Very fast machining in ply with a Multicam Trident CNC router

Hi there, new proud member of Wodwork Forums here, glad to be on board!

I'm currently renting time with a Multicam Trident router over at Fab9 in Footscray, VIC. It's a combination router / sign cutter with a 6.7HP spindle and costs $50 an hour to use.

I'm cutting a large number (12-16) of small two-side 3D profiles out of 18mm plywood, making a total of 24-32 cuts in total. This means that doing the cuts quickly is critical to the viability of the project. If each side takes 2 hours to complete, the total cost of the project is at least $2,400 in router time alone, which is unacceptable. If each side takes 20 minutes to complete, the total cost is only $400.

So my big focus is on dramatically improving machining time, and I'm willing to sacrifice the quality of surface finish to this end. I have a 1/2 diameter 3 flute down cut roughing bit with a 3mm corner radius that I'm hoping will be able to fly through the plywood really quickly, and also do 3D acceptable profiling.

My question is this - does anyone here have experience using high feed rates (7200mm/min +) using a roughing bit in plywood? I guess I'm looking for validation that this is possible / safe with the right setup, and confirmation that the torque of my spindle is up for the job. Any other info along these lines would also be massively appreciated!

As Kryn has rightly pointed out, the big unknown here is the rigidity of the machine. There is no specification for rigidity that I can find, so if that is the primary limiting factor for feedrate, how do I determine it? Simply by running successively faster feeds and listening out for chatter?

The ply is furniture grade birch, 18mm.

Thanks in advance,
Jez

Welcome to a TOP FORUM.
I can't really offer any suggestions as I'm still trying to get my head around the small one I have.
When you say cutting plywood, it would help if you mentioned the type of plywood you're (proposing) using, as that can have a bearing as to the speed used.
Furniture Grade for example, is made from better quality veneers than Construction Ply and Marine Ply is different again, as they use different adhesives also. Construction ply chips/splits the surfaces, not sure about the other grades as I've not had much to do with them.
There would be other contibuting factors as well, rigidy of the machine etc, hopefully someone with knowledge of the actual machine would be able to help.
HTH
Kryn

Thanks Kryn, I updated my question with your suggestions

What you're calling "very fast" is a normal day at the office for a machine like that. I used to run a 1/2" 3-flute up-spiral roughing bit at 12,000 mm/min with a spindle speed of 18k rpm all the time in 19mm ply on a vacuum table.

That machine should have no problem with rigidity even at double that feed, they're designed for high-feed nesting and will happily run hard all day.

Thanks elanjacobs, that's great to hear. I'm a beginner so I'm still calibrating my expectations as to what is possible.

The cuts you're describing - were they full depth / full width slotting at 12,000mm/min? Or lighter cuts?

I also made a mistake - the spindle is 6.7HP, not 10HP. Does that make a big difference?

Thanks

When attempting to run "fast" with a CNC, it is important to size the bit to the job. For example, don't use a 2" long bit when you are only cutting 18mm ply. You are much better off with a 3/4" cutting length as the bit will be far less likely to snap like a twig (yeah, they do that....even the 20mm diameter carbides!!!). Also make sure you mount the bit deep into the collet, without bottoming out, so you aren't unnecessarily increasing the effective length of the tooling. The shorter you can keep everything, the less flex from the bit which will result in lower cutting noise and improved finish off the tool as well as opening up the possibility of ~30m/min feed speed.

:whs:

Full depth, full width, full speed. When nesting small parts it's best to cut all the parts leaving 1-2mm on the bottom so everything is still attached to the sheet, then come back at the end and cut through the last bit because the tool pressure of a full cut can cause small parts to move or even lift off the table entirely.

Don't worry about power, I was doing 14mm wide x 40mm deep cuts in hardwood in one pass with 7.5hp (6,000 mm/min feed for surface finish, probably could have bumped it up to 10,000 quite happily); you'll snap the bit before you run out of power.

I had a go and got 8,000mm/min @ 16,000rpm quite happily with very low noise and a good finish. That's with a 3 flute downcut roughing bit. The manager was reluctant to drive the machine any faster but I suspect that it would perform the job admirably.

I was also able to reduce my feed times by using aggressive slotting and then full depth profiling - this was about 15x faster than using the adaptive clearing algorithm in Fusion 360 (Adaptive clearing is supposedly a "high speed machining" toolpath. Turns out this approach is only really useful for cutting steel - in plywood it's much faster to simply plough through the material straight on without looking back!). Reduced cutting time from 2.5 hours to 10 minutes per side!!!!!!!!!!

Another tip specific to the Multicam Trident and Fusion 360: turning on the "Smoothing" option increased the cutting speed by about 3x. Without smoothing, the tool was dwelling in one spot for too long and started to burn the stock. Always turn this on.

Thanks for the anecdotes everyone, I'll post back here if I find anything else worth mentioning.

With the machine times that you were initially looking at, I was going to suggest that you pay a lot of attention to the router bit, but with the shorter machine times it may not be so critical. MDF, chipboard melamine and plywood all have different densities and hardness throughout the sheet for a variety of reasons, with plywood its the glue layers being typically harder than the veneer layers, causing localised wear on the bit if you are cutting at one depth most of the time.This can leave very narrow blunt points along the edge of the flutes, while most of the bit remains sharp and usable. This should not be an issue sheet to sheet with your cut times down to 10 minutes but I would still keep an eye on the bits over production runs.

Most people running these types of machines have specific CAM packages tailored to optimise and suit the machine to give them greatest efficiency and throughput. Operators can generally import your your job and process it to create an extremely efficient code for the machine to follow. Generic proccessors can typically create some code, but as you have found it can be somewhat inefficient. If you need to run a batch of parts, it's generally more cost effective to pay the owner for the programming time in order to get very efficient machine time.

Thanks Malb for sharing your experience.

Unfortunately the CAM package we have tailored for the machine is Enroute which is useful for 2D operations only. We do have a postprocessor for Fusion360 specific to A2MC routers that optimises the Gcode somewhat, but it has some inefficiencies and bugs. Currently I'm trying to figure out if the A2MC will accept 3D arcs (G18 and G19 codes), or if all 3D profiling has to be done as linear segments, which is slower.