Old World Map - A learning experience
I had to stop working on this for a while for a ski vacation last week, and then I had to do a couple of small jobs on the CNC before I could get back to this.  Doing those other jobs required me to take the map off the spoilboard, so before I did that I made a tiny hole with the 0.5 mm tapered ballnose end mill in the center of the project.  The job was designed with the center as X-Y Datum, so it was important that I know where that point is, exactly.  I put the board back on the spoilboard using the pencil marks I also made around the outside edges, but then verified the center was correct by lowering that same bit down to the hole to confirm.  It required a very small adjustment to get the two to line up, so I'm glad I did that and didn't just rely on the pencil marks.  

I wasn't happy with the look of the map from the first set of toolpaths.  Some of it was my own fault for lack of looking what each, individual toolpath was doing. It turns out the 1/8" tapered ballnose endmill, which was used for the clearing pass of the finishing cuts, was the final tool used in some areas.  I had used a 20% stepover with that bit in order to reduce the milling time, and that turned out to be a bad idea.  You can see the stepover lines really well in these two photos.

[Image: AL9nZEWtZ4ips6b-CwV_liLozWYO2hGuQo6dCAxA...authuser=1]

[Image: AL9nZEVLyBiQxtN1-F3Gki3nQVFpws1MxKbPB0op...authuser=1]

Not very refined, and not acceptable to me.  When I started reviewing what each toolpath was doing I figured it out, and the solution was easy, use a smaller stepover with that toolpath.  After some back and forth I settled on 6%, but of course that blew up the machining time to something like 75 hours just for that.  So I started looking at the speeds again, especially the plunge speed.  Each tool in the database has a recommended plunge rate.  For the 1/8" tapered ballnose endmill it's 90 ipm speed and 30 ipm plunge rate.  Some discussions on the OneFinity users' forum revealed that many folks are inputting the maximum plunge rate of the machine, which is 120 ipm, justifying the approach because it will almost never reach that speed because of the short distances involved which require acceleration/deceleration at each end.  So I set the plunge rate at 120 ipm, and left the speed alone at 90 ipm.  I also changed the rest machining from a mid value to nearly the coarsest.  Doing those two things brought the machining time down to about 27 hours.  Not great, but 2/3's better.  And here's what it looks like now:

[Image: AL9nZEUdV4LhHpeaGh0_oNffTIY7Q5G-9gJpKCoZ...authuser=1]

 In the next photo you can easily see the difference between the new toolpath in the lower half of this photo vs. what it was with the 20% stepover toolpath.  

[Image: AL9nZEVGbLoNEQY1lH4yMMaFWy756wl6BYNgzniC...authuser=1]

The wood almost looks polished now and a different color.  

So far so good.  I ordered a 1.5 mm (1/16") tapered ballnose endmill to use in the finishing toolpath.  It will run at 60 ipm and the same 120 ipm plunge rate.  I can't see the plunge rates on the computer screen when it's running, but I can see the X axis velocity.  With the 1/8" bit set in the program at 90 ipm, most of the time the actual rate is no more than half that.  I do see blips of 80 ipm but they are a very small percentage because there just aren't many flat areas on the carving.  I'm sure higher level controllers could do better, but this is what the OneFinity does with the Buildbotics controller, and a key reason I have to use a scale factor of nearly 3 for the projected time in V-Carve to match up with the actual time on the CNC.  You will be very surprised the first time you want to run a 3D carving in how long the actual carving time is compared to what V-Carve says if you use the stock value.  

Anyway, the toolpath for the 1.5 mill bit is going to take nearly as long at 22 hours.  I have looked at adding the 0.5 mm tapered ballnose endmill as a third finishing pass, which would also take around 25 hours, but will hold off on that until see what it looks like after the 1.5 mm bit has run.  More to follow as it occurs.  

The finishing pass finished last night.  Total machining time was about 60 hours for the roughing, rough finish pass, and final finish pass.  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. The roughness I had the first time I run this are completely gone now.  The 6% stepover on the rough finishing pass gave a smooth, almost polished finish on those areas that needed no further machining, like the surface of the hemispheres and the deep background, and the 1.5 mm did the same on all the intricate carvings.  I did no sanding; this is how it came off the CNC.  The wood is Sapele.  
[Image: AL9nZEWVCVa-EwBbJpJtTH0jPPYc4AU9SRkz6BnN...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.  

[Image: AL9nZEXqDOGmO-dVjHK6eE62ql-TBzSc8mu3NKjG...authuser=1]

[Image: AL9nZEUIgNBTzZ2YFhqonDRn1SXWlE5YGGOUG4IW...authuser=1]

[Image: AL9nZEXsfrqC34q1403iGEf_Cv5g3wQUkXLipbAA...authuser=1]

I'm continually impressed with what this machine can do.  


Forum Jump:

Users browsing this thread: 1 Guest(s)

Product Recommendations

Here are some supplies and tools we find essential in our everyday work around the shop. We may receive a commission from sales referred by our links; however, we have carefully selected these products for their usefulness and quality.