# Help with 3D



## Rusty Nesmith (Feb 1, 2020)

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 (Jan 3, 2012)

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

David


----------



## honesttjohn (Feb 17, 2015)

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 (Feb 1, 2020)

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 (Feb 1, 2020)

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 (Feb 17, 2015)

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 (Nov 12, 2012)

What are your step overs for both bits?


----------



## Pro4824 (Oct 17, 2015)

gwilki said:


> What are your step overs for both bits?


Yep!


----------



## Rusty Nesmith (Feb 1, 2020)

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


----------



## Gaffboat (Mar 11, 2012)

Rusty Nesmith said:


> 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 (Feb 1, 2020)

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


----------



## stevenrf (Jul 30, 2010)

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 (Sep 25, 2014)

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 (Feb 1, 2020)

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 (Jan 14, 2012)

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 (Feb 1, 2020)

MEBCWD said:


> 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.
> 
> ...


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 (Nov 12, 2012)

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 (Feb 17, 2015)

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

Told ya MEBCWD had the knowledge.


----------



## BalloonEngineer (Mar 27, 2009)

MEBCWD said:


> 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 (Feb 1, 2020)

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


----------



## Rusty Nesmith (Feb 1, 2020)

I made the changes in Vcarve pro and it took it from a 1.5 hour cut to a 3 hour cut.


----------



## MEBCWD (Jan 14, 2012)

Rusty Nesmith said:


> I made the changes in Vcarve pro and it took it from a 1.5 hour cut to a 3 hour cut.


What % of stepover is it set on now? Did you adjust your feed and plunge rates to 150 inches/min? Remember you changed the stepover from 10% to 25% so that is what made it 1.5 hours instead of 3.5 hours. It should be okay at 10% but don't go above that. Also remember until you cut a few 3D projects and find the actual time with these settings you can not adjust your scale factor in the time menu, the times shown could be off quite a bit so for now don't worry about the times shown.


----------



## MEBCWD (Jan 14, 2012)

Rusty Nesmith said:


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


Your pass depth will not affect your 3D work because you will not be leaving very much material for the finish pass when you do your roughing pass. I always leave at least 0.03 for the finish allowance when roughing, larger projects I might leave more because I'll be using larger bits.. 

If you are not doing a rouging pass then you will be cutting all the material in one pass. This is okay if your cut length on your tool is long enough to cut the full depth and the toolpath starts at one edge and continues across the model. This works because of the small stepover (6% > 10%) required for 3D toolpath.


----------



## Rusty Nesmith (Feb 1, 2020)

MEBCWD said:


> What % of stepover is it set on now? Did you adjust your feed and plunge rates to 150 inches/min? Remember you changed the stepover from 10% to 25% so that is what made it 1.5 hours instead of 3.5 hours. It should be okay at 10% but don't go above that. Also remember until you cut a few 3D projects and find the actual time with these settings you can not adjust your scale factor in the time menu, the times shown could be off quite a bit so for now don't worry about the times shown.


Stepover set at 10% feed and plunge set at 150. Now I have a new problem I can’t figure out. Zero is set to the center of the project. In vcarve when I run the tool pass everything is fine. When I take it to the machine and zero everything to the center of the project and start the 3D carve it goes to the bottom left and wants to cut a straight line all the way across the board.


----------



## difalkner (Jan 3, 2012)

Do you have just the shell carving selected?

David


----------



## Rusty Nesmith (Feb 1, 2020)

difalkner said:


> Do you have just the shell carving selected?
> 
> David


Yes


----------



## MEBCWD (Jan 14, 2012)

Rusty Nesmith said:


> Stepover set at 10% feed and plunge set at 150. Now I have a new problem I can’t figure out. Zero is set to the center of the project. In vcarve when I run the tool pass everything is fine. When I take it to the machine and zero everything to the center of the project and start the 3D carve it goes to the bottom left and wants to cut a straight line all the way across the board.


Can you post your design file so I can look at it?

You can drag the file to the section under the text entry box of your post and it will upload to the post.


----------



## Rusty Nesmith (Feb 1, 2020)

MEBCWD said:


> Can you post your design file so I can look at it?
> 
> You can drag the file to the section under the text entry box of your post and it will upload to the post.


I hope this is what you asked for.


----------



## difalkner (Jan 3, 2012)

I think Mike wants the actual file, Rusty, not a screenshot of it on your computer.

David


----------



## MEBCWD (Jan 14, 2012)

Rusty Nesmith said:


> I hope this is what you asked for.


That is not the design file but the pictures look like you have a Zero Plane which is right but you don't want to machine the Zero plane because it is just a big flat area outside the model (dish with shell) you want to carve. The rest of the design is all 2D carving.

Go to the modeling tab, *select* the dish/shell model and *click* on the "Create vector boundary around selected components" button. Then go back to the toolpath tab, *double click* on the Finish toolpath, *select* the vector you just created and *choose* "Selected Vectors", then recalculate the toolpath.

What was happening was, you were trying to machine the entire zero plane so your time for the finish pass was too high. 

I don't know why it would start in the lower-left corner and cut a straight line to the other corner. When you save your cut file what post processor are you using?


----------



## MEBCWD (Jan 14, 2012)

I just reread your description of how it was cutting and realized you said cutting from the lower-left corner across the board (not to the upper corner), so for how you had it setup that would have been right because it was trying to raster across the board to machine the whole zero plane, just like you told it to do.

One other thing to check would be, check the settings on the Material Setup Menu on the Toolpath Tab. * Select* gap above model and set it to 0.00. If you had to make that change, recalculate all toolpaths.


----------



## Rusty Nesmith (Feb 1, 2020)

Thank you very much Mike. I went in and set the boundary and recalculated like you said. It still looks good when I run it in the program. It changed the cut time from 3 hours down to 39 minutes. I have to run a few errands and will try it when I get home.


----------



## Rusty Nesmith (Feb 1, 2020)

Mike adding the boundary did the trick. Thank you very much for your help. Thank you to everybody that replied. It took longer to cut than it said but I had a lot of other things to do in the shop so not a big deal. Here it is cut out. Still have some sanding and painting to do.


----------



## difalkner (Jan 3, 2012)

How long did it take, Rusty? Looking nice!

David


----------



## Pro4824 (Oct 17, 2015)

Looks great Rusty! Now we expect pictures of all your future projects!!


----------



## Oscar36 (Feb 23, 2019)

Ditto on the comments. Looking good. Making clocks is addicting. Watch out.


----------



## Rusty Nesmith (Feb 1, 2020)

difalkner said:


> How long did it take, Rusty? Looking nice!
> 
> David


David I wasn’t paying close attention. At the half way point it was at 45 minutes. The next time I looked over it was done and the router was at zero running but doing nothing. Around 2.5 hours for the total project.


----------



## MEBCWD (Jan 14, 2012)

Rusty the carving looks good. Looks like you might have a problem with bleeding from the black. You might try using a couple of good coats of sanding sealer before using the black, make sure you let the sanding sealer dry before you do the black. 

If I remember your pendant will show you exactly how long it took and then you can use that to set the scale factor in the software so time estimates are closer. You will never get it perfect but will get you closer.

Overall this was a good project, good design and carving. The bleeding problem is just part of the learning curve and you will find out what works for you.


----------



## honesttjohn (Feb 17, 2015)

Mike, that's not bleeding. It's the individual wood personality coming thru.


----------



## Rusty Nesmith (Feb 1, 2020)

I think it will come out with a little sanding. I didn’t do much sanding yet.


----------



## Rusty Nesmith (Feb 1, 2020)

Here it is finished.


----------



## FixitMike (Aug 14, 2011)

One thing to remember is that when the tool path combines X or Y and Z movements, it will move at the slowest feed speed specified for the tool. Increasing the plunge speed usually help. Also, in VCarve or Vspire, setting some small value for 
Z2 such as .03" will mean the tool can move to that depth at a high speed when moving to a new location.


----------



## Rusty Nesmith (Feb 1, 2020)

Somebody saw the clock and wanted to buy one so I made another one. It took 70 minutes the cut the 3D Scallop shell.


----------

