Since even before getting the CNC (just recently) I kept reading about panel processing times around 5-6 minutes.

We just did a run of 22 pieces of Columbia 7-ply for some relatively simple vanities, and our average run time (From Go Button to Sweep) was almost 22-minutes per panel with onion skin on the small parts (that's basically 2-panels per hour once you factor in loading, breaks, talking, etc).

I mean, could we do them in 6-minutes? Sure, I could throw them through at 24k and 1200/ipm with no onion skin, but the edge finish would be terrible with extensive fuzzing of alternating plies and we might have to duck an airborne small part here and there.

We have settled on 1/4" 2F Comp at 16,000 / 180ipm, because it seems to give the best results. Anything faster and we get terrible fuzzing of the ply edges. We've tried every combination of climb/conventional possible. We've tried multiple passes and single pass.

Our Block is half as big as our 21 spindle so we're dropping multiple shelf and dowel holes at a time.

What aren't we doing right? Are 5-minute panel processing times only for melamine? Is 20+ minutes on a sheet of plywood normal?

Don't get me wrong, we still walk away from that machine every day shaking our heads at how much wasted labor we have had over the years before we got the CNC, especially for our origami solid surface processing.

What used to take 6 individual processes at 4 separate stations (and some of those processes were pretty back-breaking) now happens in 1/10 of the time at one station.

But, because we don't know what we don't know, if we can somehow speed up our panel processing times, we sure would like to.

What machine do you have and do you do frameless or face frame cabinets?

Are you using a chip breaker bit? 1/4" is way too small if you want to go fast. 3/8 chip breaker should be your starting point for plywood.

We were using a 3/8 comp and even tried a 1/2” comp. The 1/4” seemed to give us the cleanest cuts in the plywood. No idea why. We haven’t tried any chip breaker bits yet. I’ll get a few and see if they can get our feed speeds up while keeping a clean edge.

I don’t think the limiting factor is the machine, it will push whatever we want as fast as we want.

I do remember reading that feed speeds aren’t the end all when it comes to panel processing, but if it isn’t the feed speeds that decrease panel processing times, then what else could it be?

Harry,
Depending on the rigidity of you machine, I run plywood with a 3/8" moritse compression tool, which gives me an acceptable cut on both faces without fuzzing. 18k and 1000ipm. Been doing it that way on 2 different machines for 20+ years, no problem. We just stay away from cheap plywood due to fuzzing and the panels not being flat enough.

We cut mostly ply.

Average I would guess 7 to 8 minutes per sheet of cabinet parts. Less than 3 minutes on concrete form jobs with no drilling and single pass.

Minimum 3/8 bit, best 1/2 chipbreaker compression spiral. As short a flute as you can get - we use 7/8. We use 2 passes, mainly for dust control, 0.5mm oversize depth less 1mm climb the first, conventional the second.

18K, 750 IPM minimum - usually 900 IPM.

Drilling is the biggest time waster on a CNC. Use solid carbide and 100 or 150 IPM feed with a 4K rpm drill block.

Some ply is worse than others for edge finish. If you need perfect, do the finish pass with a standard compression spiral, not a chipbreaker.

20 minutes per sheet is a lot. That's hardly worth the floorspace the cnc occupies at that rate, in my opinion.

We have a new machine and we haven't ran enough sheets to really have any data with it.

The old machine was 12hp spindle, and a 4x3 drill block. Average sheet time was 6-7 minutes on with 3/4" plywood. Which is the bulk of what we cut. And my cabinets are heavy on the machining. That's just machining. Total cycle time was around 12 minutes on average iv would say. From hitting the "go button" to hitting the "go button"

1/2" chipbreaker. Compression for cut out. Downsheer for non-through operations. 16k rpm, 672 ipm.
Cut out is done in 2 passes leaving a .030" skin. Mostly to aid the dust collection, but also to help prevent small part movement.
Dado operations are all single depth passes with that diameter tool.

I'm not overly concerned with the cut quality. Rarely is there anything we do, where those edges are left untreated or matter. It's either against another part, in a dado, against a countertop, or the floor. The remaining is either covered by a face frame or edge banding.

As already mentioned, cheap plywood cuts like crap. I'll add fir/aspen cores also cut poorly. The poplar core plywoods cut much cleaner in my experience.

This is one that kills me with watching some of the other machines. The ONLY time you are making money is when a tool is buried in the work piece. The rest of the time you are losing money.
So the rapid move between operations is REAL important.
Rapid on the old machine was ~2850ipm. My new one is supposed to be around 3500, but I haven't seen that performance from it yet.

I tend to not use stay down profile cutting when doing plywood. I think there's some speed gains to be had there, but it's pretty marginal and I've had more part movement from that than I would like.

And you never answered what machine

Without seeing the machining required for the panels it is difficult to give a good answer.

Though a 1/4" cutter at 180imp is likely part of the issue. Most users will use a 3/8" or 1/2" cutter at 900ipm or greater. In simple math what a larger cutter can do in 2 minutes or less a 1/4" cutter at 1/80ipm is taking 10 minutes.

Also, drilling holes adds a substantial amount of time to the time needed for each sheet. In most of the sheets I run, drilling consumes at around half or more of the time required to run a sheet.

Another factor is the type of CNC you are running. What are the capabilities of your machine? What size router bits can be used? What software is used to program the machine?

Thanks for all the responses.
I've been mulling them over to come up with a plan.

Software is Mozaik
The machine is a Holzher 7535 Flat Table Nesting 5x12.
Spindle is 24hp, 24k capable.
Transverse is 2k in X and 4k in Y.
8hp, 24 spindle block -w- 11 in X and 6 in Y; 1k to 6k rpm.

We dowel everything; 3 in the bottoms and two for nailers/stretchers.
Shotgun 5 or 7 hole shelf pins. Each line of holes drilled in one drop.
Mounting plate holes and glide holes all drilled.
We don't bore our hinges on doors.

I know the drilling takes a long time. But I am going to dig into those settings and see if they can't be sped up.

I ordered some "chip-breaker" bits to try and we'll go back to 1/2" instead of the 1/4". Currently we use 2 or 3 flute spiral compression bits. I'm thinking we went to the 1/4" because of a combination of small part movement and finish quality. We seem to have the small part movement resolved now that we have the onion skin sort of dialed in.

Climb vs Conventional? Well, sh%$, that's a whole different level of Rabbit Hole. I mean, apparently almost everyone if Australia cuts climb and most shops in the USA cut conventional? Some people do both? Does it help the feeds and the speeds? Well, some say yes, and some say no.

All I know is that I want to burn through material just as fast as possible, but also have an edge that doesn't have an 1/8" of fuzz on the alternating plies.

I know our machine is more than capable. As I've said, we can blaze through solid surface with a 1/2" O at ludicrous speeds. We can do a 4-side drop lip with pre-groove and v-groove, sink cut-out and faucet holes in about 3 and a half minutes. and the finish of the v-grooves is flawless.

As I've mentioned before, this is all brand new to us. We were a saw shop up until a few months ago. But 20-minutes on a panel is excruciating.

Some guys, from this forum and others, have mentioned slower RPMs from the 12k to 16k range. Other things I have read said to run the RPMs just as high as you can go. Do lower RPMs translate to a better finish or higher feed rates? We have followed the Tooling Manufacturers suggested feeds and speeds, but our results have definitely varied.

It's Saturday, so I'm first going to see just how fast I can blaze through some melamine, and then see if I can't ruin some super-cheap ApplePly we've got laying around to try and dial in the feeds and speeds for plywood.
(That was sarcasm. ApplePly is NOT cheap. But, it is sitting up there on the shelf just begging to be turned into dust.)

Again, thanks for the responses. Everything helps.

If your parts are moving you need to deal with that first. What size vacuum pump do you have? What vacuum are you pulling with a sheet on? Is the spoil board screwed down on the machine?

If you are doing 2 passes do the first climb and the 2nd conventional.

I have never found 3 flute bits to be worth it, especially with cabinet parts. You can't run the required feedrates.

~"I'm thinking we went to the 1/4" because of a combination of small part movement and finish quality. We seem to have the small part movement resolved now that we have the onion skin sort of dialed in."~

Dropout-
We don't have hold down issues anymore.
A combination of Part Placement and onion skinning eliminated that problem all-together.