Hi Arthur, maybe, depends on what you have now? Struggling with power? Your depth of cut and feed rate is more constrained by machine rigidity, so keep that in mind. Gary
Ok. I have the stock router 11. I was told that with a 1/4 inch bit I probably shouldn’t cut deeper than 1/8 per pass on MDF. I haven’t made any cuts yet because I am unable to control the speed rate or depth of caught yet. I’m still working on that. I was just thinking if anybody has successfully installed a larger horsepower without any modifications.
The 1/2 diameter is a rough guideline for starting out. And it's not a HP constraint. You will get chatter from flex on a hobby machine before you stall out the router11. But yes people have put bigger routers on their machines. Experiment with what you have before dreaming of Titan cnc level material removal! Cheers Gary
You can get 8mm ER11 collets. I saw a previous post where you wanted to cut deeper because you were using a down cut that had up cut at the end of the endmill. If you are worried about tear-out just use a straight flute endmill. I use these all the time for wood so I do not get tear-out. I can easily cut wood profiles at 2500mm/min (100ipm) using the 1/2 endmill diameter for the depth. I always do a roughing cut and leave a little stock to clean up with a full depth finishing pass. Lately, I have been cutting a little deeper (about 4mm with a 6mm end mill) and have had no issues. I use the 8mm ball nose end mills when I want to rough 3d carves. I do 4mm deep passes at a 40% step over at 3000 t0 3500 mm/min depending on what type of wood. I have never observed the need to get a larger spindle. As Gary said, the spindle can put out more power than the frame can handle. I have accidentally cut 1/4" aluminum in one pass as well as the a bit of the spoil board below it because I forgot to re-zero my Z axis after a tool change. The cut was ugly and did not quite follow the path it was supposed to due to flexing in the framework. The router did not seem to be affected much, other than slowing down a little.
High Speed Machining strategies are the solution to HP-limited MRR, not spindle upgrades. (I'm just gonna quote-reply this post forever, I know)
Thanks for the info. I have quite a few kitchen cabinets to make and my mentality is bigger must be better but more passes is the way to go. My problem now is trying to figure out how to control the speed and the feed rate. I can’t figure that out. I’m assuming the software I use is supposed to do that but any chance I make in the feed and speed makes no difference when I actually start to cut. The software I am using is Mozaik but if I can figure out how to design a test project with the provider software of the machine, I would like to see if I have the same issue.
You set the speed in the software that generates your gcode (CAM software). What are you using? If it is Vectric, you set the speed, step over, depth of cut, etc when you enter the endmill into your endmill database. If it were me and I was cutting wood, I would start with 100 ipm (2500 mm/min). I have never had an issue cutting woods and plastics with that speed. If it works well at 1/2 the diameter for depth of cut, increase the speed a bit, or the depth of cut until you get your machine dialed in. One of the things that will really take time off of a job, especially 3D carves, is getting your acceleration rates maximized.
Here is a video that shows where these numbers are. It is similar to Vectric. The question is, do they have a grbl post processor? I did not see one.
Arthur, have you looked at the video on the Mozaik website? At about 4.03 mins, it shows the tab for feeds and speeds etc. Home
I did see that video and I even received 5 hours of training from Mozaik. The even set up my libraries and showed me how to set my depth and speed pervoas but for some reason it didn’t work. I have opened a ticket with there help desk
you coudl also search and replace the existing numbers in the Gcode file with new numbers. if you post a sample Gcode file here we can check for other problems as well.
Post the code that it's outputting so we can see what it is/is not doing. If it doesn't have a grbl post-processor you'll probably have to output the most generically-compatible version of the code and spend a little time in Notepad++ cleaning it up with regex find-and-replace.
I think the problem must be with Mosaik because I have been able to control the speed in the feed with the provided software Mosaik has a ticket open and is looking at the issue as well
I think the problem, maybe with Mosaic because I can control the speed with the provided software that came with the machine. Mosaic has a ticket open and is looking into the problem.
I see and 'M3 S18000' line which is commanding 18000rpm however, this won't work unless your GRBL settings are correct for your spindle. look at $31 and $30 in the GRBL setttings, the defaults are 0 and 1000 but for your code to work the max setting must be the max for your spindle.
Yeah this trips a lot of people up. I don't really understand why it's trying to set a feed rate for a G0 in line 12 since G0 rapids are set to the maximum acceleration/speed of the machine hardware (controllable in grbl's parameters), but it does set a 5080mm/min feed rate under the first G1 feed block on line 15. Then it ramps down in Y, then comes back the way it came really fast, plunges down 3/8", comes back the way it came in Y some more, etc... Then cuts full depth around two more sides of the rectangle. This is a very odd, inefficient strategy to me, maybe someone who deals more in wood panel cutouts will understand it better. Personally I'd set it to ramp down 2mm around each full cutout (so 0.5mm per side) and keep the feedrate up there around 5000mm/min or as high as the machine can go (I'm not convinced that's 10160mm/min though...?). You could actually hand-write that code once you know the outside corners where the tool head needs to be in order to get the correct internal workpiece size.
My apologies, I may have use my terms incorrectly. I shouldn’t have use the term speed and feed what I meant was how deep it cuts and how fast it travels my router has a manual dial.
This would be depth of cut, or DOC, and feed rate, or feed, which is correct. Speed always refers to spindle speed (or, more accurately, actual surface speed of the cutter blades on a mill and the workpiece on a lathe)
Oh my that is way above my skill set. I am very new and do not understand much of anything right now I’m waiting on the Mosaic support team to see if the problem is on their end because I did program the feed rate at 100 in./min. and a cut depth of 1/8 And when I place the work piece on the table with out a bit installed it cuts half inch deep and it runs at 130 in./min.
Seems like it because 5080/25.4 = 200IPM (maybe grbl's settings are maxing out at 130IPM/3300mm/min there, which is good to protect the machine) and those Z-13mm blocks that you see are the half-inch DoC. One of the most important things you can do when getting into CNC is learn G-code- how to read it, how to write it (for very basic things). For example, in your case the outside dimensions of the actual cutter path appear to be X1212.775mm, which is 47-3/4" *including* the cutter diameter, and Y1166.775mm, which is 45-15/16" including the cutter diameter. So we could write that as a square ramp-down starting at the G54 origin like this: G21 G54 G90 G0 Z38.1 (Safe Z-height) G0 X0Y0 (Go to G54 origin) M3 S1000 (Max spindle speed at grbl default, doesn't matter for your manual router) G0 Z1 (Drop to just above the workpiece) G1 Z0 F1000 (Touch workpiece gently) G1 Y1166.775 Z-0.5 F5000 (Go to top left corner) G1 X1212.775 Z-1 (Go to top right corner) G1 Y0 Z-1.5 (Go to bottom right corner) G1 X0 Z-2 (Go back to starting position at bottom left) And then you'd just continue copying and pasting this section, dropping in Z each time: G1 Y1166.775 Z-2.5 (Go to top left corner) G1 X1212.775 Z-3 (Go to top right corner) G1 Y0 Z-3.5 (Go to bottom right corner) G1 X0 Z-4 (Go back to starting position at bottom left) Etc, until you hit the bottom of your workpiece or, if you want to keep it attached, maybe skip the very last line and trim off the last 0.5mm along the bottom edge by hand. Hopefully this was clear and helpful, but until Mozaik figure out what's going on, knowing the basics is what keeps the work flowing. Now, to be clear, this is just to cut out a rectangle. If you have hinge pockets to add or inlaid handles or anything like that, that gets slightly more complex with arcs.
That is actually very interesting advice. I have been doing a lot of research on everything but how to read and write G code. I am going to work on that next.
some posts do that because GRBL insists that a feeedrate be set before the first g1 move, and since they coudl not figure out how to ensure an F word on the G1 line, they set it early as a default. most controllers don't care that F is on a G0 line, it just has to be set before the first G1/2/3 move.
ah, ok, missed the clues (-: what are you max rates for the machine? I see in the code speeds over 10 meters a minute, which is pretty fast
In his other thread Error 9 Locked out LEAD1515 standard profile set XY to 3500mm/min As I mentioned in the other thread, I think he is hitting max rate
Interesting. I don't remember running into an issue with that, but the only times I've deliberately put it on the first G1 line were with LinuxCNC. Normally it's in the header block because I secretly love global variables.
