[Rusty Nesmith]

I designed a clock for my wife. The 3D part in the center is 5.8 inches in diameter. It says it will take around 8 hours to do that. Are there any tricks to speed that up any? Here is a picture of what I am doing.

 

[difalkner]

What are your feeds/speeds/bits used, Rusty?

David

 

[honesttjohn]

Also - what machine do you have? Does it have leadscews or rack and pinion? Also are you doing a roughcut first? 3d carving is not fast with a small machine. My Avid CNC carves 4 times or better faster than my Probotix.

I can set the Probotix to 200 ipm but it never reaches that speed carving, and very rarely on a straight cut. It will stay in the 15-35 ipm while carving. The Avid CNC whizzes right along at over 3-400+ ipm if set to that. I'm most comfortable around 180 to 250 ipm.

Your settings have a lot to do with it, but with a hobby machine it still boils down to the fact that 3d carving is slow going compared to other things. Another thing to consider - the computer's timelines are seldom right, even if you have the correct settings because of the up and down of the cutter. That is not a complicated model so it should whiz right along - but only as fast as your machine's capabilities.

 

[Rusty Nesmith]

I have a piranha XL. It has the screw drive. I am doing a rough cut with a 1/4 inch ball nose end mill. 16,000 rpm, pass depth .1 inch, feed rate 60 in min. Finish cut is a 1/8 inch ball nose. 16,000 rpm, pass depth .1 inch, feed rate 50 in min. I changed the pass depth in the program and it didn’t make much difference. The rough cut will take 42 minutes. The finish cut will take 7 hours 46 minutes. Everything looks fairly quick except the finish cut for the 3D.

 

[Rusty Nesmith]

Ok I just went into the program and changed the feed rate for the 1/8” ball nose to 100 in min and it cut the time down to 3 hours 53 minutes. Is it ok to run that fast and if so should I turn up the rpm? Also is there a chart somewhere that tells how fast the different bits can be run?

 

[honesttjohn]

MEBCWD can answer those questions quite accurately. You can set it to 200 ipm, but chances are it'll never reach those speeds. Watch your velocity rate and you'll see exactly how fast you're really running. 100 ipm is no problem, IF you can get to cut that fast. I doubt it. And don't rely on the computer times until you've had some experience doing 3d carving. Chances are it'll be slower than the program says unless you adjust it. Remember, 3d carving ain't fast!!

I've eliminated the rough cut on carvings that aren't complicated or deep.

 

[gwilki]

What are your step overs for both bits?

 

[Pro4824]

What are your step overs for both bits?

Yep!

 

[Rusty Nesmith]

Step over on the 1/4” is .025 and the 1/8” is .0125.

 

[Gaffboat]

Ok I just went into the program and changed the feed rate for the 1/8” ball nose to 100 in min and it cut the time down to 3 hours 53 minutes. Is it ok to run that fast and if so should I turn up the rpm? Also is there a chart somewhere that tells how fast the different bits can be run?

I replicated your 3D carving in V Carve, Rusty, and I got a carve time a lot faster than yours. I set up a 5.8 inch carving of the shell using a 1/4” ballnose for the rough carve and a 1/8” for the finish carve. My feed rate on the finish carve was 60 ipm with a step-over of 8%.

My total carve time shows 1 hour and 40 minutes. I suspect I know what may be your problem. Did you set your carving boundary to the Model Boundary or the Material Boundary? The reason I ask is that when I set the finish tool path to the material boundary (assuming 12” x 12” stock), I get a carve time of 8:04:03 hours. Since the rest of your design is a standard v-carve, you don't need to waste time on the 3D carve with the tool working over the entire piece.

I also noticed that for the shell design, the roughing carve removes very little material. If it were me, I’d eliminate that tool path and go with only a finish carve.

 

[Rusty Nesmith]

Thanks Oliver for the tip. I will go in and check that. I am using Vcarve pro.

 

[stevenrf]

I think this is the correct answer to your problem. Just watch the step over and set the material boundary..
Bin there : done that.

 

[PhilBa]

10% stepover is too low for roughing. OK for detail. You are probably spending most of the time roughing, counter to the whole point of it, I'd experiment but even as high as 70% is probably be ok.

 

[Rusty Nesmith]

On the finish cut I raised the step over from 10% to 25% and it changed it from a 3.5 hour cut to a 1.5 hour cut. The cut boundary was already set correct. Much happier with the 1.5 hour cut. I deleted the rough cut. Wow so much to learn. A big thank you to everybody that helped it is greatly appreciated.

 

[MEBCWD]

Rusty the finish pass needs to have the stepover set around 6 to 10 percent. The time shown in the software for a toolpath is just an estimate and you need to use the scale factor to get a closer estimate for your machine, tooling and your settings. You have to use your machine and keep track of the actual time it takes to cut files then use the scale factor to adjust to the actual time it took. Of course, this actual time will vary for different bits and settings but will give you a better estimate.

I own a Piranha FX. The Piranha is a good tight little machine compared to the larger Sharks so you can set higher feed rates but remember it will only go as fast as the controller can run it.

Another thing to remember with 3D work is that most of the movements sent by the controller are short movements so the stepper motors never have a chance to accelerate to the feed rate you set.

For that 3D toolpath on my Piranha, I would run the finishing toolpath with the 1/8" ball nose at 150 inches/min feed rate and plunge rate, 12000 rpm with the stepover set to 8%. It will never get to 150 inches/min but will be cutting as fast as the controller will allow it to run.

If you think it is running too fast you can use the FRO on the pendent to slow it down.

 

[Rusty Nesmith]

Rusty the finish pass needs to have the stepover set around 6 to 10 percent. The time shown in the software for a toolpath is just an estimate and you need to use the scale factor to get a closer estimate for your machine, tooling and your settings. You have to use your machine and keep track of the actual time it takes to cut files then use the scale factor to adjust to the actual time it took. Of course, this actual time will vary for different bits and settings but will give you a better estimate.

I own a Piranha FX. The Piranha is a good tight little machine compared to the larger Sharks so you can set higher feed rates but remember it will only go as fast as the controller can run it.

Another thing to remember with 3D work is that most of the movements sent by the controller are short movements so the stepper motors never have a chance to accelerate to the feed rate you set.

For that 3D toolpath on my Piranha, I would run the finishing toolpath with the 1/8" ball nose at 150 inches/min feed rate and plunge rate, 12000 rpm with the stepover set to 8%. It will never get to 150 inches/min but will be cutting as fast as the controller will allow it to run.

If you think it is running too fast you can use the FRO on the pendent to slow it down.

Thanks. I will go back in and change the settings and recalibrate it. I am already using the 1/8” ball nose. Thanks again.

 

[gwilki]

If my math is correct, your roughing cut is set to a 10% step over. Since it is a roughing cut, you might want to increase that to at least 40%. I realize that the roughing cut is not the big time user, but it's a start.

 

[honesttjohn]

I use an end mill for roughing, not a bigger ball nose with 5-30% stepover.

Told ya MEBCWD had the knowledge.

 

[BalloonEngineer]

For that 3D toolpath on my Piranha, I would run the finishing toolpath with the 1/8" ball nose at 150 inches/min feed rate and plunge rate, 12000 rpm with the stepover set to 8%. It will never get to 150 inches/min but will be cutting as fast as the controller will allow it to run.

I hope you noticed that Mike recommended that the plunge rate is the same as the feed rate, this is a huge time saver in 3D carves. As he says, 3D carves are all short G1 (straight line) moves. If plunge rate is lower than feed, it will slow feed for most moves (to move in a straight line).

 

[Rusty Nesmith]

What about pass depth? Mine is set at .1 inch.