[sploo]

I've been successfully cutting MDF on a K2 CNC machine, details below:

Bit: 1/4" two-flute spiral upcut
Speed: 120ipm
Depth of cut: 1/4"
Router: 2.25hp Porter-Cable
RPM: 14,000 to 16,000

The RPM is higher than what I've calculated from most chip load charts, but seems to give the best results. I also tend to do a full depth, 60ipm finishing pass to remove the final 1/16" if I'm cutting 3/4" boards.

I've been asked to cut some parts from good quality plywood, but I've not had much experience/luck with this material. I get a pretty clean cut in MDF, but I've always found plywood splinters with the upcut spiral bit.

I'm assuming a two flute straight bit would be preferable*, but could someone give me a starting point for suitable feeds and speeds, given the above HP capabilities?

* I don't have the HP to do a full depth cut (3/4"), so a compression bit probably wouldn't be ideal, and they're incredibly expensive in the UK.

[CNCPROMAN]

A mortising compression bit will work fine because the up cut part is only 0.200 and you can make 3 passes. Rule of thumb is bit diameter X 600 will be your speed. At horse power would be your depth 7.5 hp will be one pass, 0.5hp will be 2 passes, so 2.5hp will be 3 passes. RPM is 16000-18000

hope that helps

CVV

[Syil_Australia]

Hello sploo.

In our main business (www.capeboatworks.com.au) we cut Marine Plywood every day. for plywood 6mm and less we use a 1/4 Solid Carbide upcut 2 flute and cut at 400 IPM , one pass and nice clean edges. Sometimes with plywood you will get some chip out across the grain but it is minimal.

For 9mm and thicker ply we use a 3/8 2 flute upcut as we need a stronger bit at those speeds otherwise they just snap.

When we have to cut plywood 15mm and above we do the cut in 2 passes using the 3/8 bit. 3/8 is about as large as you would want to go without having a larger HP spindle.

Keep the feed rates up as fast as you can.

Are you using Mach Quantum???.. Since switching to Quantum the quality of our cutting has improved because Quantum slows down and produces better curves and corners.

Hope this helps.

Cheers

Frans

[sploo]

Thanks for the responses guys!

A mortising compression bit will work fine because the up cut part is only 0.200 and you can make 3 passes. Rule of thumb is bit diameter X 600 will be your speed. At horse power would be your depth 7.5 hp will be one pass, 0.5hp will be 2 passes, so 2.5hp will be 3 passes. RPM is 16000-18000

hope that helps

CVV

Interesting... bit diameter x 600 would be 150ipm for me, which is faster than I'm running through MDF.

I keep getting the feeling I could/should be pushing the machine faster than I am currently, though I'm a little reluctant after having a couple of unpleasant experiences with hardwoods.

150ipm at 16-18k is basically scaling up the speeds I listed about by around 25%.

I don't mind taking quite a few passes if that protects the router bit. It's mainly getting a clean cut that I'm after.

Hello sploo.

In our main business (www.capeboatworks.com.au) we cut Marine Plywood every day. for plywood 6mm and less we use a 1/4 Solid Carbide upcut 2 flute and cut at 400 IPM , one pass and nice clean edges. Sometimes with plywood you will get some chip out across the grain but it is minimal.

For 9mm and thicker ply we use a 3/8 2 flute upcut as we need a stronger bit at those speeds otherwise they just snap.

When we have to cut plywood 15mm and above we do the cut in 2 passes using the 3/8 bit. 3/8 is about as large as you would want to go without having a larger HP spindle.

Keep the feed rates up as fast as you can.

Are you using Mach Quantum???.. Since switching to Quantum the quality of our cutting has improved because Quantum slows down and produces better curves and corners.

Hope this helps.

Cheers

Frans

400ipm is way out of my league... and budget!

That's good news to hear you're using a 1/4 Solid Carbide upcut 2 flute bit, as that's exactly what I'm using. What RPM speeds are you running? I guess I could scale the feed and RPM speeds down to the 120ipm region my machine is comfortable doing.

I'm currently using Mach 3, and haven't seen Quantum. Can it coexist on one PC with Mach 3?

Nice boats BTW - I have seen your site before.

[ger21]

I'm currently using Mach 3, and haven't seen Quantum. Can it coexist on one PC with Mach 3?

Yes, it can co exist. Get it at www.machsupport.com

[sploo]

Thanks Gerry. I've been a bit out of the loop regarding Mach development, as I got a setup that works, and haven't played with it since (the K2 control box does seem to be quite sensitive to changes in the Mach setup - I can easily get it to cut out by making things a little faster, or not respond at all).

Having read some of the forum posts about Quantum I'm quite interested. I'd be fairly confident a low weight gantry machine like my 3925 would benefit from the acceleration ramping, as the jerks due to rapid changes in direction can easily be felt if touching the machine.

That said, it's still in an unsupported development state, so I'd be reluctant to use it on a 'live' setup until it's a bit more mature (though I do see very positive feedback on the forum).

Do you use upcut bits on plywood when you're after a clean cut, or are you using straight fluted (or even compression) bits?

[ger21]

Straight carbide tipped bits will always leave a fuzzy edge when cutting across the grain. With sharp bits, though, it's easy to sand off. For best results, a compression bit is the way to go. But I only have experience with a 10HP router, so don't know how that would work with your Porter Cable.

[buckey29]

I had some similiar questions. Found a page that gives some info in upcut vs downcut, vs compression, etc.

http://www.toolsxp.com/onrbtoolselection.asp

[sploo]

Straight carbide tipped bits will always leave a fuzzy edge when cutting across the grain. With sharp bits, though, it's easy to sand off. For best results, a compression bit is the way to go. But I only have experience with a 10HP router, so don't know how that would work with your Porter Cable.

Thanks Gerry. I'm beginning to wonder if the small amount of plywood I've cut before is of particularly poor quality, as it splintered quite a lot.

Something I'd love to see, but have never found, is a table of feed speeds, RPM and depth of cut for different types of bit in different materials for different spindle HP ratings.

Or is this not that easy (i.e. it's likely to change for different machines, even if they have the same spindle HP)?

I had some similiar questions. Found a page that gives some info in upcut vs downcut, vs compression, etc.

http://www.toolsxp.com/onrbtoolselection.asp

Thanks buckey.

[ger21]

They don't consider HP when they tell you the chip load, because that's the ideal rpm and feedrate that that tool should be run at. If you don't have the HP to run at that chipload, you have two options. Take shallower cuts at the proper chip load, or slow down the feedrate. Unfortunately, using a compression bit, you're only option would be to lower the feedrate. Although that will work, it will have an effect on tool life.

[CNCPROMAN]

ger21
I think we agree with each other. When you don’t have the horse power you need to make multiply passes. This formula has work good for me for the past 15 years and it is a good start point for anyone cutting on a CNC machine, cutting wood. I just wanted to share what works good for me.

CVV