Cutting BB

[Dan Richeson]

So the speeds they have listed is not a good speed? What should one be running the 1/2" bits at? I'm guessing their is some kind of formula? thank again Dan

[Michael Burnside]

So the speeds they have listed is not a good speed? What should one be running the 1/2" bits at? I'm guessing their is some kind of formula? thank again Dan

The formula boils down to chipload.

Chipload = feedrate / (RPM * number of flutes)

Basically what you're looking to get out of the cutter is nice chips of a certain thickness depending on material. If you search for "chipload" you'll usually find a table that lists the material, bit diameter and target chipload. The right sized chip will help pull heat away and keep the bit cool. Too small of a chip (or dust) and the bit gets hot and it breaks. Often people associate this with moving too fast, when in fact, they should just lower the RPM. Too large a chip and you'll tear the material or, obviously, break a bit. One rule of thumb to stick to until you really understand things more, is keep each pass close to no more than the diameter of the bit.

Many years ago I read a post from, I believe Gary, that said something like, you want to have as high an RPM you can to prevent tearing and once you've got that, figure out how fast you need to move (feed) for the chip load. That's the best starting advice I have. Hobby CNCs that can't control speed muddy the waters and confuse people because they're stuck at 18000-36000 RPM usually chiploads are WAY too low. There are a myriad of YouTubers, etc make it worse by passing bad info to the CNC community.

Since you have an AVID, you CAN control speed, which means you're well on your way to getting a handle on chipload. A lot of exact chipload comes with experience and all hardwood isn't the same. I usually recommend people start out with 70-80% of the chipload target and see how it goes. For example, maybe the ideal chipload for walnut is 0.009" with a 1/4 tool, so instead try 0.007. This means you'd setup your toolpath for 1/4" depth of cut, 200IPM (196 but I rounded) and 14000 RPM. See how it goes. A machine like an avid can do 200IPM all day long. Now, if you want to do a 1/2" bit, that's a monster and you can double the chipload. Larger bits are a little more forgiving, so maybe shoot for 10K-11K RPM and 250 IPM and test it. That's a lower chipload, but high enough that the bigger bit should be just fine. A 1/2" bit can probably handle more than your machine is capable so you'll need to learn those limits.

[Dan Richeson]

Thank you very much for the reply. I meant to say 1/4" but will look up the chip feed rate like you said. I don't mind taking a extra pass to save a bit and have a better finish right now. The 1/4" bit and no more than 1'4" path is a good one to remember.

[Jim Becker]

I'll add that part of the chip load challenge with non-industrial machines is that they just cannot move (feed rate) all that fast which makes things hairy if you do not have the granular control of RPM via software with a spindle. A machine may be able to do 300 ipm in a long straight line, but not in short distances with turns, etc. Routers motors can only slow down so far, so if you can't move them through the material fast enough, getting proper chip load can be nearly impossible. (and that makes breaking tooling a lot more common as someone already mentioned due to heat build up...the chips are what takes the heat away)

[Brian Tymchak]

Interesting thread as I just overheated a bit. Need to learn more about chip load.

I'll second the use of a compression bit. I use a Whiteside for this with the first pass at least .25"/6mm to insure that the up-cut portion is below the surface and the top surface is maintained cleanly.

Jim, are you creating a specific toolpath for this first pass with a slightly deeper cut, then another toolpath for the rest of the cut? Or all subsequent passes at the same depth as the first?

Thanks!

[Dan Richeson]

I found this chart from carbide processors. So with wanting to stay with in the feed rate chart green area. This chart did not separate the type of wood but for the speed of 160 that the white side file had for it the RPM should be much lower than the 16 or 18 k the file had for that bit also. More like 12 to 13 k rpm. White side files are way off it seems. Plus on 3/4" need to to at least 3 passes with a 1/4" bit.

With looking and messing with a chip load calculator I found here online which is better to get your number in the range? Lower the spindle speed or speed up the feed IPM? It showed hardwood at .009-.011 with a 1/4" bit 2 flutes. To get a .009 chip rate it shows 180 IPM and 10K rpm. That seems fast IPM and really slow for a 1/4" bit. I used to just running a hand held router at 20K for that small of a bit.

[Michael Burnside]

Interesting thread as I just overheated a bit. Need to learn more about chip load.

Jim, are you creating a specific toolpath for this first pass with a slightly deeper cut, then another toolpath for the rest of the cut? Or all subsequent passes at the same depth as the first?

Thanks!

No, you just need to modify the first pass of a given toolpath one of two ways after clicking the "Edit Passes" button. 1) adjust the slider or number so the first pass is at least 0.25" as Jim outlined. 2) Check the box "Maintain exact tool pass depth" and click "Set Passes"

I do (2) 90% of the time as I have my tool's max-depth set to spiral change depth + 0.007 which is pretty close to the Whiteside bit at 0.25"

[Michael Burnside]

I found this chart from carbide processors. So with wanting to stay with in the feed rate chart green area. This chart did not separate the type of wood but for the speed of 160 that the white side file had for it the RPM should be much lower than the 16 or 18 k the file had for that bit also. More like 12 to 13 k rpm. White side files are way off it seems. Plus on 3/4" need to to at least 3 passes with a 1/4" bit.

I wrote my own calculator (I'm a software nerd) that gives me multiple options simultaneously based on IPM or RPM or chipload and +/- 5/10/15%. That said, this is a good link to start from:

https://gdptooling.com/chipload-calc/

I've found most manufactures tool databases are garbage. I download them but pretty much modify the depth of cut, IPM and RPM right away. I have my vectric database broken into hardwood, plywood/mdf, acrylic (I rarely use this one).

With looking and messing with a chip load calculator I found here online which is better to get your number in the range? Lower the spindle speed or speed up the feed IPM? It showed hardwood at .009-.011 with a 1/4" bit 2 flutes. To get a .009 chip rate it shows 180 IPM and 10K rpm. That seems fast IPM and really slow for a 1/4" bit. I used to just running a hand held router at 20K for that small of a bit.

It's counter intuitive, which is why so many YouTubers and content creators get it wrong. Remember, depth of cut is only 0.25" (the bit diameter), don't go deeper until you really know what you're doing (or have an industrial, rigid machine). For hardwood I try to shoot for around 10k-13.5k RPM. Softer woods higher RPM, harder woods, a little slower. MDF/PLY are a little faster RPM/IPM. My tool database is setup for the hardest and I will tweak as needed. At these speeds and extensive testing, the wood NEVER burns, cuts are always nice and the IPM is in range that my machine can handle.

So with 0.009", I have my 1/4" downcut setup by default to 210 IPM and 13k RPM which yields around 0.008" (always use a ramp with up/down cut endmills). For upcuts I usually push harder at 220IPM. I've cut miles of wood with 200-220 IPM with a 1/4" endmill. It's been a long time since I broke a bit and when I did, I realized I was a moron and changed my RPM to 18K somehow. Plywood like BB I think I'm closer to 260-275 IPM, but I like to spin faster for the veneers so I usually start around 13-15k. If the wood looks ok at 11-12k with a quality bit, lower IPM and you're good. If not, spin faster and move quicker... Generally, for 1/4" endmills, I target 0.0065-0.009 for hardwoods, 0.009-0.011 for most Ply and MDF 0.015...that stuff is butter

These numbers I'm quoting aren't even "pushing" it for an AVID PRO or my machine. It's just properly setting up. Sometimes YouTubers will say, "oh I just want to be conservative" or something like that. Not realizing that over-heating the bit is THE worst thing you can do to reduce life. A dull cutter that isn't broken is no better than one that is sharp and broken. Get your chiploads close and they'll last a long time. It doesn't have to be exact - drop it down to 0.007 or 0.008" chipload and test, just get close to the target and see how your machine/material perform. Some people say listen to the machine/wood. I don't get that. Trust the numbers and look at the chips and cuts. Once you trust them, you'll be able to adjust as needed and you'll be able to detect when your cutter needs sharpening.

As Jim points out, if you're using a hobby CNC with a router, then it's really hard to control and picking an IPM at 18-24k would be basically impossible. So, people compensate by taking shallower depts of cut, etc. The bit still heats up but it's less likely to break in those scenarios.

[Jim Becker]

Jim, are you creating a specific toolpath for this first pass with a slightly deeper cut, then another toolpath for the rest of the cut? Or all subsequent passes at the same depth as the first?

I use Vectric software and would do a cut like this with a single toolpath and multiple passes. I would adjust the number of passes (at least on my machine) to have at least a 6mm depth of cut when using a .25" compression tool to clear the switchover and maintain a clean top. Depending on the material, I might make it a heavier cut per pass with less passes. My machine "can" do 18mm material in two passes easily, but I'd rather do three on anything important for better cut quality and less deflection. .25" tools do "bend" if you force them too hard...

The only time I ever do a separate toolpath over the same vector is if I've chosen to use a downcut for some specific reason to clear the top layer first and then I switch to an upcut piece of tooling to remove the rest to the required depth. I don't like using down cut tools for deep cuts, especially for profiles because the really pack the swarf into the cutline and not only does it make cutting harder, but it raises the risk of fire from friction. (really...it does)

Now I used a phrase above, "at least on my machine". Everyone has to get to know their particular machine very well so they understand what they can push and what they have to be more conservative about. After owning my machine since early 2018, I kinda know what works and what doesn't and it's been quite a long time since I've broken a tool while cutting. (Knock on, um...wood)

[Brian Tymchak]

Jim, Michael, thanks for the detailed replies. I use Carveco Maker and can't find any comparable parameters to manipulate depth of cut per pass. Well, not fully true. I can set depth of last pass. It may be a more advanced feature reserved for the premium versions. I'll look deeper.

Thanks again.

[Jim Becker]

I'm not familiar with Carveco Maker. In the Vectric software, there are two opportunities to determine pass depth. The first is in the tool library...a default max pass depth for a given tool (and one can make multiple copies of that tool and configure them for different purposes/material). This setting, if you change nothing else, will allow the toolpath generation to determine the number of passes required for the total depth of cut specified for the toolpath. Now in the toolpath generation process, Vectric also allows one to manually change the number of passes for a given tool (including separate settings where there is more than one tool being used for a toolpath, such as for clearing and final). I actually use this a lot rather than changing my tool database or making the tool inventory unreasonably complicated. I kinda know at this point what's possible/reasonable for depth of cut for a given tool in a particular materai since I've been using the machine since spring 2018. So I tweak it while creating the toolpath. The one downside to this is that if I change the depth of cut for that specific toolpath, the calculation defaults back to the settings in the tool inventory. So I try to not make many manual changes until I have things worked out and make those adjustments just prior to writing out the toolpath file(s). (I generally only write one file as my machine has automatic tool measuring and will ask for a tooling change when it's required)

[Michael Burnside]

Jim, Michael, thanks for the detailed replies. I use Carveco Maker and can't find any comparable parameters to manipulate depth of cut per pass. Well, not fully true. I can set depth of last pass. It may be a more advanced feature reserved for the premium versions. I'll look deeper.

Thanks again.

Sorry about that Brian. I don't know Carveco very much, wish I could help further. I imagine a poor mans version is as Jim outlined with a tool database that has the max depth set to the depth you want the pass to. However, I don't know if that would always work depending on material thickness and number of passes configured or calculated.

If your machine is supported, I do recommend giving Vcarve or Vcarve Pro a test run.

[Brian Tymchak]

Sorry about that Brian. I don't know Carveco very much, wish I could help further. I imagine a poor mans version is as Jim outlined with a tool database that has the max depth set to the depth you want the pass to. However, I don't know if that would always work depending on material thickness and number of passes configured or calculated.

If your machine is supported, I do recommend giving Vcarve or Vcarve Pro a test run.

No apology needed. I found the information you and Jim provided valuable.

A Vcarve test drive is on my to do list. Just need to get thru this month and then I should have some spare time to do that.

[Steven O Smith]

Whiteside's drawing of the UD2101 compression bit (for example) shows that the upcut portion ends <1/4" from the tip. I can see there being some uncertainty in where the line is between upcut and downcut. How do you figure out the minimum depth of cut for the compression benefit?

One answer (given by Holbren sales) is to go deeper into the spoilboard, which would mean cutting more than 1/4" deep with a 1/4" diameter bit. This all seems very vague. If I had bits, I could cut some wood and figure it out, but that doesn't help buying a bit.

[Michael Burnside]

Whiteside's drawing of the UD2101 compression bit (for example) shows that the upcut portion ends <1/4" from the tip. I can see there being some uncertainty in where the line is between upcut and downcut. How do you figure out the minimum depth of cut for the compression benefit?

One answer (given by Holbren sales) is to go deeper into the spoilboard, which would mean cutting more than 1/4" deep with a 1/4" diameter bit. This all seems very vague. If I had bits, I could cut some wood and figure it out, but that doesn't help buying a bit.

Not sure I agree with the "deeper into the spoilboard" comment, makes no sense for a compression bit. I use the Bits and Bits version which has a shorter change depth so I just plunge to 1/4". If the UD2101 is close to 1/4", I would setup a test. First I would do 1/4" - 0.005", then 1/4", then 1/4" + 0.005", then 1/4" + 0.010" and maybe a final 0.015". Just be sure NOT to ramp a compression bit. You need to pluge immediately down to the cut depth. From there, I'd chose based on the quality of cut for the top. The bottom cut is irrelevant as the upcut will yield a nice finish. I always zero to the spoilboard for 99% of the jobs I do and I never go more than 0.003" into the board ever.