A tooling dilemma

[bcammack]

We cut some very dense, 3cm thick solid surface material. We use a 5HP Colombo spindle and a 1/2" carbide bit to cut out a sink hole and faucet holes in the material.

I changed from a straight plunge and single pass to a spiral plunge out of deference to the spindle and the $400-a-pop bearings within it.

Of course, now we find that this method is effective, but it only used the 25% of the CEL of the bit nearest the tip and, naturally, wears the used portion out 4 times as fast.

We could do 80-100 cutouts with a bit and now we only get 20-25 sinks. That's about four bits per shift.

I don't know if there's any solution to this. I simply felt like sharing.

[harryball]

All I can say is factor the cost of new bearings per expected life vs. the cost of using 4 times as many bits and let the math guide you.

Or... I suppose you could peck drill or zig-zag to depth going slowly and then make a single pass once at depth. This should decrease the stress on the bearings and increase the cutter life by using the full CEL.

Robert

[billp]

Brett,
You don't mention the tool geometry (straight,upcut , downcut, etc.) in your message, but have you considered some of the replaceable tipped tooling like "Her-Saf" ? It would seem to minimize the cost of keeping a sharp cutter on your tool.
In general I've also found it's a better technique to use the shortest bit for the job as it not only eliminates the wasted/unused portion you mention, but it also minimizes vibration, and deflection...

[innovative_cabinetry]

Brett

What brand are you cutting? I have been using Affinity but have considered adding EOS also. I mainly do cabinets but supply SS tops when the customers don't want stone. I would imagine the dust is very hard on the bearings.

[bcammack]

We import the product ourselves. 35% acrylic-modified polyester and 65% alumina trihydrate powder. Dense and hard stuff.

The 'bot has a custom-made telescoping dust collection shroud that keeps most of the debris in the collection system, not in the air. (amazing what a fellow can do with PVC pipe, setscrews, and some small springs...)

We use 1/2" carbide bits. Single-flute straight, two-flute up-spiral, and a compression spiral. Varying results, but generally acceptable.

Currently cutting at 30 IPM and around 7k RPM. Anything north of 8K and we burn up the cutting edge on the tool. Much under 7K RPM and the tool chatters.

Never a dull moment 'round here. I'm presently toying with the idea of boring a hole through the center of the table and putting a T-nut underneath. Then I'll have the program go to the centerpoint and plunge cut through the material before backing off to the side so the operater can run a bolt through the piece to lock it down.

[innovative_cabinetry]

Do you do your seaming on the bot when you get wide tops like you get on Islands? I have been curious as to whether the bot would be able to run smooth enough to get a perfect seam with the 3 cm material. Are you doing edge profiles on there or is that done with hand routers?

[bcammack]

The material is strictly for bathroom vanities tops. It comes out of the containers 22.5" wide and 10' long. They come off the pallet and are given a demi-bullnose on one long edge with a specialized machine.

Pieces do get seamed for "L" shapes and "banjo" tops, but we use a couple of 3-1/2HP Porter Cable Routers with seaming bits for that.

The ShopBot does sink cutouts and faucet hole cutouts. Either china undermounts, routed face up, or solid surface undermounts, routed face down (because it gets recessed). Narrow faucet set, wide faucet set, or no faucet hole at all.

The intention is to product 80 to 120 tops per shift with the unit at about 5 minutes per top.

We use a fence, pneumatic rams and clamps, and a laser centerline projector. Slabs roll on, get aligned on the sink centerline mark with the laser and clamped in place. The operator selects the combo from the touch screen, touches the "GO" bar on the screen to initiate the cut.

We have a couple of distributors signed on that are replicating our setup.

[ryan_slaback]

Is there any reason you cannot make the best of both worlds? Perhaps change the entry to a single long ramp and then cut the rest of the profile at the full depth. In other words something like this:

M3 1,1,1
JZ 0
M3 1,13,-.5
M3 10,13,-.5
M3 10,1,-.5
M3 1,1,-.5
M3 1,13,-.5
JZ 1
JH

It won't cut as much with the whole bit as the original, but it will cut twice as much with the whole bit as your new method. I would think the long ramp would be sufficient to take most of the vertical stress off the bearings too.

[bcammack]

I use the CC command presently. Here's the sink cutout code. I only use discrete movement commands for the lead out subroutine.:

&repetitions = 1

' Jog to safe height if not already there.
IF %(3) < %(28) THEN JZ, %(28)

[ryan_slaback]

Brett,
Knowing now that these are ovals makes it a bit more difficult, but the code could be changed to make the Z plunge from say 2 o'clock to 6 o'clock and then cut the regular ellipse command at the full depth.

As far as programing it to cut the entry arc, I would think you could do it in a 3D CAD package. I personally have no experience with it though.