# Advise on speeds and feeds for 3D



## SteveMI (May 29, 2011)

I am probably going to make my first attempt at cutting a 3D image on Monday. Going to be solid wood, most likely red oak or white oak. Yesterday I picked up some Amana bits and on Saturday will have some Whiteside bits.

The Amana are carbide tip half-round: 1/8" (45900), 3/16" (45902) and a 1/4" (45904). 

The Whiteside are solid carbide: 1/8" Ball Nose w/ 1/16" Radius (SC66), 3/16" Ball Round Nose w/ 3/32" Radius (RU1800RN) and 1/4" Ball Round Nose Bit w/ 1/8" Radius (RU2075RN).

The job will run on a Shopbot with 4 hp spindle and ER20 collet. CAM will be generated by Vectric V-Carve 8 Pro. Using the 1/4" for roughing and the smaller for finish.

So, what are the recommendations for speed and feed from the people with wisdom at this? Anything special with V-Carve? Can V-Carve do two roughing passes, such as my 1/4" and 3/16" before the 1/8" ?

I'm not concerned with the wood and cut time is less than 3 hours, but would like to have the bits to cut another day.

Steve.


----------



## honesttjohn (Feb 17, 2015)

Steve,

I got mine set at 18000 rpm and use that for most everything. 

What are you going to carve? And how big or how deep is the cut going to be?

HJ


----------



## SteveMI (May 29, 2011)

A smaller eagle like scottart does. It is 18" x 9" x 0.45" depth. My concern is the IPM and cut depth. Currently I have the job set for 0.125" pass depth and 100" per minute feed which I have used many times with a 1/4" end mill. For the finishing pass I have the job at 0.0625" pass depth and 50" per minute feed.

I don't do much raster type cutting unless pocketing. Just asking for any differences with 3D.

Steve.


----------



## Frazil (Apr 21, 2015)

You can do multiple roughing passes using VCarve Pro. You would calculate each one seperately. The first one could be a Z level roughing with a large bit and big stepover because it is quickest. If you do another one it should be a 3D roughing pass with the pass depth set to reach the bottom of the carving. The material allowance will still be left. If you do the second one as a 3D it won't re-cut all the air from the first toolpath. 
I have done several 3D carves this week. In walnut with a .75" ball nose for both roughing and final. And in hickory with a .5" ball nose roughing and .125" ball nose for final.
I often do a profile pass with the roughing bit in order to provide clearance for the small bit to start in a low stress area.


----------



## fixtureman (Jul 5, 2012)

Yo can run it as fast as your shopbot will run as it will never get to that speed. once the First pass is done there is very little force on your cutter so you should be able to go deep


----------



## SteveMI (May 29, 2011)

Frazil said:


> (1) The first one could be a Z level roughing with a large bit and big stepover because it is quickest.
> (2) If you do another one it should be a 3D roughing pass with the pass depth set to reach the bottom of the carving. The material allowance will still be left. If you do the second one as a 3D it won't re-cut all the air from the first toolpath.


I have VCP, so for your #1 step I would use "3D" with the largest tool, then another "3D" (#2) with second largest diameter bit as second roughing? Then use the final smaller bit for the Finishing cut. 

Steve.


----------



## fixtureman (Jul 5, 2012)

I run my shopbot with a 2.2 kw spindle at 12000 rpm and 6 ips or 300 ipm full depth using a 1/16 tapered ball nose bit for 3D work


----------



## MEBCWD (Jan 14, 2012)

Steve,

One thing to consider is the detail level of the model you are carving. If your 1/4" bit will cut all the detail of the model there is no need to use a smaller bit, it will just take longer and add ware and tear to the CNC components and bits. You can see the difference in VCarve when you run the preview of your toolpaths. Create finish toolpaths for each one of the bits and preview each one from the largest to the smallest (I normally zoom in on the most detailed part of the carving for the preview). If there is little or no change to the preview image when cutting with a smaller bit then use the larger tool at that point. 

You know how fast you can run your machine before it starts cutting badly so that is a good starting point for determining how fast you can go with 3d. Remember some ball nose bits don't have large cutting flutes so they will have to be feed slower. I would use a feed rate calculator based on the cutting parameters of each bit.

I use straight bits for 3d roughing most of the time but any bit you choose can be used for roughing, a ball nose bit will get closer to the finished model. I see no need in running several roughing passes with increasingly smaller bits.

Here are two things to consider when developing 3d toolpaths:

1. A 3d roughing pass cuts from the surface of the material and removes all the material inside the selected boundary leaving a machining allowance of material for the 3d finish toolpath. If you run several 3d roughing passes you are cutting air most of the time on the additional toolpaths. Just use one roughing pass with a large tool, small enough to get most of the material cleared, so the finish bit will not have to cut too much material.

2. A large project with fine detail that will have a great amount of waste material to remove might benefit from using the following approach: 
Duplicate the model and resize the duplicate adding the thickness of the material you wish to leave for the final finish pass. Turn off the original model.
Calculate a 3d rouging pass using the resized model with a really large bit and leave a machining allowance for the bit you will use for the special roughing toolpath.
Calculate a 3d finish tollpath using the resize model with a larger tool than you intend to use for the final finish (this is the special roughing pass). It will only machine the material left by the 3d roughing pass and leave material for the 3d finish pass. Another 3d roughing pass would cut air most of the time so doing this limits all the air cutting.
Turn off the oversize model and turn the original model back on, calculate a 3d finish tool path with your smaller tool you want to use to get the fine detail.
Run the toolpaths on your machine.
One thing to remember, don't use the recalculate all toolpaths feature because the model needs to be the right size for each toolpath.


----------

