[neeboy]

Hello to all:

I would like to get a small cnc machine to make detailed architectural wooden blocks; I have been looking at small machines like Zenbot, Romaxx, Taig mills, etc. I have also been experimenting with Vectric's 3D cut, and after playing with the program, I'd like to know where to get info on machining speeds for wood. Please take a look at the attached pics; these are from Cut3D. The pic is a 1.5" cube, and the defaults in Cut3D say it will take an hour to machine this thing using the settings shown. Is that really true for say, hard maple?? I'm very much hoping not, but I need to find out before I go any farther.

This block is a very simple one; there may be a faster way to machine this specific block using other tools besides a CNC router, but a lot of my designs are more complex and I'm using this example as a starting point. Thanks in advance for any informed replies!

[Phife]

3d objects require a ballnose bit and several passes with a small stepover to make curved surfaces look smooth.

1 Hour is probably a little slow for a 1.5" half sphere, but it all depends on your machine, how fast it can move and how rigid it is.

On my machine it would take probably about 30mins to make that.

[ger21]

I'd use a 1/16" tool, and up the feedrate to 100-150ipm. If you want it really smooth, leave the stepover at .005". That should get you closer to 10 minutes, if the machine can do it.

[todd71]

I'd sub it out to a "lathe" shop. Take less than a minute with the right set up. I dont know what your shop rate is, but an hour for a part like that is a waste of time. Unless you got the time to wait. :cheers:

[rich909]

Hi Neeboy --

I don't use 3D Cut, but I do use Vectric's V-Carve Pro and I am guessing the machine time estimate calculation may be similar.

My experience using v-carve pro is that the machine time estimate is about 2x what the actual run takes. What I normally do is save the tool path(s) that make up the job and load the code on my mach-3 controller system and run it there ...in "simulation mode". That produces a time estimate that is very accurate.

Unfortunately, if you are using the 3D Cut trial, you probably can't save the toolpath (g-code), and if you only have a trial version of Mach-3 you can only run up to 500 lines of code, so you probably don't have that option.

As you say, this is a "simple" example, that might be better done on a lathe, as was suggested. But for your more complex designs, you might divide the 3D Cut estimate you get in half to see if it makes sense.

--Rich

[jeffrey001]

On the estimated machining time on VCarve Pro, you can adjust the ratio to get a closer estimated machining time. If your machine always take 1 hour instead of 30 minutes, just add a ratio of 2 to 1 on the scale factor input tab.

You can adjust it very precisely by experimenting different scale factor.


Jeff

[rich909]

On the estimated machining time on VCarve Pro, you can adjust the ratio to get a closer estimated machining time. If your machine always take 1 hour instead of 30 minutes, just add a ratio of 2 to 1 on the scale factor input tab.

You can adjust it very precisely by experimenting different scale factor.

Jeff

Hi Jeff --

You are correct. I checked my scale factor and IPS settings on a couple of jobs I ran yesterday and the V-Carve estimates were right on target with the Mach-3 simulation estimates and actual run time. The scale factor was 2:1, which I think was the default setting and explains the est. time being twice the actual. Once I changed it to 1:1 and set it for my tool speed the estimate was accurate.

Thanks for the clarification.

--Rich

[louieatienza]

I actually had to make something similar for a cabinet project a long time ago. If I had to make exactly what you show, in quantity, on a CNC, I would either locate a non-piloted roundover bit or take a piloted rondover bit and have the pilot removed by a machine shop. You would then use a large straight bit to hog the circle perimeter, and the roundover bit to do the ball, which would be basically a profile toolpath set half the bit-flat away... Could go real fast if you do it in multiple pieces...

[Delw]

The fastest way to make this part hands down is a cnc Lathe.
there are many ways to hold a square block in a lathe.
A cnc Mill will take about an hour or so depending on the rpm of the mill. the step over you need will be mainly detailed to the bal endmill you are using, with a 1/4" ball endmill and a nice finish you really need to run .002 step over. that will take some time to run. the other thing with most mills and cheaper programming software your not going to be able to run arcs, you will be stuck with polylines IE line segments.
your program will also need .005 in between each line segment or less along with the .002 step over. this makes for a HUGE program in excess of 3-5 megs(guestimate)
with the .0312 rad ball nose endmill you picked your going to need to run a MAXIMUM step over of .002 to get a decent finish.

Delw

[twoartistic]

I do a lot of complex shapes in expensive woods. I don't want to have any tear out, so I am careful in my raster angles and step over and feed rate. A fairly good rule of thumb for my machine, the depths that I cut, the material, etc. is 1hr per 40,000 lines of g-code.

I have done a few jobs that had a lot of the same parts (240 shaped door panels) With that many panels it was worth the time to maximize every cut and rapid move. I could do a 32"x26" pyramid shaped panel, using a 1.5" end mill in about 8 min.

Most of the time I don't worry about how long it will take to run a program. It would take longer to refine the toolpath, feed rate, rough cuts, etc to make it worth fussing with.

Here is a sample of my work if you want to get a reference to the kinds of shapes I create. Animoto - Shane McKenna Engineer - Designer - Artist - Craftsman

[louieatienza]

I actually had to make something similar for a cabinet project a long time ago. If I had to make exactly what you show, in quantity, on a CNC, I would either locate a non-piloted roundover bit or take a piloted rondover bit and have the pilot removed by a machine shop. You would then use a large straight bit to hog the circle perimeter, and the roundover bit to do the ball, which would be basically a profile toolpath set half the bit-flat away... Could go real fast if you do it in multiple pieces...

Still can't remember what the bit is called... a raised flute bit? But with a decent spindle it would take literally seconds to do this on a CNC router.