World Map

[John TenEyck]

I just finished this last night. Total machining time was about 60 hours for the roughing, rough finish pass, and final finish pass on my CNC. The little Makita router ran like a champ, never even got warm after the roughing passes were done. Anyway, here it is after finishing with Danish Oil. I did no sanding; this is how it came off the CNC. The wood is Sapele and the size is 14 x 26"

https://lh3.googleusercontent.com/pw/AL9nZEWVCVa-EwBbJpJtTH0jPPYc4AU9SRkz6BnNzWJkISCgNMwDR0_5FEsI7I 0lRda9LPsALoNvct6DfN8UEdh6jiTZnn9CjHAJEjgTtqFM67IA BNPcMhg9xbCbIHqCFRoORgG1f6sRLIw7pNpOTTckSoeWlA=w15 88-h893-no?authuser=1

There is more detail that could be gotten by running another finishing pass with a smaller diameter tapered ballnose endmill, but I'm not going to do that for fear of creating sharp contour changes that give an unfinished look, which is what happened the first time I ran this. That means some of the lettering isn't as clear as it could be, which I would like to be able to mill separately, but I don't know how to parse that out of the STL file. So this is it. The level of detail is still pretty amazing, with all sorts of things going on in the background.

https://lh3.googleusercontent.com/pw/AL9nZEXqDOGmO-dVjHK6eE62ql-TBzSc8mu3NKjGMvggb6YV22eKz9fAEm1inYKlAyT0KgssZN_zI Paw4G9YE4dxm05Otj9jqQPnZJZ5k7BQrwAMfBz1_rdNNHY_PxW KJFOuWr3Shnm8ZNvX4YPzrW7k5NhNVw=w1588-h893-no?authuser=1

https://lh3.googleusercontent.com/pw/AL9nZEUIgNBTzZ2YFhqonDRn1SXWlE5YGGOUG4IWgm-T9V63KxbkdcNgrzkuusrF4ox_s2rYOAJbKkYsv9-CCwNaDuOiv9wpacOdZRo5CGllZ68TcnY6wls-zn_M4X-eR__i7NHg3oAdzVaJHoas7uHermFJwg=w1588-h893-no?authuser=1

https://lh3.googleusercontent.com/pw/AL9nZEXsfrqC34q1403iGEf_Cv5g3wQUkXLipbAAfa_tqrGwk3 H0jQccdaq71O_Ggq7UcUzQfv_0nxgXtjN8igCYIpzLe5pAflLf aTKBr2kBiIFuz5dbTdWtqvcCThgj8k0Jhvg_YYy6HgtwFzygsf VOdTe_3A=w1588-h893-no?authuser=1

I'm continually impressed with what my CNC is capable of. And before anyone says, yeah, but you're just pushing the button and the machine does everything for you, I'll point out that there is a lot of decision making and trial and error involved in selecting the right milling bits, sequence, speeds and feeds, and several other parameters that make for success or failure.

John

John

[Chris Walls]

That's very nice !!

[Kris Cook]

John - that is pretty awesome.

[David Falkner]

That looks fantastic!! I've never used Sapele on the CNC but now I want to find a suitable project.

[Steve Eure]

Extremely intricate. Very nice. I showed my wife, who is into lasers, etc. and her response was, "whoa". That means well done sir.

[Mel Fulks]

I would not have believed that was possible by any means other than about 30 to 50 years in a prison cell ! Extraordinary! Gonna send all
my modeling clay ash trays to the basement !

[Bruce Page]

Great job John. I haven’t cut any sapele but want to! Can you provide a link to the model?

[Jim Becker]

That's a beautiful end result John. Sapele works pretty much the same as true mahogany in my experience. I've cut both on my CNC with outstanding results. They maintain detail nicely. There is interlocking grain, but the CNC doesn't care so much, especially with detail carving like that.

[John TenEyck]

Great job John. I haven’t cut any sapele but want to! Can you provide a link to the model?

Thanks for the kind comments, all. Bruce, here's a link to the Etsy vendor I bought the file from. https://www.etsy.com/listing/1016850010/world-map-3d-stl-model-cnc-router?click_key=8a106adab0d8bedc08f555e4b49974a51 0b0b765%3A1016850010&click_sum=85750614&ref=as_recently_viewed-3&pro=1&sts=1

I used a 1/4" ballnose end mill for the clearing pass, then a 1/8" ballnose end mill for the rough finishing cut, and a 1.5 mm ballnose end mill for the finishing pass. There is more detail to be gotten if you can figure out how to get it w/o making it look ugly, as it did for me when I first tried it with a 0.5 mm ballnose end mill for the finishing pass.

As Jim said, Sapele machines beautifully on the CNC. Honestly, I did no sanding on it. What you see is how it came off the machine. Good luck.

John

[Bruce Page]

Thanks for the link. How much step over did you use?

[Andrew Hughes]

It is pretty spectacular John. I haven’t a clue what the programming side entails.
My first thought how did you keep the piece from warping as wood was removed?
Prayer ,Luck, sorcery ?
It just seems impossible but there it is.

[Christopher Charles]

Whoa-that’s next level!

[John TenEyck]

Thanks for the link. How much step over did you use?

I used a 1/4" BN EM with 40% stepover for the roughing cut. Then I used a 1/8" tapered ballnose endmill for the clearing finishing pass at 6% stepover, followed by a 1.5 mm tapered BN EM with 8% stepover for the finial finishing pass. I'm using VCarve Pro. The key one in my opinion was with the 1/8" tapered BN EM, because it's the one that does the finishing work on the surface of the hemispheres and deep flat areas. Having said that, a guy on the CNC forum I participate on said hogwash, forget the two step approach and just run the 1.5 mm bit with 8% stepover on a 45 deg raster cut. And he even said at 300 ipm. I don't know if it would look as good, but the simulation does look good, and takes the machining time down from over 48 hours for the two-step finishing approach to around 13 hours. I don't plan to make another one of these but when I do something similar I definitely will try a test piece to see how his recommendations work.

John

[John TenEyck]

It is pretty spectacular John. I haven’t a clue what the programming side entails.
My first thought how did you keep the piece from warping as wood was removed?
Prayer ,Luck, sorcery ?
It just seems impossible but there it is.

Thanks Andrew. I bought my CNC to do furniture and cabinet work, but it's fun to see what other things are possible on the art side of computerized woodworking. I bought the STL file from a person on Etsy, so they did the hard work. All I had to do was figure out a combination of toolpaths to carve it out of a thick piece of wood. Vectric's tutorials are top notch IMO, and I followed their recommendations for the most part. I had already done a few other 2.5D carvings, so I knew the approach to use, or should I say, one approach. There's no right or wrong, only what works for you. I probably spent 2 or 3 hours fooling around with various combinations of toolpaths that looked good on the simulation but was "only" 60 hours of machine time. Later, some folks have told me that with a different approach, using fewer endmills, I could do it much faster. I've looked at that idea on the simulation and if it worked it would take the total machine time down to about 20 hours. Pretty huge.

Ha, funny you should mention warping. It did exactly that the first time I ran it. After the roughing was done, I noticed on the first finishing pass that the bit was cutting deeper in some areas than others. Hmm. Then I saw that the workpiece had bowed up on the ends. Well, that explained that. What to do? I used washer head screws all around the perimeter to flatten the workpiece back down to the spoilboard. Then I reran the entire process with the toolpaths set to eliminate the deepest overcut, about 0.080". And what you see is what I got. The workpiece is still bowed a little, but it's only going to hang on the wall so I'm fine with that. It would be interesting to see if a vacuum table would have held the workpiece flat.

John

[Kris Cook]

Thanks Andrew. I bought my CNC to do furniture and cabinet work, but it's fun to see what other things are possible on the art side of computerized woodworking. I bought the STL file from a person on Etsy, so they did the hard work. All I had to do was figure out a combination of toolpaths to carve it out of a thick piece of wood. Vectric's tutorials are top notch IMO, and I followed their recommendations for the most part. I had already done a few other 2.5D carvings, so I knew the approach to use, or should I say, one approach. There's no right or wrong, only what works for you. I probably spent 2 or 3 hours fooling around with various combinations of toolpaths that looked good on the simulation but was "only" 60 hours of machine time. Later, some folks have told me that with a different approach, using fewer endmills, I could do it much faster. I've looked at that idea on the simulation and if it worked it would take the total machine time down to about 20 hours. Pretty huge.

Ha, funny you should mention warping. It did exactly that the first time I ran it. After the roughing was done, I noticed on the first finishing pass that the bit was cutting deeper in some areas than others. Hmm. Then I saw that the workpiece had bowed up on the ends. Well, that explained that. What to do? I used washer head screws all around the perimeter to flatten the workpiece back down to the spoilboard. Then I reran the entire process with the toolpaths set to eliminate the deepest overcut, about 0.080". And what you see is what I got. The workpiece is still bowed a little, but it's only going to hang on the wall so I'm fine with that. It would be interesting to see if a vacuum table would have held the workpiece flat.

John

John - just a thought. Is there enough thickness to make some relief cuts on the back? Would that help with the warping long-term?

[John TenEyck]

John - just a thought. Is there enough thickness to make some relief cuts on the back? Would that help with the warping long-term?

I thought about that, Kris, but it's only about 1/4" thick at the bottom of the carving. It's cupped less than 1/8" now. I hung it on the wall today and it can't be seen. BTW, I used a new to me picture hanging system. The wall I hung it on has a pocket door inside, so I had to use something that would work with the approximately 3/4" thick plaster coated drywall without going through. These worked great.

https://www.homedepot.com/p/PicGenie123-Picture-Hanging-Kit-40-Piece-Hangs-Pics-Up-To-50-lbs-4-Pack-N50-MK4S/306800860

John

[Jim Becker]

I used a 1/4" BN EM with 40% stepover for the roughing cut. Then I used a 1/8" tapered ballnose endmill for the clearing finishing pass at 6% stepover, followed by a 1.5 mm tapered BN EM with 8% stepover for the finial finishing pass. I'm using VCarve Pro. The key one in my opinion was with the 1/8" tapered BN EM, because it's the one that does the finishing work on the surface of the hemispheres and deep flat areas. Having said that, a guy on the CNC forum I participate on said hogwash, forget the two step approach and just run the 1.5 mm bit with 8% stepover on a 45 deg raster cut. And he even said at 300 ipm. I don't know if it would look as good, but the simulation does look good, and takes the machining time down from over 48 hours for the two-step finishing approach to around 13 hours. I don't plan to make another one of these but when I do something similar I definitely will try a test piece to see how his recommendations work.

John

You'll really have to do some experiments with what works best with your machine for these cuts relative to paring down. I generally have used a tapered BN for a single finish cut about the same size as you. You may need to adjust your Z speed in VCP as it's often set quite slow compared to the horizontal feed speed and Z is a "yuge" factor in cut time for 3D models. I frankly set it at about the same as the horizontal speed and let the machine deal with how fast it can actually move. Your step overs are reasonable for fine detail, IMHO.

[Frederick Skelly]

That's really nice!

[John TenEyck]

I set the plunge (Z) speed to 120 ipm, for the long finishing passes. That's the maximum rate for the stock Z-axis on my machine, so I can't go any faster with that parameter. In all cases, that's faster than the recommended plunge speed for the bits I used, by up to 3X. You might want to look into that with your 3D carvings.

John

[Andrew Hughes]

John Thanks for replying back to my post.
The map is the coolest piece I’ve seen made with cnc.
Good Luck Always

[Jim Becker]

I set the plunge (Z) speed to 120 ipm, for the long finishing passes. That's the maximum rate for the stock Z-axis on my machine, so I can't go any faster with that parameter. In all cases, that's faster than the recommended plunge speed for the bits I used, by up to 3X. You might want to look into that with your 3D carvings.

John
I generally set the Z to about 200 ipm if the horizontal speed is running in that range. The machine will never exceed what it's capable of, of course, but it will also not be limited to some artificially low value since 3D carving naturally has a whole lot of Z axis action to do the job. My machine has 900 oz NEMA 34 steppers and there's an air assisted counterbalance on the Z axis to counter the weight of the spindle for best performance up and down, particularly in the up direction...the stepper doesn't' have to work so hard lifting the heavy spindle.

[John TenEyck]

I generally set the Z to about 200 ipm if the horizontal speed is running in that range. The machine will never exceed what it's capable of, of course, but it will also not be limited to some artificially low value since 3D carving naturally has a whole lot of Z axis action to do the job. My machine has 900 oz NEMA 34 steppers and there's an air assisted counterbalance on the Z axis to counter the weight of the spindle for best performance up and down, particularly in the up direction...the stepper doesn't' have to work so hard lifting the heavy spindle.

As you said, there's a lot of wasted time with the Z-axis when doing 3D carving. I'm limited to 120 ipm, no matter how high I set it, so there's nothing to be done unless I want to upgrade to 1F's new heavy-duty Z-axis which has a faster max. speed. At this point, I'd get a spindle before spending even more on the new Z-axis. From what some are suggesting on the CNC forum I look at, there are other ways to potentially reduce carving times, so I'm going to explore those first.

FWIW, the little Makita router showed no signs of problems running those long carves. It's removing so little stock it doesn't even get warm. I'm sure the runout is higher than with a spindle, but the results speak for themselves, whether doing carvings where it probably matters less, or cutting parts for clocks where it does really matter. A higher level machine would be nice, but at this point there's no burning need to justify the money. I haven't paid off the money I have in this one yet, but I will.

John

[Jim Becker]

I was only relating to how I put the settings on my machine and why, John, and making no negative commentary or comparisons.

As to carving time, a lot of that is figuring out what stepover does the job for acceptable surface quality. It can be amazing how the expected carve time changes. While I honestly don't trust the time estimates in the Vectric software relative to actual accuracy, they are at least good for comparing what the effect of changes are to something like stepover. A few years ago when I was doing those magnolia carves for a big old house (and completely new to 3D modeling/carving) I had the same fun you are having right now trying to work out what was the best set of choices 'cause I wasn't going to sleep in the shop. :) (fortunately, actually can pause a job with some controllers when necessary for bathroom and meal breaks!)

[Keith Outten]

Beautiful work John

[John TenEyck]

I didn't take offense, Jim, I was just explaining the limitations I have.

Too high a stepover on the first finishing pass is one of the reasons I had to do the carve a second time. I didn't realize that it was the final pass in some areas, so I set it at 20% to reduce the time; of course that left unacceptable ridges. I ended up using 6% stepover with that pass and that's what you see on the hemispheres.

The time estimates in Vectric are only that, but they can be very useful if you are running similar projects, and if your machine provides a time estimate when you load the file. There is a scale factor in the time estimate window which you can adjust to bring the estimated time in line with the actual time on the machine. My machine gives a very accurate estimate of machine time when I load the file, within a second, so I know how long it's actually going to take, and can go back and adjust the scale factor in Vectric if it's off, and also rethink the machining strategy if it's unacceptable. My machine has a pause feature, fortunately, which works seamlessly, at least so far. On these 24+ hour toolpaths I would start them whenever I got to, hit the pause button before bedtime, and hit the run button when I got up the next morning. I let them run whether or not I was in the shop, but never if I was going to leave home. I have a Wyze camera on it and can check it on my phone, and I go physically check if I hear anything odd. It's not loud upstairs, but I can hear it humming and moving.

John

[Jim Becker]

I forget what the stepover was that I used for that "yuge" carve I mentioned, but I think it was in the 8% or so range for the finishing pass. I didn't do it diagonally as these were 4' long pieces, so I followed the grain on the axis I had the workpiece oriented to; y in my case.