Finally got my ATC set up and running on my CNC

[bobby milam]

I've spent a good time trying to figure out macros and settings and after much help from a forum, I have my CNC running an ATC spindle controlled by Centroid Acorn. Can't wait to get back to using it for work again. It's been a huge learning experience and believe me I had zero experience when I started this. It was frustrating work at times but rewarding.

Can you imagine how long it would take to do this file with manual tool changes? Here's a video of it in operation.


https://www.youtube.com/watch?v=R0c5StkFUWc&t=84s

[Bruce Page]

Very slick setup Bobby. It makes my Camaster "fast tool change" look Neander!

[David Buchhauser]

Nice work Bobby!! That's one awesome machine. I hope to get mine running one of these days as well.
David

[Jim Becker]

I would positively love that, Bobby! Nice job on the implementation.

[Keith Outten]

That's pretty slick, congratulations on getting it to work. That would be a major challenge for me.

[bobby milam]

Thanks for the comments. David and I have spent many nights discussing the macros and how to implement this. The people at Centroid were a major help. I'm not sure what time a tool change took doing it manually. I know that I'd be waiting at the machine for a bit to stop so I could change it and that kept me from doing other things. I never timed it but I would guess a tool change took me around 4 minutes from strat to cutting. Now it will be under 20 seconds total. I know that I have gotten lazy on some files where I could have done a better job by using more tools but ran it with fewer just to make it easier. This should allow me to use better tool management as well as being faster. The average things that I make run 1- 1.5 hours. I probably spent 20-30 minutes of that waiting for the tool change. That is 20-30 minutes of time that I can be finishing something else.

I gave up about 4" of the Y travel to instal the tool rack this way so I can no longer cut full sheets of plywood but since I rarely do that anyway, I will gladly give up the bit of travel for the convenience. I already have plans for the future to make a sliding tool rack and reclaim that 4" as I become more knowledgeable with the software.

Keith, believe me this was a major challenge for me. I know virtually zero about writing macros. If I can do it anyone can if you have some good guidance.

[Brian Lamb]

Nicely done, most rack tool changers move terribly slow, which I don't understand. I have Centroid on my CNC mill and it has no tool changer and it couldn't be implemented because of the tool can only be changed when the spindle is all the way up. Looking at acquiring a 4x8 router myself and adapt this style of changer.

A couple of comments, and I don't know what you have been through, but it seems you should drop a little lower in Z over the rack, looks like the tools drop a bit, and they get sucked up when changing, maybe Z-.05" or so would help. In your code, I don't think you need G49Z0 and the M25, the M25 will cancel the Z offset and raise the spindle to the top, at least that is what I do. Might want to take out the return to G54 X0 Y0 too as that's going to eat up some time over a lot of tool changes.

[bobby milam]

Thanks Brian. I think you are right about the Z height. I haven't figured out what to use to make it move to the rack without the G54Z0. I will look at the macro and see what I can do to improve it. This is just the first time I had it actually operating and making tool changes. I definitely appreciate the feedback.

[Brian Lamb]

Well, I just went and caught up a bit on the Centroid forum, and you first posted on the 11th and here you have it running on the 18th, that's amazing! Good job! In your macro you should be able to go from where ever on the table to the tool in the spindles rack position directly, then to the called for next tools rack position, and then it seems you are already coming back into the program and going to the next called position to machine. I think it would be just eliminate the G54X0Y0 that must be in there somewhere.

I could be wrong on the G49Z0 to cancel any tool offset, but I think all you need is the M25, that's what I use and modified my post to output in my G-code. The M25 sends the spindle up to home position (quill in my case), then you rapid to the pot, and call up the macro which should have your distance from home to the Z depth required to drop/grab the tool.

Obviously you have smarter guys than me on the Centroid forum, so they probably have better input.

[bobby milam]

Its been much longer than a week. I've been working on this for a couple of months trying to figure out the macros.

I don't have a G49 in my macro. I'll bre looking at it trying to make it better.

[Mark Bolton]

very nice. I have played around with a lot of Macros and I dont envy what you had to do to get that setup though Im sure you learned a ton in the process which is very advantageous.

I recently kicked around the idea of adding a second rack to our machine (10 pos now at the back in X) and thought of a small 6 pos rack in Y along the X0 and have since scrapped it due to the complexity.

Fast tool changes are imperative with fixed rack machines. When I first fired ours up it was scary but now it seems like a snail.

[Mark Bolton]

Thanks Brian. I think you are right about the Z height. I haven't figured out what to use to make it move to the rack without the G54Z0. I will look at the macro and see what I can do to improve it. This is just the first time I had it actually operating and making tool changes. I definitely appreciate the feedback.


I am most definitely wrong but I think the reason for this sort of approach to the rack is because the tool offset doesnt take into consideration the tool diameter. Which means if you came into the rack diagonally with a tool in the spindle there is a serious crash potential.

[Brian Lamb]

I re-watched his video and I was trying to read the code posted on the screen, he is cancelling any cutter diameter compensation with a line that says G49 H0 M25, which cancels tool length offset (G49), any cutter diameter compensation (H0) and then sends it to Z home (M25). I did see (I think) a G90 X0 Y0 in the code, that might be what is sending it to home before each tool change. I don't know what software Bobby is using for g-code, but it might be a setting in his post processor there that is causing the move to 0,0 and not anything to do with the macro.

I noticed that after his tool change he is dropping in Z before he starts off across the table, I would stay at Z home and wait until I got into position before going Z minus... safer in case you have any clamps in the way. Again, that might be a post processor thing.

I learned G-code back in the late 70's and we did everything with a pencil and paper. I don't do that any longer of course, but I have a real thing for all sorts of extra moves and monkey motion, which almost all software seems to spit out today.

[bobby milam]

Good point Mark. Originally the file after clamping a tool, the z would lower to move back into the cutting gcode which with a long tool could cut into the rack or I worried about crashing into another tool leaving at an extreme angle. I added to it so that after the clamping, it raised the Z then it stepped out 1.5" to clear the rack before going back to doing what the gcode called for. I am working right now to make a dust shoe docking station. The shoe will be a magnetic 2 piece and will slide into the dock, the Z will raise which will seperate the dust shoe, do the tool changes then go back and grab the shoe and slide it back out of the station. I saw someone else on the Centroid forum that made one and thought that was a good idea now so as to not have to deal with pneumatic system. Once I figure the dock out and mount it I am going to have to edit the macro again to put those movements in. So, this is going to be an ongoing process and I have much more to learn.

In the mean time, I need to find more money to order more tool holders.

Mark, the beauty of Centroid is that they have sample macros for different types of tool racks already made up. I didn't have to start off from scratch. I just had to learn what everything meant then edit things with my coordinates and put in or take out commands. I could never have done this from scratch on my own.

[Mark Bolton]

I agree on all points. All the wasted steps get pretty irritating. I have several in my post I have never had the time to wring out. But on the flip side Im always cautious as I know they are there for the rare event/instance I dont foresee.

Thankfully Im rarely in an instance where a few wasted moves are critical to profitability but its definitely nice to get rid of them when you can.

[bobby milam]

Brian, I am using vcarve pro for the gcode. The dropping of the Z is a postprocessor thing. I had questioned about this and was told I had to change in vcarve. I don't use clamps so I never bothered with it. Here is my macro if you are interested in seeing it. Some of the things are handled in other parts in the software and those I am still learning about.

; File: mfunc6.mac
; Desc: Tool change macro for no finger rack mount ATC
;
; Inputs:
; ToolIsUnclamped IS INP2
;
;
; Outputs:
;
; ToolUnclamp IS OUT8
;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;;
O9101
;Enter the XY coordinate of Tool #1
G53 X6.3231Y96.9599
M99
O9102
;Enter the XY coordinate of Tool #2
G53 X11.1710Y96.9599
M99
O9103
;Enter the XY coordinate of Tool #3
G53 X16.019Y96.9599
M99
O9104
;Enter the XY coordinate of Tool #4
G53 X20.8670Y96.9599
M99
O9105
;Enter the XY coordinate of Tool #5
G53 X25.7148Y96.9599
M99
O9106
;Enter the XY coordinate of Tool #6
G53 X30.563Y96.9599
M99
O9107
;Enter the XY coordinate of Tool #7
G53 X35.4107Y96.9599
M99
O9108
;Enter the XY coordinate of Tool #8
G53 X40.2787Y96.9599
M99
O9109
;Enter the XY coordinate of Tool #9
G53 X45.1265Y96.9599
M99
O9110
;Enter the XY coordinate of Tool #10
G53 X49.9675Y96.9599
M99
; Variable Definitions:
;#150 = Tool currently in the spindle
#100 = -8.0 ; Z height of tool rack
;skip if graphing or searching or if at the same tool
IF [[#4120] == [#150]] || #4202 || #4201 THEN GOTO 500
IF (#150 == 0) THEN #150 = 1 ; Initialize tool
G53 Z0 ; Move to tool change height
M3 S0 ; Turn the spindle on
M98 P[#150 + 9100] ; Go to tool location for the tool that's in the spindle
G53 G1 Z[#100] F10 ; Move Z down to the tool rack
M15 ; Unclamp the tool
G53 Z0 ; Move Z up to tool change height
M98 P[#4120 + 9100] ; Go to the desired tool location
G53 G1 Z[#100] F10 ; Move Z down to the tool rack
M16 ; Clamp the tool
G53 Z0 ; Move Z up to tool change height
G53 Y93.5 ; Move Y to clear tool rack
IF #50001 ; Prevent lookahead from parsing past here
#150 = #4120
N500

N1000 ;End of Macro

[Brian Lamb]

Hi Bobby,

That Macro looks clean, I understand most of it, not sure what the 4120, 4202 and 4201 are, but I'm assuming that line means if the tool called is the tool that's already in the spindle, you skip down to line 500. The rest makes sense to me, you can dial in the #100 variable to be the height down to the rack... I'd put a tool in the spindle and move down over the pocket until a .005" feeler fits between the tool holder and top of pocket and see what that number turns out to be.

Nothing in the Macro is causing the move to machine home before taking off for the tool change, so that must be in V-carve, along with the drop in Z before you get to your first XY position. I suspect you might have something like "Return to safe Z after tool change" as an option in your software. I use Sheetcam and that's what it is called in there. I changed my post to not move from Z home (all the way up), until it reaches the first XY position. It might not be an issue with vacuum clamping, but a lot of times I have vises, length stops and all sorts of issues on my table that I don't want to slam a tool into as it's going from my tool change position back to cut the part.

Now if I can just find a suitable router, I can play with this macro too! :D

[bobby milam]

I did go back and change the rack height so they aren't dropping any more. The dropping of the Z to get to the first XY position is set in vcarve. I never changed it and the default is 0.2 ". I use screws to hold down so it has never been an issue. I can make it higher but the higher you go the longer it will take to run the file so you have to have a happy medium. I could use the CNC12 software to create a safe zone that the spindle wouldn't enter those areas for clamps and such if I had the need to. I am not sure but I think the G53 is what is sending it to the front of the work piece but am not sure what to replace it with. Right now I can live with it because it keeps it from coming at an extreme angle and crashing and gives the spindle time to stop. I will probably alter that as I learn more.

I need to put the bits back in and check my tool library and then remeasure all of the tools and verify that they will all be at the proper Z zero.

[Dennis Peacock]

Love this!!!! I'm just working to have a stable and working CNC. Once day....I'll have a nice stable CNC solution and ATC is something I hope to have. Thanks for posting.

[bobby milam]

Thanks Dennis. I actually removed the tool rack yesterday. I am changing it up a little to make using a dustboot easier and more efficient. If it works I'll update with a new video.

[bobby milam]

Thought I would update this thread with what I have changed. The initial rack had the holders spaced apart much further than it had to be and I could add more tools to the rack. I didn't really like the idea of building a docking station and editing the macro to include that plus it would slow the tool changes down. I thought about a pneumatic boot so it would lift out of the way but really wasn't sure what parts and lengths would be needed and that was more money. David Buchhauser (https://sawmillcreek.org/member.php?178337-David-Buchhauser)
and I have been talking and tossing ideas back and forth for this and his machine. He gave me the idea of making donuts to build a rack that would allow the shoe to remain in place. That is the route that I ended up going. Thankfully MDF is cheap so making different racks is relatively inexpensive.

I built the rack with the same spacing between holders and used the metal dust shoe that came with my machine. I had to make some minor changes to the dustshoe so that the bristles wouldn't get stuck in an inward facing direction and cause an issue with putting a tool in the rack. Now I am able to leave the boot in place and it just lowers around the tool holder position allowing tool changes without removing it.

Here's a new video that shows it performing tool changes.

https://www.youtube.com/watch?v=M9cPYcuct7s

[Mark Bolton]

coming along. very nice work.

[Daniel Araya]

Very nice work, smooth!

I came to the forum to see if I could find any info about a CNC machine I just bought (cheap!) and the first thread I found was this, my machine looks very similar to yours!
I got zero manuals for it but I have cleaned it out and started to get to know it, it runs fine but the control system is NCStudio and the tool change is manual so I have to upgrade a bit!
Do you happen to have any info about the spindle (mine is a 6KW) and spindle connections, specifically about the air seal and control valve for the ATC?

Here is my machine:

428427

[bobby milam]

Not uncommon on the Chinese machines to not get much in the way of manuals. My spindle is smaller than yours and I did not receive any manuals with it. The seller still contacts me regularly to see how everything is going and I am able to ask him and get a quick answer back on most questions that I have. What are you trying to figure out? I have never used the NCStudio control system so can't help you out at all on anything there. Manual tool changes aren't too bad with an ATC spindle but might as well set it up to do them automatically since you have all the expensive stuff you need already. I love having the big machine vs the my first one which was a desktop.

[David Buchhauser]

Here are several manuals for NCStudio.
https://www.cnczone.com/forums/attachments/1/9/6/7/1/4/175197.attach

(https://www.cnczone.com/forums/attachments/1/9/6/7/1/4/175197.attach)https://m.darxton.ru/files/pdf/controller/PCIMC-63A-53BC-user-manual.pdf

(https://m.darxton.ru/files/pdf/controller/PCIMC-63A-53BC-user-manual.pdf)http://www.bestcutters4u.com/PDF/NCstudio.pdf

https://www.elephant-cnc.com/wp-content/uploads/2017/01/NC-studio-Gen6A-manual-V8-R6.pdf

[David Buchhauser]

Here are several videos pertaining to NCStudio.

https://www.youtube.com/watch?v=NtaKckKcgFw
428468


https://www.youtube.com/watch?v=p65zNjBNs3w
428469

https://www.youtube.com/watch?v=2B0sH53fpsE
428470

[David Buchhauser]

You can do a Google Search similar to the one shown below to find more information about your control software.
David


https://www.google.com/search?client=firefox-b-1-d&ei=7Zx1XtD7C4T--gShgpP4DQ&q=ncstudio+software+manual+english&oq=ncstudio+software+manual+eng&gs_l=psy-ab.1.0.33i160l3.5848.8082..11575...0.2..0.135.1270 .0j11......0....1..gws-wiz.......0i71j0j0i22i30j33i22i29i30j33i299.-a9jn39zA_A
428471

[David Buchhauser]

Do you already have the solenoid valve for the ATC? And are you wanting to know how to wire it up? Or are you looking to purchase one?
David

[Gary Campbell]

"I understand most of it, not sure what the 4120, 4202 and 4201 are,"

Brian...
System variables. For example, 4120 = Current tool