I chose to do a helical ramping at 30ipm into the material, and set the ramp angle to 1° (as per Christian’s advice in the instructable page, which makes a lot of sense, and should help a lot in not losing steps on your stock Z axis). That’s the red part above, and here’s a simulation of that part:
then the tool will take circular passes at the material, shaving off just a little each time (but moving fast, 60ipm). In that example I chose to apply the same settings as Christian: 8% of the endmill diameter, so 0.02":
with those settings, the three letters would be done in about 11 minutes. HOWEVER, for this test we will do, I suggest we dial back the settings to an even lower stepover, say 0.004" (still at 60ipm), and see if that works. If it does, then we can then easily increase that and find out when the machine/the tool gives up. That same toolpath at this 0.004" stepover at 60ipm would take 34minutes (but you wouldn’t have to wait that long: a couple of minutes should suffice to determine if the cut is good, and then we can move on to an incrementally larger stepover.
However this assumes the use of that other tool in the picture, that is only rounded at the tip, to be able to cut 0.25" deep in one pass. The ball tool is 1/4" in diameter, so it cannot take more than 1/8" in depth and you woud need two passes:
=> let me know which one you have and want to use, I’ll adjust the toolpath and post a first G-code test file !
Julien,
That is fantastic. Let’s use the ball end mill with the straight sides, not the in-cut.
I agree with the smaller stepover on the first attempt.
A couple of notes about why concrete is even more difficult than stone.
Most stone is relatively homogenous and therefore it is simpler to set up parameters for that type of stone.
Concrete has a very difficult mixture of softer abrasive particles of sand and cement. This is mixed with much harder aggregate. Sometimes, as is the case with the concrete in this mix, the aggregate is river rock and therefore smooth and round.
The abrasive particles will eat the electroplated coating and the hard, round aggregate will cause deflection of the cutting tool.
The combination of factors is the most devastating combination. This is true for large, heavy-duty concrete cutting machines and even more so for a small ball end mill.
It will be very interesting to see how the adaptive tool path will behave.
And you are correct, the tool is 6 shaft but the OD over the diamonds is .25".
Allright, so first the obligatory “use at your own risk” disclaimer:
running a G-code file from a stranger (me) is usually not a good idea. You will be able to at least preview/double-check it in any G-code viewer, e.g. this one.
since this toolpath/material combo is highly experimental, and even though I tried to use conservative settings, you may break the tool…
to match the rest of Christian’s settings, I suggest you set your router to 25000 RPM, that’s 4 on the dial. The higher the better (but the router screams at 30.000RPM, so 25k is probably good enough)
the settings are what I described above: 30ipm helical plunge at 1° angle, followed by adaptive clearing at 60ipm and 0.004" stepover and full 0.25" depth.
Fingers crossed, I’m curious to see the results!
EDIT: I forgot to add, that you may want to run the G-code file as an air cut first, to check that there is no obvious issue/surprise, at least for the first few seconds.
I would like to increase the overstep and run it again. The initial suggestion was .020 and it was run at .004. So let’s try .012 as the new step over.
The one minor issue is that it seemed to spall the edges just a bit more.
So now the decision is whether to move to Fusion 360. I am worried about your comment that it has a steep learning curve. CUrious about input on this from people who have made the switch.
Really impressive work! I recently made the switch to fusion 360. I started using carbide create and Vectric software for CAM earlier this year but I was finding it limiting in a lot of the same ways you seem to be. I can say there’s a lot to it at first so it is a little daunting but I went through all of the Fusion 360 CAM tutorials on the NYCCNC website and its all been much easier since then. I really love Fusion 360 now and most of my other CAD/CAM software has gone unused (Besides Vectric Vcarve since its so quick and easy for simple stuff).
P.S. I’ve also tried EstlCAM but find the lack of a preview option to be too nerve wracking. The fusion 360 preview is top notch and really helps to catch small mistakes before breaking stuff.
Glad to hear it worked out fine!
Here’s the same example file regenerated with a 0.012" stepover MAR_AdaptiveTest_0.012stepover.nc (1.1 MB)
If this works, we may want to try a slightly lower feedrate and check whether that reduces the spalling
About the chipped edges, what we could try is running a first shallow & slow regular toolpath (as you did initially), and then follow up with the adaptive clearing. Another approach which is typical when using adaptive, is to use some “stock to leave” in the adaptive clearning toolpath (which I have set to 0 in the examples above), and then follow up with a contour pass on all walls to shave off the remaining material (slower but at full depth).
I did not mean to scare you off from trying it, it’s actually not that difficult but there is an initial step that I estimate to be around 10 hours. Totally worth it if you ask me.
BUT if you consider it, do read the fine print about using it for a small business: it’s not free then. I think it’s reasonably priced given how incredibly rich and powerful it is, but it’s still a fair amount of money for a small business. If it’s only to have access to adaptive toolpaths, Estlcam may be a much cheaper deal and easier learning experience. If you intend on investing time in modelling and advanced CAM, then go for it, Fusion360 is awesome!
Julien - I will be headed to the shop late this morning to see how new tools paths go.
I saw that you posted the 0.0.12 stepover path and was going to ask you now for the other files. But you anticipated that question. So thank you for the .016 and .020 stepover files.
Hmmm. I didn’t know that Fusion360 was a CAD/CAM platform.
I have a OnShape license so I am not inclined to get into another CAD program. OnShape has a number of CAM plugins. On first glance VisualCAM appears to the first choice, though not free.
I’m not familiar at all with Onshape, it does seem like VisualCAM implements “high speed machining” (so likely adaptive toolpaths). Another option could be to do the CAD in Onshape and the CAM in Fusion360 but of course that would be a less convenient workflow.
Julien - here is the update.
Concrete is such a difficult material to work with being non-homogenous.
Overall the the adaptive toolpaths are much faster. So we are absolutely on the right path. Here is a video of the 0.020" stepover. https://youtu.be/6DB4Zf2K1do
The downside is that the Z axis was skipping on all three of the trial runs Sunday. When the aggregate is hard, the forces are just too high for the stepper motor to hold. The worst attempt was made when the plunge hit a hard piece of aggregate on the plunge. Skipping like a kid with a jump rope. Obviously the depth control was, well, not in control. Need that HDZ upgrade!
The comment about the non-homogeneous material is related to the small inside of the A was knocked over during the milling process. However, this is not due to the toolpath or speed of travel this is due to the material that was supporting the small column. The top and bottom A are broken and the middle is still standing. The middle had a piece of aggregate that the center of the A was carved out of.
Quite interesting. So 0.02" radial stepover it is, for now.
I can see how the Z axis would skip steps in such a demanding material, however:
I can’t quite picture why the first helical ramping zone in the M went deeper than the surrounding areas that were milled in the adaptive circular passes. If the Z motor lost steps during the plunge, I would expect the cut to be shallower than designed, but then at whatever max depth it started the post-ramping part of the toolpath it should have proceeded at constant Z from there, because then the Z axis does not move anymore. I’ll have to think about this and take a look at the toolpath simulation to figure this one out.
Sure the stock Z axis is less rigid that the HDZ, but I wonder if in this specific scenario we are not limited by the Z motor torque anyway. Do you want to try dialing down the forces during the ramping? We could either slow down the helical ramping feedrate, or reduce the ramping angle further, or a combination of both. We could also play with the diameter of the ramping helix.
This is why I posted the picture of the M with the circle. This is was a second attempt to recut the M. The surrounding depth is from the first pass when the Z skipped and was shallow. So this is not really a mystery.
However,
It is very difficult to tell in the pictures but the 0.20" stepover also lost it’s Z-axis mind when cutting the M. It went much deeper. I checked the the tool was not loose - it wasn’t. I have been setting the tool to the maximum depth into the router so that it bottoms out anyway. So this did not make sense.
I know that the Z can skip when cutting at a fixed Z depth. This is becasue the force pushing up overloads the stepper motor’s ability to hold in position. This happens when the piece of aggregate is very hard and using a ball endmill.
I do not think this has anything to do with the motor torque. There is absolutely no pitch change that would indicate the overloading of the motor.
I think slowing down the helical feedrate and angle would both be a good idea.
WIth the HDZ is there a gearbox between the stepper and the shaft or direct drive? The reason I am asking is to understand how much more stability in height there will be.
First - I’m really impressed with this concrete milling.
Second - the HDZ has a ballscrew driven by the stepper so it is inherently geared down a lot from the belt drive, downside is much slower rapid retracts, upside is it can push down hard enough to bend your spoilboard and break end mills, I don’t think Z position will be an issue for you once you have the HDZ.
All clear now, thanks. @LiamN answered about the benefit of the HDZ (but you were convinced already…and I know it’s no fun that they are out of stock)
Regarding the toolpaths, I’ll regenerate a few combinations of ramp rate/angle and post them here later today.
I took this project on very naively. Thought I knew about machining and concrete cutting. I mean, how hard can it be? Once we get this all tuned up and we do the real project I will be share on this forum. I will just say that it is part on an installation project at a state park. I am getting some serious pressure for having to push the schedule out until the HDZ is available.
Thank you for the clarification on the Z-axis. Geared down is good and a thread will not slip or skip so this will be a huge improvement.
