Spiral 2 flute vs. O flute bits

This forum is for users to post tips and tricks they have found useful while working with VCarve Pro

Spiral 2 flute vs. O flute bits

Postby CharliesWoodStuff » Mon May 27, 2019 12:44 pm

I’ve been using up and down cut spiral end mills.

The down cut bits pack chips into my profile cut. A pita to clean out and I know that can’t be good for the bit.

The uncut bits frequently leave rough bottoms and usually fuzzy at the perimeter.

I’ve been doing a little reading about O flute bits. Can anyone dumb it down for me?

Will O flutes help with deep profile cuts?

Will they help give me smooth pocket cuts while efficiently removing chips?
CharliesWoodStuff
 
Posts: 16
Joined: Thu Apr 04, 2019 12:17 am
Model of CNC Machine: HD4

Re: Spiral 2 flute vs. O flute bits

Postby ger21 » Mon May 27, 2019 1:02 pm

What size bits, and what are you cutting?
Gerry - http://www.thecncwoodworker.com
ger21
Vectric Wizard
 
Posts: 1471
Joined: Sun Sep 16, 2007 2:59 pm
Location: Shelby Township, MI, USA
Model of CNC Machine: Custom DIY

Re: Spiral 2 flute vs. O flute bits

Postby CharliesWoodStuff » Mon May 27, 2019 1:07 pm

I’m mostly cutting signs out of Lowe’s pine boards. Some recycled pallet oak.

My end mills are a cluster of 2mm down cut, .125” up & down & compression, and .25” up & down cut. Depending on the size of the cut...
CharliesWoodStuff
 
Posts: 16
Joined: Thu Apr 04, 2019 12:17 am
Model of CNC Machine: HD4

Re: Spiral 2 flute vs. O flute bits

Postby TReischl » Mon May 27, 2019 1:41 pm

It is difficult to get good results in pine. Some of what I do is NOT optimum but it helps and unfortunately also slows down the process.

If I am doing lettering on a sign I will pocket down to the face of the letters +.005-.010. Then I will put in a 1.5mm/2.0mm bit to profile around them to depth using a spiral strategy. The small bits do not chip things out like a larger bit will and leave very little fizz around the edges. The added benefit is that the letters are much crisper than profiling with a larger bit.

Next I pocket out around the letters leaving .005/010 on the bottom and the walls of the pocket with a larger bit, usually a 6mm. IMHO using finish cuts is key to getting good results in pine. Note: I usually offset the profiles of the letters by a few thousandths just to keep the larger bit from touching the edges of the letter that have been cut.

To finish up I will make a pocket cut to remove that .005/.010 that was left on the face of the letters, always cutting with the grain, no offset strategy.

Yup, it takes more time than just tossing in a bit and telling it to just pocket out the letters all in one go. But then when it is done I do not have chipped out edges and lots of fuzzies all over the place. One of the problems I have is that 1.5mm and 2.0 mm bits will only cut .375 deep maximum. But usually that is good enough for most lettering tasks.

I work a lot with big box store pine. Most of what I am doing lately is painted. There is a lot of what I will call "cathedral" face lumber in those piles of boards. Almost all of it. So the other thing I do is rip the boards to the thickness I need, then turn them 90 degrees so that "cathedral" face becomes the glue face. That way there is much tighter grain on the surface of the blank. Yup, another step that takes time. The other benefit to doing this is that you end up with blank that does not cup as badly. Also, I always use a blank that is about .125 -.250 thicker than the final thickness. I leave fairly thick tabs, about .187. When I am done cutting the sign I flip the whole thing over if it is a bit warped and take a skim pass on the back side.

Ah, yes, one other thing I do to avoid problems is cut a slot along the ends of the blanks for the clamps. That way I can surface both sides without having clamps or screws in the way.

Well, that is how I cut big box pine these days.

Oops, one other thing. If I am doing something large that will raise a lot of nasty fuzzies when painting I will leave it on the machine and put a coat of thinned out water based Kilz on it. Talk about raise the grain! Then rerun the profiling programs to remove the huge fuzzies that appear. Seems to work pretty well, but is downright slow.

Edit: I use HSS bits whenever possible, they are sharper and cut pine better than carbide.
"If you see a good fight, get in it." Dr. Vernon Jones
User avatar
TReischl
Vectric Wizard
 
Posts: 2775
Joined: Thu Jan 18, 2007 6:04 pm
Location: Leland NC
Model of CNC Machine: 8020 Build 48X36X10 RP 2010 Screenset

Re: Spiral 2 flute vs. O flute bits

Postby CharliesWoodStuff » Mon May 27, 2019 1:59 pm

Wow - great info! Thanks
CharliesWoodStuff
 
Posts: 16
Joined: Thu Apr 04, 2019 12:17 am
Model of CNC Machine: HD4

Re: Spiral 2 flute vs. O flute bits

Postby ger21 » Mon May 27, 2019 2:15 pm

To answer the original question regarding "O" flute bits.

O flutes are typically used for plastics and aluminum. They still come in both upcut and downcut, and will have the same issues standard spirals do with regards to fuzzy edges.

Deep cuts with small bits are always going to pack the chips in the kerf. One thing you can do is make a rough cut of .02--.03" first, which will allow more room for the chips when you make the final cuts.

An alternative to O flutes might be single flute spirals. These will clear the chips better as well.

But you'll always have a very difficult time clearing chips with downcuts.
Gerry - http://www.thecncwoodworker.com
ger21
Vectric Wizard
 
Posts: 1471
Joined: Sun Sep 16, 2007 2:59 pm
Location: Shelby Township, MI, USA
Model of CNC Machine: Custom DIY


Return to VCarve - Tips and Tricks

Who is online

Users browsing this forum: No registered users and 5 guests