other CAM packages…
I know manual gcode editing isn’t for everyone…I hope this all makes sense.
M1
(!!! RAISE Z+.015 NEXT PROGRAM !!!)
G53G0Z-0.200
G53G0X-2.000Y-2.000
M02
4 Likes
@4wm or anyone for that matter…
I am curious if this can be done at the start of a program but instead stating…
“Turn on Chiller!”
AND possibly at the end of the program…
“Turn off Chiller!”
Thank you
It should be possible. I would have to test to be sure its at the right point.
So you need Create Pro to save gcode as a separate file. with .nc file type. (I use Vcarve Pro, but the same principle works)
Here’s what the beginning of random Create test gcode file looks like up to the first plunge into material. It already has many comments built in.
stock code click to expand
(Design File: D:.create-test.c2d)
(stockMin:0.000in, 0.000in, -0.750in)
(stockMax:12.000in, 12.000in, 0.000in)
(STOCK/BLOCK,12.000, 12.000, 0.750,0.000, 0.000, 0.750)
G90
G20
(Move to safe Z to avoid workholding)
G53G0Z-0.197
(TOOL 201: .201 End Mill .1.4..)
(Toolpath: Pocket Toolpath 1)
(Pocket Toolpath 1 - Pocket)
M05
(TOOL/MILL,0.250, 0.000, 0.750, 0.00)
M6T201
M03S18000
(PREPOSITION FOR RAPID PLUNGE)
G0X4.1226Y4.0248
Z0.2000
Z0.0394
G1X4.1283Y3.9312Z0.0455F20.0
I would try adding it here first. This should make the machine sit idle with spindle off displaying “Turn On Chiller!” When you press Start then it will retract and run as normal.
edited code click to expand
(Design File: D:.create-test.c2d)
(stockMin:0.000in, 0.000in, -0.750in)
(stockMax:12.000in, 12.000in, 0.000in)
(STOCK/BLOCK,12.000, 12.000, 0.750,0.000, 0.000, 0.750)
G90
G20
(Move to safe Z to avoid workholding)
M1
(Turn On Chiller!)
G53G0Z-0.197
(TOOL 201: .201 End Mill .1.4..)
(Toolpath: Pocket Toolpath 1)
(Pocket Toolpath 1 - Pocket)
M05
(TOOL/MILL,0.250, 0.000, 0.750, 0.00)
M6T201
M03S18000
(PREPOSITION FOR RAPID PLUNGE)
G0X4.1226Y4.0248
Z0.2000
Z0.0394
G1X4.1283Y3.9312Z0.0455F20.
EDIT: I think its a little trickier at the end. Normally last 3 lines are this.
G0Z0.2000
M05
M02
On my programs with ending messages I inserted coordinates. I’m set for inches. So what this does is move the machine moves to 1" short of the far right corner then it Pauses and displays the message. When Start is pressed then it moves to the M02 end program spot 5mm (-.0197") from the back right
G0Z0.2000
M05
M1
(Turn Off Chiller)
G53 G0 X-1 Y-1
M02