Machining 2D/3D Fillets

[george]

I've got a model with a fillet on the edge and I'm having trouble selecting the right tool paths and operations. I'm using a flat end mill and I know a ball nose would be better but I just wanted to try the operation and see how it turns out.

I've tried different 2D and 3D operations but none of them allow to select the profile of the curved edge.

Perhaps someone has some helpful advice. Here's a link to the project, http://a360.co/23ZRn9x

Thanks,

George

[jeff.walters]

From what I'm seeing you are trying to cut a radius with a flat mill. This wouldn’t be a simple one pass type of tool path. But I would recommend using a 3D parallel operation for it.

[kb9ydn]

I do fillets like this a lot because I don't want to have to do another setup.  It isn't machine time efficient but it does work.  It does work better with a rounded tool but if you don't care about the finish a flat tool will do it.  The trick is to use the parallel operation and select the fillet face as a touch surface.  You'll have to set the stepover fairly small to get a decent finish; try 0.005 inches for example.  Also you need to set the angle so that the passes are perpendicular to the original unfilleted edge.

C|

[george]

Would you mind taking a look at this setup and see if you think it's "good" enough? The slot that this board is going into will be cut with a 1/4" bit so the fillet is 1/4".

Thanks,

George

[Steinwerks]

A .0965 stepover is huge. I'd bring that down to .004-.006 and see what it looks like in simulation, especially with a little cutter. Are you running your path in Z arcs or Z steps? Change your Pass Direction to make sure you're interpolating in Z, it'll be nicer with a square end mill otherwise you'll get little tiny steps all the way up your radius (think staircase).

If you can share the part or some screenshots of the toolpath and other tabs that'd be best.

Edit: noticed you DID share the part! I should read more carefully before responding 

[george]

I guess that explains why they didn't turn out too well. Here's a link to the part, take a look and let me know where I've gone wrong.

Thanks,

George

[Steinwerks]

Well some of your geometry selection was a bit funky, as well as the passes. Considering the sharp corner of your feature a 3D toolpath is not going to do it completely. I would suggest using a Pencil operation with the smallest tool you can find to get in there and clean it out if you don't want to do it by hand. I've attached a revision that works "okay" but better than the original.

[kb9ydn]

This is one of those parts where it really would be better to flip it up on end and cut the fillets from the end. That's the only way you will keep that flat edge at the corners.

Or if you don't care about the flat edge you could use a roundover bit for just the length of the fillet.  If you want to cut the entire part from the same orientation that would be the way to go.

C|

[george]

I wasn't looking for perfection on this operation just saving some hand filing or having to setup the table router just for a 10 second cut. Your operation is obviously much better than what I did but I can't seem to find out how you were able to select that square under the fillet to choose the machining boundry. I had played around with all sorts of selections and what I ended up with was the only way to get close to what I wanted.

If you could tell me how you did that or make a quick screencast that would be great!

Thanks again,

George

[Steinwerks]

I agree with kb9ydn, for what it's worth.

I will try and do a screencast after work, no time right now.

[george]

I don't have the Z height for all the shelves I'm making so I was just looking for something to help eliminate the hand filing. Right now my CNC is mounted on top of my router table so doing this "properly" on the router is kind of a pain right now

[george]

Well if at first you don't succeed, try, try again. I guess when I was trying to select the fillet area I never selected one of the 2 sides that would create the square boundry. Not sure even if I had I would of thought to use that and select the outside edge as the bottom height.

I assume that you changed the direction to 90 degrees because machinging in this direction would give a better finish?

I made a screencast of how to do it, http://autode.sk/1PRctgP