Questions on CNC Bits

[wsteffan]

I am looking to get a better result on my 2D/3D/Signs when using my CNC.

I have the Shark 60th, using the Bosch 1617.
Vcarve Pro 8.

I'm thinking my biggest problem is the bits.
I was looking at the Amana 2D/3D set and the Amana Carving set.
AMS-146
AMS-143
AMS-132


Does anybody know if these will work with Vcarve Pro and where can I import the tool paths from?

Any suggests on other CNC bits?
I'm not the best at Vcarve, so just looking for any tips.

Thank you
Wayne

[Rando]

If your bits are reasonably sharp, bad surface results are usually more about getting the feeds-and-speeds right. If the bit spins too fast and the head doesn't move fast enough, you'll get burn marks on the wood and the heat will dull the bit. If the bit spins too slowly, and the head is moving too fast, it will bog down, create a surface that looks hacked up, not smooth, and sometimes pull the material off the bed, or break bits entirely.

Getting that balance right is key to not only cutting properly, but also getting the most life out of your bits.

The other area to look at are things like stepover (how far over the bit moves on each line) and depth-of-cut (how far down it goes with each pass).

Getting all those things just right takes some learning, to be sure. But, once you get them dialed in, it will become just a normal part of getting your designs ready for the machine.

Thom

[wsteffan]

Thom,

Looking over some of my settings, I think your right about speeds/feeds.

I was looking over one of my bits 1/4 EM which I used to do roughing pass on a design.
That is the pass that is giving me the most trouble. Used 1/4EM for roughing.
I noticed the bit was black in color like it got to hot and burned. I never really noticed and burn marks on the wood, but the bit have marks on it,

Do you know any resources or help guides for the for the following.
Shark 60th
Bosch 1617.

Speed Rate, I think I have the same tooling setup for all the Em and the same for all the V bits so matter what size.
I think the bosch is set for max speed.

Most of the bits I have are yonico, or Kodiak.
I have the 1/2 V90 that came with the Shark.
Then I have about 30 Generics from China.
Funny the ones from China seem to do better. They are smaller in size 1/32 1/16 1/8.

Anybody else have suggestions, please offer your suggestions.

Wayne

[Rando]

Ouch! Blackened bits that have overheated are usually wasted, since the overheating kills the hardening, which dulls the bit pretty fast.

I have the same machine (60th), so we both have the "fun" with the flexing plastic parts. You can use pretty much ANY bit with the Vectric software, as long as it's not some weird shape. But even those can be accommodated. Ballnose end mills, flat-end end mills, tapered ball nose, v-bits, engraving bits, all of them can be specified with the Vectric software. But, the vectric software doesn't make decisions about whether the bit and material and feeds and speeds will actually work properly.

I do Aluminum machining, so my F&S are going to be different than your's. I use CNCCookbook's GWizard F&S calculator, though there are others (cheaper though less capable, IMO). The thing about F&S calculators is that they all use, at their base, the same set of calculations. They're a somewhat confusing, tangled web of relationships between bit size, bit material, the material being cut, the number of cutting flutes, RPM, how deep the cut is (depth of cut), how much of the bit's circumference is doing the cutting (stepover), and how much power the spindle (router) can provide, and how much torque the machine can handle without flexing and making the cut inaccurate. There's also flex that's influenced by the bit shaft diameter, and how far it sticks out of the chuck.

Another huge hazard for the bit comes from re-cutting chips that were just removed, but didn't get blown/vacuumed away. This is especially true in "full slotting" situations where there's no room on the front (where it's cutting), nor to the left or right of the bit. Since anything of any real depth usually takes multiple passes, there may be chips sitting in the slot as the bit comes through on the next pass.

Each material wants to be cut in a specific way by a bit of a particular cutting material. Hopefully I didn't just miss it, but what type of wood are you cutting. I'll use generic hardwood as an example. I have my calculations set at max 24K RPM, and 80 IPM cut rate. I've seen that the flex in the system doesn't usually let me get any above that, but I'm probably trying to get greater accuracy than you are, as I'm usually working in Aluminum, not wood.

1/4" 2-flute square end mill, cutting 1/4" deep, with 0.1" "step over" can be run at 18K RPM and 80 IPM for "roughing" operations
for "finish" operations, that same bit and cut should be run closer to 16K RPM and 10 IPM for a "fine finish" operation.

If you have a 4-flute end mill, you'll want to turn the RPMs down considerably, ideally by half, because it can remove twice as much material per revolution.

For a carbide 1/2", 2-flute V-bit at 1/8" cut (width is the same as depth with 90 degree bits), 17K RPM at 13 IPM.

Deeper cuts have to go slower, shallower cuts can go faster.

When choosing the (horizontal) stepover amount, avoid exactly 50%, since technically the very center of the bit isn't actually rotating, so very often that part of the bit is recessed or cut out. The amounts of stepover, and the kind of cut are typically like the following. Small percentages mean narrower cuts. The stepover can be thought of as either a dimension, or a percentage of the bit width, and is somewhat related to the surface finish you'll get.

Finish: <10% overlap (can do this pretty fast)
Light Roughing: 5-25%
Medium roughing: 25-50%
Hard roughing: 50-80%
Full slotting: 85+%

With full slotting, there's little or no room to the side of the bit for the chips to get ejected, so there's a big slowdown typically done there.

Anyway, definitely look into either a web site or an app to calculate the F&S. Vectric software allows you to enter the values, but it doesn't calculate "proper" values.

Anyway, hope that helps...it's part of the CNC learning curve. When bits go for $25 and up, and wasted material costs $$ to, learning to mater your Feeds and Speeds will be the single best investment of your time and (mental) energy. The CNCCookbook.com site has a LOT of great information about feeds and speeds.

Regards,

Thom

[wsteffan]

Thom,

I'm sure all he info you typed in your last post will really help.

I have the trial going already from the cookbook.

I printed out your post so I can keep going over it as I try and learn CNC better.

Thanks for the speeds/feeds info. I'm beginning to understand more how they work.

[wsteffan]

Tony,

Does more flutes mean better or is one of those it depends answers?

I am going to replace the bits that show burning on them and I was looking over your replies and that only thing I think was not mentioned was number of flutes.

Most of what I do is, 1/8 1/4 EM or Ball Nose right now.

Thank you
Wayne

[Rando]

Tony,

Does more flutes mean better or is one of those it depends answers?

I am going to replace the bits that show burning on them and I was looking over your replies and that only thing I think was not mentioned was number of flutes.

Most of what I do is, 1/8 1/4 EM or Ball Nose right now.

Thank you
Wayne

Glad you're starting to see there's a method inside the madness, Wayne!

"More flutes" fits right into the F&S equations. Each revolution of the bit takes that number of chips off the material. So for a given RPM and feed rate (inches per minute), a 4-flute can remove twice as much as a 2-flute bit of the same size. Which means that to keep the bit taking off the "proper" amount of material, the feedrate for a 4-flute bit needs to be aout twice that for a 2-flute. The issue with more flutes not always being better comes down to whether the machine can **accurately** move that fast. The more material removed, the more torque on the spindle/router, and thus the more flex in the system, leading to cut inaccuracies. The faster the system moves, the more acceleration-related positioning issues happen, sometimes even "losing" stepper-motor steps.

When working in Aluminum, 1/8" and 1/4" 2-flute bits fit best within our machine's capabilities for roughing and most finishing operations. An 1/8" bit needs to be spinning flat out (24K RPM) to get into the SFM range for the material, so a 4-flute 1/8" will need to be spinning likely faster than the router can go. For high-polish finishes in Al, I do use a 1/4" 4-flute bit, and it produces some very smooth surfaces. Like, nearly mirror-finish.

The recommended surface feet per minute (SFM) range for wood looks to be in the 650-800 range. So, a 2-flute bit is going to work well for most uses, which is what I've seen in most traditional router bits. I like 3-flute bits too, as they tend to vibrate/chatter less, and can run faster for a given RPM compared to the 2-flute. 4-flute ball-nose endmills are very common, and work well when doing 3D profiling, because they can handle the plunges more easily than a 2-flute can.

This link: http://acssgt01.tripod.com/documents/Sp ... _Feeds.pdf (downloaded PDF) has a chart of nominal SFM for some materials, in bits made out of High Speed Steel and Carbide. I've included a screen-grab of one of the tables in there. Wood can be very high with carbide bits; GWizard says to use ~1500.

SFM values for various materials

Well, back at it for me!

Regards,

Thom

[bmiestervs]

What are the best size bits to cut a bitmap of a picture. EG: Rose, Flower Design

[Rando]

That can come down to a couple questions:

How big is the final piece?
How much detail are you interested in?
How deep (into the surface) do you want the carving to go.

For a large (say, 18x12), you'd probably start with a 1/4" tapered ballnose (4 flute) for the roughing,
and then the finishing as an 1/8" ballnose.

For smaller things (like 8x10), you'd be more likely to finish using either a 1/16" tapered ball nose, and possibly even a 1/32" tapered ballnose.

The taper means the edges can't be perfectly vertical, but it makes for a much stronger mill that can better handle the 3D toolpaths produced by the Vectric software.

As for F&S, it's usually only going to be engaging the rounded tip of the bit, so use that diameter as the bit width.

There are also some shallow-cup ball end mills that can give a better surface with less "scalloping", or "cupping". To get a smoother surface, make the passes of the bit closer together. For faster material removal, use a bigger roughing bit with the passes farther apart, then have it do a final cleanup/finish pass.

Regards,

Thom

[bmiestervs]

My piece is 8" x 12" with the design in about a 4" x 4" area inside the piece. Deep enough to fill in with black or white paint over different colors to show the design. Thanks for the above info Thom.