Printable View
Hi guys,
We are trying to cut through 6.5mm and 9mm birch plywood sheets, ideally with a 5mm wide bit (so we can drill 5mm holes in the same pass).
We have purchased a number of different bits, double flute straight .. Up cut spiral etc..
What spindle speed do you think we should be running at? And feed rate also?
Cutting through the wood in 2/3 or three passes is fine!
We are using a 8x4 router, with a max spindle speed of 24'000 rpm (I believe).
Many thanks!
Well this depends really.!! How strong or well built is your machine.? If you go by the Calcs etc then the feeds and speeds are very high for a 5mm cutter.
For instance G-wizzard gives the following for PLy with 5mm 2 flute carbide cutter cutting full 5mm slot.
Opitmized for best tool deflection, which is good for thin tooling as reduces chances of snapping. . . DOC 1.4mm Feed 17500mm/min spindle 28700RPM. . !!!!!
Carbide tooling but not optimized with DOC 2mm(40% cutter Dia) feed= 16,500mm/min spindle =27,000rpm
HSS tooling not optimized with DOC 2mm(40% cutter Dia) Feed= 13,700mm/min spindle= 18,700rpm
Obviously your machine needs to be very strong and powerfull to handle these numbers so you'll need to decide for your self thru trial and error the best setup balance which suits your machine and the cutters/material your using.
Personally if your machine can handle the feed rates then I'd go with the HSS settings as a first port of call, even with carbide tooling.
Without knowing your machine it's very hard to advise so just take these numbers and use them as a guide.
Hi, Thanks for that.
We have a system based on this..
http://www.worldofcnc.com/complete-c...ge-p-2669.html
Its has a spindle Elte HF Spindle TMPE 9/2 220v and ''according'' to our quote paperwork is 1.1kw 2400 rpm 220v.
But this doesn't sound right.. i'm sure its spinning nearer 24000 rpm! I'm actually waiting to hear back from the supplier as we've been left with the installed machine and no instructions how to change the spindle speed! It's running off an invertor which controls the speed.
Its all working nicely, but looking to improve and optimise the cut setup.
So going back to the router bits, what style of bit (and width) would you recommend?
I've seen it said that single flute upcut spiral would be good?
Ignoring the drilling of 5mm holes.. so could increase the width of bit for the channeling work.
Thanks again.
James
p.s we are pretty new to this and really appreciate the advice.
Sorry to say this but that machine won't be able to cut anywhere near those speeds & feeds.!! It's just not strong enough. If it did manage to do them it wouldn't handle them for very long before stressing the machine.
The spindle is a good brand but it's still low power at 1.1KW (1.5HP) and between the machine strength and this then you'll have to cut at much lower DOC and feeds.. . . OR . . . really low DOC and high feeds. . . Basicly you won't be able to have both deep DOC & high feeds.!
Regards cutters then yes spiral single flute will work good and actually would lower the required feed rate and spindle speeds.
The spiral upcut would work ok because they are designed to lift and clear chips and give a very clean cut with very little burning when plunging.! . . .BUT . . This depends on the material your cutting and it's thickness.? Because it's a upcut then it's trying to lift the material so if it's thinner material and wide with very little support in the middle then it will lift material off the bed. Upcuts and thinner material really need to be used with vacuum beds.
Down cuts are safer bet and best used for thin material with no vacuum and they give a very nice finish.! . . .BUT. . They require very good chip extraction due to the fact they are pushing the chips downwards which will clog and pack the cutter resulting in re-cutting chips leaving a poor finish or even breakage.
So basicly if the material is heavy then go for spiral up cut.! . . If thin then spiral downcut.
Just remember the biggest killer of tooling regards wear and even breakage is insufficient feed rates. Ideally you want to find the chipload for that particular cutter, Chipload is the most accurate way to judge feeds & speeds regards tool life and giving best finish. Most good tool suppliers should be able to supply this info or give a guide to feed & speeds for material being cut.
So here's another guide for you based on single flute carbide cutter in plywood in various DOC.
( I quote Carbide because they last the longest, esp in MDF and Ply)
Carbide standard single flute (not spiral) 6mm cutter full slot.
DOC= 1mm Feed=7600mm/min Spindle 24,250RPM
DOC= 2mm Feed=7300mm/min Spindle 23,300RPM
DOC= 3mm Feed=6650mm/min Spindle 21,200RPM
DOC= 4mm Feed=5850mm/min Spindle 20,900RPM
Opitmised for deflection 6mm carbide
DOC= 6mm Feed=5850mm/min Spindle 20,100RPM
Hope this helps.
L
Hi,
Thank you for all this info!
We are cutting 6.5mm and 9mm Birch plywood, ideally cutting right through within 2/3 passes. (ie 3mm per pass maybe?)
We have a large side channel blower (vac pump) connected to a pipe distro system under the table, which then feeds into 5 vacuum zones. We have ultralight 25mm MDF (plained on both sides) spoil board, so vacuum old down is covered!
We are meant to have this spindle .. http://www.marchantdice.com/worldofcnc/pdf/ELTE.pdf .. The 1.1kw version.
The inverter runs it at 3 phase I believe.
We were assured it was more than suitable for the requirements we have, and that they have clients cutting though 21mm ply. We have run a few tests on 6.5mm ply and it does work quite nicely, just looking to optimise it now..
However we think they've installed a different spindle to what we are meant to have! We think we have this .. http://www.worldofcnc.com/milling-sp...or-p-2671.html
Once we've straightened out the spindle clarification we should have a machine that can run upto 24000 rpm and a max feedrate of around 5800 mm/min.
I hope that clarifies our situation!
Cheers James
Hi James,Quote:
Originally Posted by FlightCaseCo
Can the machine cut at 5,800 feed or is that just rapid speed? There's a big difference.! I would would expect with it being R&P that would be cutting feed.?
Hi,
Had some major progress this afternoon, using a single flute up cut bit (5mm wide).
With spindle at max (18000 rpm we think) we tested cutting through the plywood at 3mm and 5mm depths, then tested speeds from 1200 mm/m upto 5000 mm/m.
All speeds gave good results, however over 2000 mm/m it was fantastic! Beautifully clean finish.
More tests to be done this week, also need to get the spindle issue sorted! Ie the one we paid for!
Will keep you updated!
Thank you.
A quick on-topic hijack if I may. Why do hand-held routers use straight flute cutters? A good brand is certainly expensive enough to have any design that works well. When cutting wood on CNC, is there a reason to use spiral cutters instead?
Yes because hand routing is relatively slow feed rates in comparison to CNC the straight flute cutters have more time to clear chips. CNC use high feed rates so spiral upcut helps with chip clearence and still maintain a good quality finish.Quote:
Originally Posted by Tenson
So what is the advantage of straight flute then?
Mainly because there generaly cheaper and easier to handle in a Hand router.!Quote:
Originally Posted by Tenson
The straight flute hand-router bits I have are certainly not cheaper. I like Trend cutters, and you can see the price list here for straight 2-flute. These prices are not uncommon. Trend also make spiral bits, but strangely they only maker larger than 3mm dia. with a guide bearing attached?
Anyway, you recommend spiral cutters for CNC. Should I use a different type of bit for routing hardwood / MDF than for aluminium and other soft metals? I'd intuitively expect metal cutting bits to take a more shallow angle of cut.
Is there a worthwhile difference using HSS for softwood or should I just stick to carbide?
I suspect they are if you compare like with like - i.e. compare trend prices to companies in England/USA selling carbide spiral cutters intended for CNC.Quote:
Originally Posted by Tenson
It depends on that many factors we can't really recommend without more idea of what you're cutting. Balsa and oak are both hardwoods yet clearly will be treated differently.Quote:
Originally Posted by Tenson
In general on a CNC router single flute carbide cutters are the best for aluminium/brass since only one flute leaves more room for the swarf to clear. This helps prevent re-cutting of the chips, ultimately resulting in a higher feedrate and better finish than other cutters:
http://www.ebay.co.uk/itm/5x-6mm-Car...item20b95dbb6d
If you're looking for one cutter to do everything those are the nearest I've found since they also work well in plywood, nylon, polycarbonate, copper, pine plus some other hardwoods I've cut but don't know the name of.
Definitely use carbide as it will last much longer. That's especially true for composite woods, like MDF or plywood where the adhesive makes the material very abrasive.Quote:
Originally Posted by Tenson
Apparently the bits you linked to there are 'tasteless' :)