I want to learn all about macros. Where to start?
Currently I don't have much knowledge of computers in general. No experience with coding, scripting, etc. Learning to write macros is something I'm really interested in. With my current machine there's really only so much I could actually do with macros, but i may have other machines in the future. One thing I'm curious about, if I spent the time to learn about macros in mach3, is it similar for other control software if I switched to something else? I imagine this is a pretty huge subject and goes hand in hand with other things like fully understanding g code, editing posts, etc.
Considering that I really have no knowledge on the subject at all, is it realistic to expect this is something I could learn on my own with info from Google, youtube, etc? Where would I start? Any recommendations on how to go about learning something like this?
Re: I want to learn all about macros. Where to start?
Looking for a lot of the same info. Except I want to learn it for my Fadal and probing routines.
Re: I want to learn all about macros. Where to start?
IMO, the best way to start is to study existing macros, and learn what each part of them is doing.
Most macros are very basic, and don't really require a lot of programming knowledge. You can use Google to learn about VB.
I'm a self taught programmer, and when I want to learn how to do something, I always just Google it.
Mach3 uses a language called Cypress Enable, which they ;icensed from Cypress Software.
It's really just a form of basic, and is practically identical to Microsoft Visual Basic.
As far as the knowledge transferring to other programs, it depends on the language those programs use.
Mach4 uses Lua, which imo is more difficult to learn and understand.
UCCNC uses C#. It's actually quite similar to basic, and is not too difficult to learn.
Re: I want to learn all about macros. Where to start?
Also, there are two manuals you can download at machsupport.com
One that covers the language itself, and one with the Mach3 specific functions.
Re: I want to learn all about macros. Where to start?
Managed to make use of a couple macros, almost. Watched the intro to scripting tutorial video. From that I figured out how to send my machine to a specific location for tool changes which is pretty handy. Before my m6 did nothing at all but stop directly above the work where I can't reach the spindle with wrenches conveniently, now my tool changes are faster since I don't need to jog away first. The other thing I tried to implement is a probing routine for z. I used the common macro posted in here which seemed to work when running it directly in the vb script page. I didn't hook up a probe yet but it ran it's routine feeding down the specific distance at specific feed. I decided i want this to happen automatically after tool changes so I pasted the probing script into the m6 end. When running it in gcode, it almost works. When it comes to an m6, the spindle moves over to my specified tool change location, then stops and waits for cycle start, I then change my tool, hit start, at which point it continues with m6 end which is where I pasted the probing macro. It starts feeding down as it should (my probe plate will be directly below tool change location) but it continues to feed beyond the specified feed distance in the macro, even ignores z minimum soft limit. When running it in vb page it stopped when it was supposed to. It may or may not work properly once I actually have a probe plate there for it to stop against but I would still like to know why it's feeding beyond the specified distance. A probable issue is that I don't have the proper screenset. It's calling values that I don't know if they are actually there so I still need to get that figured out, but it still doesn't make sense to me that the script behaves differently when running in vb page vs running when triggered in gcode.
Re: I want to learn all about macros. Where to start?
Re: I want to learn all about macros. Where to start?
heres the one i used:
PlateThickness = GetUserDRO(1151) 'Z-plate thickness DRO
If GetOemLed (825)=0 Then 'Check to see if the probe is already grounded or faulty
DoOEMButton (1010) 'zero the Z axis so the probe move will start from here
Code "G4 P1" ' this delay gives me time to get from computer to hold probe in place
Code "G31Z-100 F500" 'probing move, can set the feed rate here as well as how far to move
While IsMoving() 'wait while it happens
Wend
ZProbePos = GetVar(2002) 'get the axact point the probe was hit
Code "G0 Z" &ZProbePos 'go back to that point, always a very small amount of overrun
While IsMoving ()
Wend
Call SetDro (2, PlateThickness) 'set the Z axis DRO to whatever is set as plate thickness
Code "G4 P0.25" 'Pause for Dro to update.
Code "G0 Z25.4" 'put the Z retract height you want here
Code "(Z axis is now zeroed)" 'puts this message in the status bar
Else
Code "(Z-Plate is grounded, check connection and try again)" 'this goes in the status bar if aplicable
Exit Sub
End If
the only things i have changed are the feed distance from -40 to -100 and the delay before probe from 5 to 1 seconds since i really dont need any delay at all but wasnt sure if it would cause problems by deleting the line completely. one issue i know i have is when its grabbing user dro 1151. not sure if its getting a value form somewhere or what that value is. do i need to modify my screen set to add this in? can i temporarily just give it a value directly in the script rather than having it get the value from somewhere else? like i mentioned, i dont even have a probe plate hooked up yet, but i did enable the probe so it works up until the point where tool should touch the probe. probably a bit premature to start diagnosing this before i actually set up the probe and make the needed changes for get userdro 1151 , but like i mentioned, when running the script as is in vb page, it feeds the -100, then stops (since i dont have a probe there yet) then retracts and sets z zero to where it reached the max feed of -100. when i paste the script in my m6 end macro (so it executes automatically after tool change) it behaves differently and does not stop feeding when reaching -100. If you have an explanation why, that would be great, but at this point im assuming i should just set up the probe and figure out the dro 1151 thing. how do i need to go about doing that? its really not important to me to have an easy access place to enter a plate thickness. if theres an easy way to put it directly in the script rather than modifying screen set so it can get the value from there, im fine with that.
another thing im curious about. i have a pretty rigid machine and run only carbide endmills. if it probes directly into a rigid mounted probe plate, is it really going to stop quick enough to not chip my carbide endmills? i would think a better approach might be a spring loaded touch plate that it feeds into, stops, then backs up at super slow feed and sets zero at the point it loses contact with the plate. i would assume that would be safer for the endmill and also more accurate, but im sure that would require some major changes to the scrip since its no longer a standard g31 probe. i suppose i can spring load the plate and still let it run the same way, just wont have the added accuracy of backing up at a much slower feed. reducing feed into the plate will help accuracy, but then the routine will take much longer. I did see one of your post mentioning a 2 stage probe, one fast, then a second time slow starting really close to the plate which i suppose would also work well. in the end i would really like to have at least .02mm accuracy.
Re: I want to learn all about macros. Where to start?
Just use this:
PlateThickness = 0.125 ' 1/8" plate thickness
Try it like this:
PlateThickness = 0.125 ' 1/8" plate thickness
If GetOemLed (825)=0 Then 'Check to see if the probe is already grounded or faulty
DoOEMButton (1010) 'zero the Z axis so the probe move will start from here
Sleep (150)
Code "G4 P1" ' this delay gives me time to get from computer to hold probe in place
While IsMoving()
Wend
Code "G31Z-100 F500" 'probing move, can set the feed rate here as well as how far to move
While IsMoving() 'wait while it happens
Wend
ZProbePos = GetVar(2002) 'get the axact point the probe was hit
Code "G0 Z" & ZProbePos 'go back to that point, always a very small amount of overrun
While IsMoving()
Wend
Call SetDro (2, PlateThickness) 'set the Z axis DRO to whatever is set as plate thickness
Sleep(150)
Code "G4 P0.25" 'Pause for Dro to update.
While IsMoving()
Wend
Code "G0 Z25.4" 'put the Z retract height you want here
While IsMoving()
Wend
Code "(Z axis is now zeroed)" 'puts this message in the status bar
Sleep(150)
Else
Code "(Z-Plate is grounded, check connection and try again)" 'this goes in the status bar if aplicable
Exit Sub
End If
Re: I want to learn all about macros. Where to start?
Quote:
another thing im curious about. i have a pretty rigid machine and run only carbide endmills. if it probes directly into a rigid mounted probe plate, is it really going to stop quick enough to not chip my carbide endmills?
It depends on how fast it's moving.
After Mach3 receives the probe input, the Z axis will decelerate to a stop. The faster it's moving, the longer it will take to stop after it hits the plate.
Technically, the speed shouldn't matter, as Mach3 records the point when contact is made. But testing has show that it does matter, which is why most of us use a two touch routine.
Re: I want to learn all about macros. Where to start?
excellent, thank you, i will try that. Out of curiosity, when it calls for plate thickness, why is there a 2, before plate thickness? Also, what is the sleep(150) you added?
Re: I want to learn all about macros. Where to start?
Call SetDro (2, PlateThickness)
This puts the PlateThickness value in DRO #2, which is the Z axis DRO.
That's actually an older way to do it.
I'd use this:
SetOEMDro(802, PlateThicknesss)
Which is the newer way to do it.
DRO, Button and LED numbers can be found in the Wiki: Mach3Wiki
Sleep() adds a pause, in milliseconds.
Sometimes they are helpful to allow Mach3 to "see" what the macro just did before it moves onto the next step.
The Mach3 interface only updates 10 times/second, and this gives the screen time to refresh before continuing.
Re: I want to learn all about macros. Where to start?
Call SetOEMDRO(802, PlateThickness)
Re: I want to learn all about macros. Where to start?
How does Mach3 call a macro from within a g-code program?
For instance, when you code G83, the macro M1083.m1s is what actually runs.
Re: I want to learn all about macros. Where to start?
That's a special case, where Mach3 does that internally.
If you want to call a macro like M999.m1s, you just call M999 from the g-code.
Re: I want to learn all about macros. Where to start?
That's too bad. I was thinking it would be quite simple to edit G83 into G85.
Re: I want to learn all about macros. Where to start?
It turns out that Mach does do a call for G85. There just isn't a macro there for it.
I copied M1083.m1s and renamed it M1085.m1s. I couldn't figure out how to get rid of the required Q-word so I just edited my post to stick a Q0.0 in there.
Works fine.
