Cutting BB

[Dan Richeson]

Hello

I just got my new CNC going here last week and this weekend I wanted to cut some hold downs out of some scrap BB 3/4" I had. I used the whiteside 1/4 Down cut bit but the tear out was terrible. I tried having a very light first pass of .025 but that didn't really seem to make a difference. I used the default setting of 160 IMP from the tool bit down load from whiteside. I even tried the two different feed directions and they both seemed about the same to me. Any advise would be great. Thanks.

[John TenEyck]

Are you sure you used a down cut bit? Sounds more like you used an upcut bit, or a compression bit and didn't get past the upcut portion. A genuine down cut bit will give a clean top surface if you use the recommended speeds and feeds for plywood.

John

[Mick Simon]

Yep, sounds like you were using an upcut spiral. If you hold the bit with the shank up, is the cutting edge sharp on the bottom side or the top. Downcut bits should be sharp only on the bottom edge.

[David Falkner]

I cut 1/2" (or 12mm) BB in one pass at 175 ipm with a 1/4" compression bit. No tear out on either side.

Go to about 8:15 in this video I just posted and you'll see what that looks like -

[Steven O Smith]

I needed both sides of the bb clean, so I used a straight edged bit (like a conventional router bit). There were a few fuzzies to take off, looks good now that they are removed.

[John TenEyck]

I needed both sides of the bb clean, so I used a straight edged bit (like a conventional router bit). There were a few fuzzies to take off, looks good now that they are removed.

Try a compression bit. It will cut much smoother than a straight bit and both surfaces will be clean.

John

[Jim Becker]

A down cut should leave a pristine surface on the top.

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.

[Dan Richeson]

Thanks for the reply. I will double check which bit I grabbed out of the kit I bought from Avid. I thought I had the RD one. Will let you know what I found.

[Michael Burnside]

Yea, as others mentioned, sounds like you maybe grabbed an upcut. Well, I guess it could have been a poorly sharpened downcut too

Also, for BB or similar material that is a through cut, I'd use a compression bit. However, like Jim said, make sure the first pass depth of cut is BEYOND the transition of the bit or you'll defeat the purpose. In your tool configuration set the max depth to just larger than that number and then in Vectric just double check the first pass is at least that much.

You mention 160 IMP but that's meaningless unless you state your RPM too (I assume 1/4" bit). I usually shoot for a chipload of 0.009-0.010 with BB, which for my machine is around 240 IPM at 13500-14000 or so with 1/4" tooling. If you're spinning at 18k and 160 IPM that is WAY too low of a chipload and you're going to break bits by heating them up IMHO.

EDIT: one last point is that with typical up/down endmills, especially downcut, it is a good idea to have a ramping cut, however with a compression bit, you need to immediately plunge to the DOC length or, again, you'll get top material tearout.

[Dan Richeson]

Hello, Yep you all were correct. I had the RU bit and not the RD bit. The eyes are getting old and Whiteside don't mark then very well. I do have a UD2102 bit that was included in the set I bought. So how does one know what the transition of the bit? I wonder if Whiteside lists that on their web site? SO much to learn with this CNC. I think I watch to many Y tube videos and mad it look so simple. Thanks again.

[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!

[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"

[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)