Roughing pass or no roughing pass for 3D project

[Bob Falk]

Hi, I purchased a CAMaster Stinger 1 2x4 (1.7kw spindle) a couple months ago and just completed my first 3D project (10"x10") in walnut shown below. Abstract artsy-fartsy piece.

445001
As you can see there are some rather deep cuts (up to .86 in deep). I did two roughing cuts. First with a 1/2" end mill (30 min) and a second with a 1/4 ballnose (1-1/2 hrs).

First roughing pass (1/4" steps):
445004

Second roughing pass (max depth 0.6"):
445003

Finally I did the finishing pass with an 1/8" tapered ballnose with a 1" cutting height (9 hrs). The finishing pass was with a 5% step over. The final finish was beautiful with only a couple of places with some torn grain that needed sanding (320 grit).

445005

Now to my question. Given the small stepover, is it possible to avoid the roughing passes and go directly to the finishing pass? Would save a couple of hours and bit changeover. I'm guessing the concern would be stress on the bit. However, I am assuming these bits are capable of cutting full height, but is it advisable for 9 hours? Any advice would be appreciated. Cheers, bob

[Mark Bolton]

First off, your first/last image is pretty sweet. Beautiful. Killing or reducing the roughing passes is going to do to two things, increase your number of finish passes, and depending on final finish pass reduce your final surface quality. Its a balance you you have to find that speaks to material, tool and machine rigidity, speed, and depth of cut. I would personally ditch the two roughing passes for a single roughing pass using the largest ball nose cutter you can run that will get into the detail and run as fast as possible ignoring your surface finish. Then hopefully you can have a single finish pass that will leave you with acceptable result. Second scenario would be two roughing passes with a large tool firs and the second tool only doing the final deep cleanup it can reach. You can fudge both of these in a program like VCarve Pro or you can do it with Aspire/Fusion and rest machining.

The answer with these to me is to rip off the roughing wide open as fast as your machine will run with the biggest tool possible leaving only what you absolutely need then get to your painfully slow finish pass.

[Bob Falk]

First off, your first/last image is pretty sweet. Beautiful. Killing or reducing the roughing passes is going to do to two things, increase your number of finish passes, and depending on final finish pass reduce your final surface quality. Its a balance you you have to find that speaks to material, tool and machine rigidity, speed, and depth of cut. I would personally ditch the two roughing passes for a single roughing pass using the largest ball nose cutter you can run that will get into the detail and run as fast as possible ignoring your surface finish. Then hopefully you can have a single finish pass that will leave you with acceptable result. Second scenario would be two roughing passes with a large tool firs and the second tool only doing the final deep cleanup it can reach. You can fudge both of these in a program like VCarve Pro or you can do it with Aspire/Fusion and rest machining.

The answer with these to me is to rip off the roughing wide open as fast as your machine will run with the biggest tool possible leaving only what you absolutely need then get to your painfully slow finish pass.


Makes sense Mark. I am hesitant to push my machine too hard without knowing the consequences.

[Mark Bolton]

Makes sense Mark. I am hesitant to push my machine too hard without knowing the consequences.

In my opinion in an operation like this there really arent any devastating consequences. Your either going to borderline stall your spindle (likely never happen) or break a tool (again likely never happen). Your machine can likely withstand 10X what your throwing at it. The end result will likley not be a machine issue but rather a finished product issue (bad finish).

The hard part with these textures is the finish pass is always painful and you have to do the math on post processing cleanup vs machine run time. Its very easy (for me especially) to want to speed up, increase stepover, get the part off the machine faster, only to result in a lot of painstaking hand work to clean it up. Flip side, machining the part like its a optical surface (slow, ultra tight stepover) makes a part that is unsaleable (whether that matters or not).

Your 9.5 hours seems a little steep. I 'd think your gains are in the roughing and cutting your finish by 2/3 and its still a long run-time part.

Youve got a stout machine. Dont be afraid of pushing it. They are thoroughbreds. They want to run. They protect themselves as well.

[Bruce Page]

Beautiful “artsy-fartsy” piece Bob, and congrats on the Stinger. I’m still loving mine. I will generally run one roughing pass with a .25 end mill on a piece like that. My main motivator is to reduce the wear & tear on the pricey tapered ball mill.
I’m retired and tend to baby my Stinger but you can push it pretty hard providing you have a solid work holding setup.

[Jim Becker]

I agree with Mark's advice. There are certainly sometimes when roughing passes can be skipped, but those are usually situations where the nature of the design doesn't put a lot of lateral load on the cutter. For most work that is complex and/or includes a lot of deeper plunges, roughing is essential to allow the finishing tool(s) to be able to work efficiently without extra load and resulting deflection. While this means a lot more time machining, the end result is always what's most important. My first major 3D job for a client included the "pleasure" of nearly 8 hour cut times. Per piece. Two required. Plus multiple test pieces because I was very new to it! That was a LONG, LONG week. Plus.

[Ronald Blue]

Great looking piece Bob. It's a learning curve certainly. I keep thinking I will get to the curve but not yet. So my suggestion would be to try more aggressive step over rates. I'm assuming you are using Vectric because I believe it comes with the Camaster. I believe it gives you an estimated run time when you calculate tool paths. See what more aggressive stepover rates do for the time and ultimately the finish. I'm nowhere near an expert here. Just an amateur still experimenting and learning as time permits. Following with interest.

[Jim Becker]

Stepover does need to be considered. Roughing is often done with the typical 41% stepover that's default for many tools. Finishing cuts are typically done with stepover between 5% for really critical surfaces up to about 11%, depending on the tool and the design. It can go completely the other way for special effects...Roger MacMunn's textured background technique for signs, etc., gets a 91% stepover and a different, smaller one for a more linen like effect. Stepover is your friend. :)

[Ian Stewart-Koster]

There are some great responses above.
If you omit a coarse roughing pass, and try and do everything with a tapered ballnose cutter,
Your first pass into the material will need to be VERY SLOWLY done.

It's cutting 100% of the cutter diameter in that first pass, even if the return path is only 5% to 10% stepover.
Watch you don't break the cutter if it plunges full depth in that first pass outwards.

If necessary set it superslow,cut out & cut back, and then restart the file with a faster pass for the rest of the job.

There are times in certain 3D jobs when a vertical edge does need to be vertical.
That's not going to happen with a tapered cutter.

Ive found for some jobs a 1/16" ballnose cutter with straight or parallel sides gave a far better finished job than the tapered cutter- but beware the cutter has to be long enough to be able to get into the bottom of some 3D pockets too, without the chuck scraping the keepable surface.

Onloy expereince will teach you where there are efficiencies to be made cutting corners, and where the long way might be better.

[Bob Falk]

Thank you all for the thoughtful and informative responses. Ian, I think you convinced me not to try to do this in one finishing pass. I am going to do some experimentation with stepover vs. finish quality.....I am hesitant to push the boundary on finish quality to much as I would rather the machine produce a nice finish rather than having to sand. Cheers, bob

[Ben Grefe]

Stepover does need to be considered. Roughing is often done with the typical 41% stepover that's default for many tools. Finishing cuts are typically done with stepover between 5% for really critical surfaces up to about 11%, depending on the tool and the design. It can go completely the other way for special effects...Roger MacMunn's textured background technique for signs, etc., gets a 91% stepover and a different, smaller one for a more linen like effect. Stepover is your friend. :)


Jim, I’m interested in the textured background technique. I looked up Roger (Rodger?) MacMunn and saw some nice sign work, but not many details on the textured backgrounds. Any links you know of?

[Wes Grass]

The hot setup, IMO, for this sort of thing is an 'extended reach' ball endmill. Not a long flute. They have standard length flutes, or maybe even stub, and a solid relieved shank above them for clearance. Much more rigid, much less prone to chatter and making your ears bleed from the screeching.

[Jim Becker]

Jim, I’m interested in the textured background technique. I looked up Roger (Rodger?) MacMunn and saw some nice sign work, but not many details on the textured backgrounds. Any links you know of?

It's actually relatively simple and just uses a pocketing tool path...actually two of them. The basic setup uses a ball nose cutter with the stepover raised to 91% and the raster angle set to 35º on the first pass and then to -35º for the second pass. The perimeter last pass only is used on the second toolpath. The resultant background is a cross-hatch type texture that paints up well or is nice even on oiled wood. Here's an example on a sign:

https://dm2305files.storage.live.com/y4md-t_rNlAuqJ9mjPTRueR-s0EkgvQZnh2dZH6UO_cvITZe71InmJStpq_Q5OgZlWJmNp85a9 wLF8IQ2L59qlIdqOnZsyHb2CjfRcSlpmHMy74JeHVorpqIx3t2 pu2qn5DwMISfqTEfjasC5xcXNFeCRigf48S8Lak2Wg1qzUNmum d2_ll9Hkemw7sTp8jjcjs?width=660&height=660&cropmode=none

A modification of this is to decrease the stepover and use a finer cutter (especially on small things), such as a very thin tapered ball nose...same technique otherwise. This gives a more linen-like texture. Example on this pet urn top:

https://sn3301files.storage.live.com/y4mc_e4Etun6a-fmataV0UIDe8n6B7ij2PB8Ul36crMUjAH3cEAKoWCn8qWmLrn0 qd8LkXRzIrbIm35gd9VDaSvIje0XSgn19j0j3V7HG3OTc1dvCx SAoPg3cvPY9KZfmOeSYdIWoAl2ncSiTrB3RtTk0tSi5S2oTE6h mF6YVj04IRg2N5f7WzM43NwgT5PDqsP?width=660&height=660&cropmode=none

[Jim Becker]

Thank you all for the thoughtful and informative responses. Ian, I think you convinced me not to try to do this in one finishing pass. I am going to do some experimentation with stepover vs. finish quality.....I am hesitant to push the boundary on finish quality to much as I would rather the machine produce a nice finish rather than having to sand. Cheers, bob

After looking at those photos, there's no way I'd try and do that with just a finishing pass unless it was something like HDU and even then, that particular piece of art would be pushing things. I "might" do it with one roughing and one finish, but I'd have to look at it a lot more in detail. I think you are being wise in realizing that getting a really good finish off the tool is a good thing with something like this because it's extremely difficult to sand out tool marks with all those nooks and crannies. :)

[Ronald Blue]

Okay, feed my ignorance please at the risk of hijacking the thread which I don't want to do. What is the "raster"? I saw that in the settings on Vectric and avoided it because well I didn't want to let Pandora out of her box. IF I need to do a separate thread say so.

[Bill George]

Do a quick Search on google and you will have your answer in less than 10 sec's., no need for a Thread.

[Jim Becker]

Okay, feed my ignorance please at the risk of hijacking the thread which I don't want to do. What is the "raster"? I saw that in the settings on Vectric and avoided it because well I didn't want to let Pandora out of her box. IF I need to do a separate thread say so.

When you use the pocket tool path in Vectric software, you have two choices for the "motion of the tooling" to cut out the material...Offset and Raster.

Offset has the tool start in the middle of the shape and work its way outward to the edges "in the shape" of the vector border, moving over with the requested stepover in the tool settings. The finishing pass is integral as the tool reaches the edge of the shape.

Raster causes the tool to move back and forth in straight lines, moving over with the requested requested stepover value in the tool settings. Raster cutting has options for changing the direction of the motion so you can follow the x-axis or the y-axis exactly or at any angle you wish relative to them. I often choose the angle that provides the "longest stroke" to cut fasters by taking advantage of acceleration) Raster also allows you to do a finishing pass around the perimeter of the vector, either before or after hogging out the material...or not at all. Most times, a finishing pass is done at the end of the material removal to clean up the little bit left. That's typically more efficient than doing it initially, but there's conceivably a reason where one might want to do it first I suppose.

The angle feature with raster cutting a pocket is what we take advantage of for the background effects I detailed in my most previous post in this thread.

BTW, cutting 3D shapes like the OP did can also leverage either Offset or Raster movement...cutting 3D is, if you think about it, a pocketing operation. It just has a variable depth, rather than a fixed depth.

[Ronald Blue]

Thanks for the detailed explanation Jim. I will experiment when it seems like a good place for it. I was experimenting with a 3d bird not long ago in VCarve photo and it ran at an angle rather than true to the X or Y axis. It automatically chose the most efficient cutting method for the tool paths which happened to be at an angle.

[Jim Becker]

VCarve Photo has some specialized capabilities that allow it to optimize for an image so that then end result is most accurate. When cutting "regular" 3D, 2.5F and 2D work, the decision is left to us to choose what we think will produce the best end result and/or be more efficient. Sometimes grain direction will matter. Sometimes it's about having "longer strokes" so that the machine can accelerate. I often try to accommodate both by orienting the stock so that both grain and distance can be optimized. After awhile, you start to get a feel for these things and they become habits.

[Brad Shipton]

Some of this will boil down to how many bits you want to go thru testing it. :) To me, it looks like the depth of cut is about 3/4". It will be the first plunges you would need to be most concerned with. If your first passes need to go to the max depth I suspect you could break a bit. Once you have made that pass and are only dealing with the small stepover, maybe it will work. That said, I have not tried this as I have always used the roughing pass. I agree with Mark. Use a larger hogging bit and speed it up. I usually use a 0.02" allowance in a single pass, but if you really want to fine tune the time you could increase the allowance so you reduce the z axis travel time. I have not broke any bits carving so far. I never find the roughing pass to be the problem for cut times and I have done a few pieces that took 36hrs to cut.

Adjusting your angle of cut for the one textured pattern will result in a cleaner profile, but you would have to consider how that might work for the reminder.