Need Advice - 90 Degree Chamfer on Baltic Birch Plywood

[widgetworks_unlimited]

Looking for some sage wisdom from cyberspace - this one's got me stumped...

I'm trying to use a 90 degree V bit to "knock the edge off" / chamfer the outside profile of parts that I'm cutting in Baltic birch plywood. Depth of cut is only 1/16th from the top of the part - basically just edging the top veneer to give the part a finished look, while avoiding hand sanding.

I've used the same operation on 1,000s of parts cut in UV clear coated maple ply - works great. The birch ply is giving me tear out when cutting across the grain.

I've slowed the feed down to 4 ips (going any slower than that doesn't seem to help) and switched to a brand new bit. Results still aren't what I'd like to see.

Anyone have any experience with this type of thing?

Anyone know of a downcut 90 degree V bit? Any other type of 90 degree V bit that may do better - I'm using a cheap 2-flute straight 1/2" shank, .250 DOC right now.

[knight_toolworks]

baltic is bad about that. you can try a limb cut and see if that helps also crank the rpms up to max. the centurian v bits seem to tear a bit less. but also you may try using the v first before cutting out the parts.

[dlcw]

Steve is right on the baltic birch. The maple isn't chipping because of the clear coat. The coating is holding things in place.

One way around this is to try two passes. Make the first pass almost all the way in a climb cut. Then follow that up with a very light conventional cut. This might ease the chipping considerably. Also, like Steve said, Centurian has some good 90 degree bits that do a very good job.

[widgetworks_unlimited]

A little more info on what I've tried so far...

I've tried both climb cutting and conventional cutting - climb cutting makes the tear out problem much worse, which really surprised me... oh well.

RPMs are around 19000. I may try to go higher, but I haven't seen much improvement from dropping my feed rate below 4 ips, so I'm guessing that uping the RPMs will have a similar non effect.

I'm running the V chamfer before cutting the profile with a downcut end mill. This does help considerably when the cut is parallel to the grain in the veneer, compared to chamfering after the end mill cut. But, the cross-grain cuts are still a problem.

I'll give Don's roughing/finishing cut suggestion a whirl. I do this with all my other cuts, but it seemed like overkill on a chamfer that's only .065 deep.

...will also call Centurion on Monday if no one can recommend a downcut V bit.

[Brady Watson]

You may want to try slowing things down to 1 IPS for the chamfer and crank the RPM up to 20-22k. Even though you are only going .0625" deep, you are still asking a v-shape tool to move a lot of material at the point. V tools basically drag material at the point since there are no flutes to really carry it away. Close observation while cutting will illustrate this point.

For a job like this, I prefer to use a 90 degree 0.5" diameter mill/drill. It's solid carbide, is EXACTLY 90 degrees and lasts a very long time.

-B

[widgetworks_unlimited]

@ Brady - Don't know why I never thought about a V bit that way, but it makes sense that the tip of these bits would have problems with flex and chatter along with the "dragging" effect you mentioned. The tips are ~.030 thick with no support. Even the thicker sections are only about .075

I wouldn't run a 1/16 mill at 4 ips though this material... I'm surprised I haven't broken the tip off.

The Centurion V-bit and drill mill both seem to have a lot more beef at the tips. Not sure if that will be enough to keep my feeds up - 1 ips is grueling to watch.

I may go back to chamfering the edge after I do my roughing profile. That way I can offset the bit away from the vector + lower the cutter while removing the same amount of material from the part - then tip is just cutting air and the actual cut is in the thicker part of the bit.

I went away from this method because I was getting some tear out from my roughing profile cut - even with a 3/8 down cut bit. But, after running some more parts, I think that problem will go away when new/sharp cutters arrive this week.

[jerry_stanek]

Can you run an offset and lowering the bit so it is cutting more towards the center.

[Brady Watson]

Can you run an offset and lowering the bit so it is cutting more towards the center.

Very good point, Jerry. I remember needing to do this on a few jobs in the past in hard maple to get the right finish.

-B