Printable View
This is the result I get using a new 1/4" upspiral carbide endmill at 10k RPM at 200 IPM. BTW, it's cheap boxstore MDF.
Is this excessive, I don't know what it's called, fuzzing, normal?
I did not see this using a straight bit but I ran it at high RPM and low feed rate. (newbie)
That looks more-or-less normal for an up-cut spiral in MDF. You may be able to get slightly better results by adjusting the speeds & feeds, but it will never give you a perfect crisp edge.
I usually "break" the surface with a 1/8" or 1/4" down-cut spiral, to a depth of about 1/10". I then do the full depth cuts with a larger diameter up-cut spiral. (The concept is similar to using a scoring saw on a panel saw to prevent chips along the edge.) I do this in any material where tearout is likely to be an issue.
Cheers,
- Dean
As Dean said, it's normal. If it sands off easily, it's not excessive.
Looking at Onsrud's chip load chart, I think you need to up the rpm's a bit for 200 ipm. Depending on depth of cut, from 13,000 to 15,000. This should give you slightly smaller chips, which won't tear out quite as much.
http://www.onsrud.com/xdoc/ChipMDF
The 52-200 is an upcut spiral.
Another thing is on the inside stepped are (rabbitts), cut the deeper parts first, then you'll only have the fuzzing on the very top edge. You can also try a very light first pass, maybe .01.
I tend to use downcut spirals for most cutting, though. Very clean top edges. But, you'll want to keep the chips from packing in the cut, as it will create more heat on subsequent passes, which dulls the tool faster. But, another advantage to downcuts with mdf is even when they start to dull, they'll still leave a clean top edge.
I use Dean's method when cutting hardwoods, especially thick ones. Make one pass with the downcut to prevent the edge from chipping, then switch to an upcut to finish.
A couple areas where upcut bits are much better, is peck drilling, and pocketing or surfacing.
A downcut will burn badly if you try to plunge straight down for a hole.
And if cutting a flat bottom surface, an upcut will give much better surface finish.
I use a compression (or mortise compression) bit for cutting sheet goods. This bit has both an upcut spiral and downcut spiral in the same bit. With a mortise compression you would plunge about .25" into the material and start cutting. This puts that downcut part of the bit into the material creating a very clean and crisp cut. When you are ready to punch all the way through the material, do so by about 1/64"-1/32" and the upcut part of the bit creates the same clean and crisp cut on the bottom. These bits are available in many sizes and diameters.
This type of bit works great for plywood, melamine, laminate, MDF, etc.
thanks guys, y'all gave me some really good advice to try out.