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.

[Michael Burnside]

Dan,

You’re right, I don’t see that info mentioned. You can email them and/or measure it. Use the term "spiral change depth". Just measure where the bit transitions to upcut and you can use that in your depth of cut in the Vectric tool config and maybe add 0.005" or so. It’s probably less than 0.25” (likely 0.22"). I noticed their recommended RPM is 18000-24000 LOL good grief. It’s not wonder hobby CNC people get so confused on feeds/speeds and chip load.

CNC is super fun and after you get your feet wet with a few jobs and “trials” you’ll be fine.

[Mick Simon]

Not trying to hijack this, but curious if anyone else is running into this. The last 3 Whiteside ¼" compressions I've ordered for class have left a small ridge right where it transitions from up to down cut.

[Michael Burnside]

Not trying to hijack this, but curious if anyone else is running into this. The last 3 Whiteside ¼" compressions I've ordered for class have left a small ridge right where it transitions from up to down cut.

Could be related/relevant to this thread. I’ve not used this exact bit (I prefer Bits and Bits version), but check your tool configuration has max depth to slightly more than spiral change depth. Then, when you create tool path, edit passes and make sure the “Maintain exact tool path depth” check box is selected or the first pass is at least the max depth.

[Mick Simon]

Thanks Michael. I've done that. It's a problem with the up and down portions of the flutes not overlapping the way they should. I've brought it to the attention of the Whiteside folks. I have not had the issue with their ⅜", only the ¼" compression.

[Jim Becker]

Whiteside's .25" compression bit switches over at about 3/16" which is why I made the recommendation for the first pass to be at no less than .25"/6mm.