Hi

I am having to kerf a significant amount of kerfs in 3/4" plywood on the CNC. Total kerf depth is 5/8" It needs to be a 1/4" diameter kerf for which I am currently running a 1/4" 2 flute compression bit (Whiteside) +/- 3/8" DOC 18000RPM and around 280 ipm. 2 passes total per kerf. I have broken a few bits and so am reluctant to go faster. I would ideally like to make these kerfs with one pass. I have been looking for a 1/2" shank 1/4" cutting diameter compression but haven't found anything. Any suggestions on a source for that size bit or feed/speed suggestions that would allow for a single 5/8" doc pass with a 1/4" shank/diameter bit? Running a standard 3axis flat bed 4x8 so no 4th axis to mount anything.

Thanks

You are asking to defy physics. 1/4" bit will take forever. A Sliding saw with a custom blade and an NC controlled fence or stop would be significantly faster.

If you are making a lot. I would think about a C axis with an aggregate saw and custom blade.

Good luck!

Bill

Unfortunately the kerfing is just one component of the toolpath of which other things need to be done on the CNC and so CNC is the only option. Yes it takes a while per sheet (on average 30 minutes just for kerfing on average per sheet). Long term perspective if this client continues and grows, then I will be looking at faster/more efficient options, but that is tomorrows problem. I assume that I can have custom bits made but was hoping just to find something off the shelf.
Thanks

I have never seen the bit you are describing. I don't think it would help though. We tried something similar to what you are doing and experienced similar results.

If it were me, I would call Vortex or someone like them and ask. Couldn't hurt.

Bill

Thanks. I do forget about Vortex sometimes. They don't have what I am describing, but they have a lot of options, so I may be able to find something that works.

Thanks

5/8 with a 1/4 bit is only 2-1/2 times diameter. You should be able to manage this with controlling your chip-load just a bit. I think that the key to reducing breakage is to grip the shank very close to the flutes. Counterintuitively a 2 flute tool is much stronger than a 1 flute, as there is a lot more metal left. Also use a standard compression, not a mortise compression, to evacuate more chip. I see Vortex has a 2 flute standard compression with a 7/8 depth of cut, a 3110.
An aggregate with a saw would really be best, but I see your point for low volume to begin with.

You could try a 2 flute down cutter with a smaller cut length. tools with a larger dimeter shank and smaller bit have a weak spot where the are turned down in size.

By "kerf" do you mean you are cutting 1/4" wide slots in the panels? If so then why are you using a compression bit? The purpose of a compression bit is to give an upcut spiral cut to the bottom of the panel when cutting all the way through while doing a downcut on the top of the panel. As just suggested a downcut spiral will do the job with a stronger bit.

Also, it's a little bizarre, but you might have decent results with a coated HSS bit instead of carbide. It will be stronger so you can do faster speeds. It won't last near as long as a solid carbide but is much less brittle. Or it might be worth trying a carbide tipped single flue 1/4" bit on a 1/2" shank if you can find such a thing.

BH Davis

this endmill will do what you need , we use it on daily basis cutting 3/4"ply . i say you will be able to do it in 1 pass very easy if you cnc router & vac pump that has the stiffness that is needed to keep bit from vibrating. try 14600rpm @ 250-400 ipm.
if it wants to chatter slow feed till it smooths out.
the slower spindle speed seems best for us. good luck

https://www.amazon.com/gp/product/B09H33X98L/ref=ppx_yo_dt_b_search_asin_t
itle?ie=UTF8&th=1

Definitely do not want to use a 1/2" shank with a 1/4" CD. That tool is actually weaker or more prone to break than the 1/4" shank. Because you have a stress point where it makes the transition from 1/4" to 1/2" diameter. This is why we do not make this bit. Play around with Feed and Speed. Also, what grade of plywood is this? Also, check collets, if you have not replace them lately, get a new one. Anytime you have a breakage problem, always check
everything especially collets.

Mark
Good advice. Will try that. Thank you.
Jim. Good to know about the larger shank tools. Would not have guessed.
BH. You are right, except that after all of these kerfs have been cut, I spend maybe 10 minutes per sheet clearing all of the packed chips out of the kerfs and the compression is slightly better at leaving less chips than a downspiral. I have been wanting to avoid tearout but maybe an upspiral is the answer. The face with the kerfs is completely non-visible for the finished product.
Mike. Thanks for the tool recommendation. Will give it a shot.
Chuck. Thanks for the info about the tapered bits. It is combicore (mdf skinned plywood). It could be the collets. I will explore that. I am using vacuum holddown and generally feel that it is performing as needed, but with kerfing there may be some vibration that is beyond my control.
Thanks again for all of the advice.

See if you can get a chipbreaker compression spiral. Much better for cutting ply. If the top edge doesn't matter use a slow helix upcut, chipbreaker or roughing profile if you can get it. If you are going to go custom ask for a 3/4 flute length.

Agree with not using the mortise compression, packs too much crap into the bottom of the slot.

What software are you using? We use AlphaCAM and do bi-directional cuts which sort of zig zags down and is much faster. I would start at 3 passes and 250 IPM and increase until you break a tool, then drop 25 IPM.

Can you place an air jet into the slot to help blow out the chips?

Add compressed air nozzle to the machine that will blow out the swarf.

We use a 1/4" straight carbide bit from Dimar with a dust extraction collet to cut all of our 17mm(11/16") hpl sheets. We run it at 18,000rpm and 20m/m(700ipm) and leave 1mm for the second pass because many of our pieces are 2-1/2" x 96" and we don't want them to move. We've nest 19mm melamine at 20m/m in a single pass without issues.

Bits are $40CAD dust extraction collet is $90. We've been using them for the last 3 months love them.

View higher quality, full size image (700 X 700)

View higher quality, full size image (700 X 700)

1/4" straight bit