Adding a rounded edge

[philspitler]

I want to add a rounded edge to some of my pieces and am wondering what bit would give me flexibility.

I was told that a "round over bit with a point" would be good but I would love to know more details.

Any thoughts?

I'll be cutting 1/2" plywood but will only want a small rounded bevel.

Cheers.

Phil

[adrianm]

If you're doing it on the CNC rather than a router table then it has to be a point roundover bit or a plunge roundover bit. Using anything with a bearing on it can be extremely dangerous.

The following are examples of the two types not recommendations:

http://www.toolstoday.com/p-6208-beadboard-router-bits.aspx
http://www.carbideprocessors.com/router-bits/grooving-router-bits/plunge-roundover-router-bits/

Personally I find it far easier and faster to round over on the router table afterwards but I know many disagree.

[barrowj]

I agree that you need the pointed roundover and you might want to draw a separate line for offset a very minor bit (like .02) or something so the point doesn't end up drawing a line. As for doing it with the CNC, I would do it if you are doing multiple pieces but not if it is just one piece. Again, that also depends on many factors and is an individual choice. You would want to do the roundover first, then the profile, this should clean up any marks left by the pointed end. When I do this on hardwood glue ups, I like to use several passes to get the smoothest cut.

[dlcw]

Phil,

I do roundover on the CNC all the time. Like the others have said you need a plunge/point roundover bit. Many suppliers have these bits, just Google them.

As far as the toolpathing, I tend to let the roundover just do its thing, no offsets or anything like that. When I do the cutout path, I set an offset of around -.008 to -.01 depending on how the roundover actually cuts (test it first). This negative offset on the cutout removes any little ridges created by the roundover.

Additionally, always ramp these bits in, don't plunge them. Make more then one pass with the final pass being about .0156" (can be controlled through the software). This leaves a smooth cut (if the bit is sharp).

[scottp55]

Just my 2 cents.
I like to put my offset allowance(prefer to keep the drawings cleaner and avoid grabbing the wrong line by mistake, which I sometimes do if actually making a tiny offset vector) in the Pointed roundover toolpath so that my finished product dimensions never change.
Also found that a spiral ramp seems to cut very slightly cleaner as the cutting force is more constant than a straight ramp. I'm lazy and hate sanding so I make my my final pass .001" so basically an extra pass to eliminate any fuzzies and tool deflection(almost burnishes it but bit still stays cool).
These bits seem to vary slightly from nominal Form Tool I drew, so first thing I do is determine how far down I can actually cut without the outer cutter getting into the act and leaving a "shelf"(although sometimes that is a nice decorative feature for "free").

[philspitler]

These are all excellent tips.

Thanks.

Phil

[philspitler]

I ordered these bits from Amazon.

http://www.amazon.com/gp/product/B000RA8ST8/ref=ox_ya_os_product

http://www.amazon.com/gp/product/B00063FYNY/ref=ox_ya_os_product


For feed and speed I'm guessing as usual it's trial and error but would love any advice.

Thanks again for all the help.