3/4 plywood snapping bits?

[Nils N]

I just read the other thread on snapping bit and I'm going to pass that on but the problem is this. I stopped at a friends shop, they have a 5X10 panel router and use MC V9 for programing. He's cutting some 3/4 plywood with 1/4" bit and keeps snapping them. The panel is 4'x8' and he has 72 pieces on the panel to cut out. He's snapped them running these configurations-

 

1/4" 2 flute upcut spiral

A@ 100IPM

.33 Step down

.06 final cut

 

1/4" 2 flute carbide straight

A@ 80IPM

.33 Step down

.06 final cut

 

1/4" 2 flute upcut spiral

A@ 50IPM

.2 Step down

.06 final cut

 

Any ideas on why he'd be sanpping bits?

[Todd Tracey from Fastech]

What is the Spindle Speed (RPM)?

[Nils N]

oops forgot that, 17,400 on all of them

[Namliek_J@TheeCircle™]

Any coating on the bits? How long do they run before they snap?

[Nils N]

No coatings on the bits, and they're snapping at different times, beginning of cut middle of cut, I told him about checking the collects for dust and stuff, like the other thread. I'd think he should be able to run really fast more than 100IPM with 17,400 rpm He's had to slow it down and take more pass to make it work. just seems like he should be able to go faster then he is and less down steps than 3or 4 in 3/4 ply

[Matthew Hajicek - Singularity]

Are the upcut spirals carbide or steel? I know wood can be pretty abrasive. My guess is that either the tool is getting dull, or it's loading up with chips. Setting up an air blower might help. Does the tool get really hot?

[Namliek_J@TheeCircle™]

The tool is only .250, so you are not going to be able to run it to hard. I would maybe see about getting a 4 fluted tool? The two flute has a smaller core thickness than the 4 flute.

[Nils N]

All new Tools all carbide. He ended up finishing with a carbide coated three flute bit, 50IPM, ,2 step down with a .06 finish pass at 17400 rpms. He'll try the 4 flute for the next batch.

[Thermoform Guy]

We cut 3/4 ply everyday, but normally with a larger tool. However with a 1/4 non coated we

can run 150-200IPM at 18000 rpms taking a full

radial and axial cut.

[Tom Dorgan from American Precision]

I run Onsrud 63-725 O flute and a straight flute I don't remember the number of at 200-300ipm in 3/4" yellow pine plywood all the time. I would try a brand new collet. If the first tool broke left a burr on the id of the collet, every carbide tool you put in it will break.

[Mike Gates from Barefoot CNC]

He really ought to look at using 3/8" schrupp roughers for the roughing cut. They have a serrated edge that seems to do better in plywood applications. Then do a finish pass with a 1/4 smooth edge cutter.

 

We used these roughers for cutting 7/8" in one pass doing upholstery frames with a Shoda. Another thing is to use as small a cutting edge as possible and put as much up in the collet as you can to help with the tool deflection.

 

Take a look in the link below at the 60-900 | Three Edge Solid Carbide EXHD Hogger.

 

Onsrud Router Bits

[Westgate Hardwoods]

I think Mike is on the right track here. Using a larger bit and speeding up the feed rate would probably work better. Are you using the 1/4" bit because you want to optimize the material better or is there a limitation in the Router? We cut 3/4 plywood all the time with 3/8 and 1/2 compression (up/down shear) cutters at 600ipm/18,000rpm full cut with one pass.

[Nils N]

Yep he was using a 1/4 bit to optimize space, I think he needs to take some of these suggestions on he's next project I'll pass this along. Thanks everyone all the good advise