I wired up the mini in out and with the redline HMI I can get the vac to come on if I touch the screen of the in/out button, but when I run a program, the vac does not come on. I am using Vcarve pro and the onefinity redline post processor. but the program does not seem to work in turning on the vacuum.
Did you edit the post processor to add an M code?
I will check on that too. right now I am still stymied trying to run a flattening program. It keeps telling me I am trying to exceed the x travel by 4.9 I do not know 4.9 what? inches feet mm? i am using vectrics v carve software and I downloaded the latest post processor. I have been at this now all f’ing day. and have yet to get the damned thing to cut one inch. and no there is no m8 that I can see on the HMI for this g code list when I click reset and show the gcode on the left hand side of the HMI screen. here is the g code.
%
(VECTRIC POST REVISION)
(358CAA3815B0605490C6B01BEFC20391)
(Onefinity Redline (inch))
G17 G20 G90
G0Z0.8000
G0X0.0000Y0.0000
T5
M6
M3 S20000
G0X48.2500Y0.8856
G0Z0.2000
G1Z-0.0312F50.0
G1Y0.6875F100.0
G1X0.7500
G1Y32.6875
G1X48.2500
G1Y0.8856
G1X48.0520
G1X0.9480
G1Y1.8756
G1X48.0520
G1Y2.8656
G1X0.9480
G1Y3.8556
G1X48.0520
G1Y4.8456
G1X0.9480
G1Y5.8355
G1X48.0520
G1Y6.8256
G1X0.9480
G1Y7.8155
G1X48.0520
G1Y8.8055
G1X0.9480
G1Y9.7956
G1X48.0520
G1Y10.7856
G1X0.9480
G1Y11.7755
G1X48.0520
G1Y12.7655
G1X0.9480
G1Y13.7556
G1X48.0520
G1Y14.7456
G1X0.9480
G1Y15.7355
G1X48.0520
G1Y16.7255
G1X0.9480
G1Y17.7155
G1X48.0520
G1Y18.7055
G1X0.9480
G1Y19.6956
G1X48.0520
G1Y20.6856
G1X0.9480
G1Y21.6756
G1X48.0520
G1Y22.6656
G1X0.9480
G1Y23.6556
G1X48.0520
G1Y24.6455
G1X0.9480
G1Y25.6355
G1X48.0520
G1Y26.6255
G1X0.9480
G1Y27.6156
G1X48.0520
G1Y28.6056
G1X0.9480
G1Y29.5956
G1X48.0520
G1Y30.5856
G1X0.9480
G1Y31.5756
G1X48.0520
G1Y32.4894
G1X0.9480
G1X0.7500
G1Z-0.0625F50.0
G1Y32.6875F100.0
G1X48.2500
G1Y0.6875
G1X0.7500
G1Y32.4894
G1X0.9480
G1X48.0520
G1Y31.5756
G1X0.9480
G1Y30.5856
G1X48.0520
G1Y29.5956
G1X0.9480
G1Y28.6056
G1X48.0520
G1Y27.6156
G1X0.9480
G1Y26.6255
G1X48.0520
G1Y25.6355
G1X0.9480
G1Y24.6455
G1X48.0520
G1Y23.6556
G1X0.9480
G1Y22.6656
G1X48.0520
G1Y21.6756
G1X0.9480
G1Y20.6856
G1X48.0520
G1Y19.6956
G1X0.9480
G1Y18.7055
G1X48.0520
G1Y17.7155
G1X0.9480
G1Y16.7255
G1X48.0520
G1Y15.7355
G1X0.9480
G1Y14.7456
G1X48.0520
G1Y13.7556
G1X0.9480
G1Y12.7655
G1X48.0520
G1Y11.7755
G1X0.9480
G1Y10.7856
G1X48.0520
G1Y9.7956
G1X0.9480
G1Y8.8055
G1X48.0520
G1Y7.8155
G1X0.9480
G1Y6.8256
G1X48.0520
G1Y5.8355
G1X0.9480
G1Y4.8456
G1X48.0520
G1Y3.8556
G1X0.9480
G1Y2.8656
G1X48.0520
G1Y1.8756
G1X0.9480
G1Y0.8856
G1X48.0520
G0Z0.2000
M5
G0Z0.8000
G0X0.0000Y0.0000
M2
%
also it keeps telling me that i have exceeded the y travel as well. I have gone back into the program ( vectrics) and made the pocket smaller and now it says I am exceeding the travel even more. i am next to giving up on flattening this thing. I have followed christies video explicitly and I have naught to show for it.
Why would I have to edit a post processor? I am running all the onefinity supplied hardware? no aftermarket stuff anywhere. you telling me vcarve pro is not providing the correct post processor?
At this point it may be helpful for you to share the current Vectric file you loaded, so that others can see exactly how you set it up.
i listed the gcode but here is the file
flatening toolpath.crv (34.5 KB)
“C:\Users\rober\OneDrive\Desktop\flatening toolpath.crv” i hope it helps and while they are at it I have homed and probed and started the file but it moves from x0 and y0 to y 1.83 and I do not know why it is doing that either. i have had to about it now twice and no the vac still won’t come on. today has been a very bad day. i put the zero zero at the left front corner yet when i start the program it goes to the far right hand side and about 1.83 inches towards the back of the machine to start cutting and i do not have any clue as to why. this would leave a huge ridge at the front of my spoil board. that i do not want.
Tnx. Providing the gcode is always a good start, but the actual file will allow settings, parameters, etc… to be evaluated as well.
I can understand your frustration, but try to remain positive. I remember when I was starting out I often got stuck on what others considered the simplest things, or I didn’t know the correct terminology, or the correct questions to ask, or found out I was actually correct in my thinking but the manual was incorrect (this across many forums)…and these things still happen albeit less frequently.
It is a complex hobby, but when the stars do align, wonderful things happen…
like low profile clamps from Hilljackfab (Shameless plug!)
funny I had a lot less trouble with the Masso than I am having with this explicative deleted, redline .
The Gcode command to turn on your vacuum isn’t included in the Post Processor by default because not everyone has a setup that requires it to be turned on. But editing your Post Processor is not that big of a deal. Check out this video that may help you. The machine in this video is a Masso based Onefinity, but it’s the same principle for the Redline Post Processor. https://www.youtube.com/watch?v=9Bkc3fgcd90
For what it’s worth, it’s likely MM, at least that was what I found when I was messing about w/flattening my top last week.
Looking at your gcode it looks like the maximum X is 48.25" and your maximum Y is 32.6875"
First item I’d check is to manually jog your machine to the back right corner and make sure that the Machine Position values are less than or equal to those. If the number in your g-code is larger, it’s telling the machine move farther than it can and you’ll get errors.
I’m going to try to explain the next bit as best I can though I’m still struggling to wrap my head around it, but it has to do with Work Position Zero versus Machine Position Zero. In my case my machines maximum X is 48.307 and Y is 32.126. When set my work position to zero on the front/left corner of the waste board I get X .495" and Y -2.133 (this is due to my having a QCW table where the slats are pushed back in order to make room for the ATC). So, what was happening to me was the maximum Y was reduced by 2.133" (29.993) and though my maximum X was STILL 48.307, once I set the zero to the waste board if I called for X 0 in gcode absolute (G90), it would error because it was trying to move the the head of the machine less than .495", which was actually the physical machines X 0.
It was a hot mess to figure out and I didn’t do a great job on it. But at the end of the day I had to make sure that the program never called for less than X .495" nor greater than Y 29.993" or I would get over travel errors.
What I’m trying to demonstrate is that unless your spindle dead center is exactly at the front/left corner of your waste board for X0Y0 and dead center at the back/right corner for X-Max Y-Max, once you introduce the workspace coordinate system then the numbers put out by your software may cause travel errors or not perform as you initially have in your head.
In most operational cases we’re working below the maximum reaches and well within the waste board so these issues don’t crop up, but once you get close to the edge it can get complicated fast.
Attached are modified post processors I use with my Redline to control the vacuum.
You might want to open each of these to see what’s been modified as a learning experience. Load into notepad and search for “ADD NEXT”. There are several entries made throughout the file to turn on and off the vacuum.
I use “M8”(Output 2) in my environment…you may need to change it to “M7” (Output 1) depending on which output your VAC is connected to.
It would be easier to make these mods before you import the files into VCarve
If you want to go the easy route, you can download the two files and import them into VCarve. Go to VCarve menu option Machine->Install Post-Processor and select one of the files you downloaded. Repeat the process for the second file.
OneFinity Redline (in) new.pp (4.7 KB)
Onefinity Redline (mm) new.pp (6.5 KB)