Profile Cut Hardwood: Tips/Tricks?

[RossMosh]

I have a project to cut 60 crosses out of hardwood. This is a little out of my comfort zone. I normally machine plastics for signs primarily but I figured why not take a shot at it.

I tried cutting the design out of 3 hardwoods: poplar, cherry, and hard maple. I used the same feed/speed for all three of 120ipm and 16000 rpm. DOC: .25" and climb direction. I'll admit, the 1/4" upcut bit I used has been around the block so I ordered a 1/4" Whiteside downcut which should come in tomorrow.

My issue is the edge quality I'm getting needs sanding. A good bit of sanding. The straight sections need minimal sanding but around the curves and contours, it needs quite a bit of sanding. It either shows the machining lines or has minor tear. There isn't a huge difference in quality of cut between the three woods. Hard maple machined the best with Cherry and Polar essentially tied for 2nd.

When I get the new bit tomorrow I plan on doing the following: Oversize the part cutting in the climb direction. Then do a cleanup pass, full depth conventional pass.

Any other recommendations?

[Tim Lucas]

Sounds like you have the correct plan of oversize then clean up, you may want to do conv first as the climb will give the best cut

[Xray]

Fresh bit may do wonders, might also want to tinker with feed speeds and pass depth.
I presume you are taking .125 bites, I'd slow it down to 75 ipm or so. Router RPM could also be a small factor, so you might be looking at a combo of things, but sharp bit is center stage.

[scottp55]

Ross,
Do you have the "Last Pass" option?
If so, I'd try a .005" and use a spiral ramp taking .125" passes.
That bit likes a conventional toolpath and I'd do both as conventional cuts.
I've got that bit in my laptop database for Hard Maple as 1.5,.5,12.5K
I think in my control computer database, the RPM is slightly lower and you'll have to play with it to keep it cool.
Careful with last pass if not using tab's, I've had it skew a piece on carpet tape, so don't know what it might do with vac.
scott

[steve_g]

Ross…
I just finished a run of Cherry business card holders, I used a compression bit with a climb spiral .01” oversize for the first pass and a full depth last pass conventional cut. I’m very pleased with the cuts!
I typically don’t use the Vectric “last pass” option as I like to also leave an onion skin on the bottom to cut with my last pass.

SG

[scottp55]

Off topic;
Steve, What did you finally wind up with for sanding the pocket in Biz card holders?
Yep, about 3/4's of the time I cut like you recommend

[steve_g]

Scott…
It took a combination of things to get the interior finish I wanted… Using a FEM, or bottom cutting bit helped reduce the need for sanding as did offset cutting, it has less tearout than raster.

In the end, a Milwaukee multi tool with a customized sanding head Got me the end result I was looking for.

SG

[scottp55]

Thanks Steve,
Pretty much what I found after Scott W recommended FEM
, and now I've got the Fein multi, I can adapt a head.
Appreciate it!
scott

[Cosmos275]

What I do is run a chamfer bit along the profile first. I run it outside with a negative offset, so I'm adding a small chamfer to the finished edge. Then, when the end mill goes by, there is no tearing and the edge looks good when it's done.