Fluffy mdf

I am new to the world of cnc but have been woodworking for years. I have been making models out of mdf for a few years now and have been routing these using a handheld or table top router. I have been using standard grade 18mm mdf from local B&Q stores etc with no issues. Using the same mdf on the cnc the finish cut is very poor. The core (centre part of the board) goes extremely fluffy and you can see a slight step where the cutter has moved to the next cut down. I have been reading that there are different grades of mdf and maybe the stuff I have been buying is not dense enough. The other observation I have made is following the feed speed calculator the router moves very quickly over the piece. I am wondering if anyone else has experienced this problem and can offer a solution

Thanks Steven

Make sure the mdf isn't damp.

I have.the same problem

Thanks jcb. Mdf is bone dry in my workshop. As mentioned above I don't have any issues routing the stuff manually only on the cnc

If the same material machines well wiTh a hand router, the problem must be with the cnc. Never mind the calculated speeds ctc. try to replicate the hand router conditions, speed feed same cutter etc. If the problems persists it sounds to me that it may be a rigidity or vibration problem. G.

Thanks Geoffrey. It's a brand new machine albeit from the cheaper end of the market. I have routed all sorts of other types of softwoods and hardwoods and they have been perfect. I think the speed of the router has a lot to do with it. Will try slowing down the feed rate. Steven

You might find you have to slow the CNC down to a snails pace. The MDF from B&Q and the likes is the lowest grade. Go to Wickes or Jewson and get the moisture resistant type. This is about the best you can get easily. If you have a good wood merchant they should be able to get you deep router grade which makes B&Q MDF look like toilet paper. It will be double the price though, but the reduction in messing about with sorting the edges can make it good value.

Cheers Ritchie. Just went and bought a sheet of Medite MR. It's a much denser board and not that much more expensive £26 per 8x4 sheet. Thinking about the speed I pass the piece with manual router it's an awful lot slower than the cnc. So with denser mdf and slower feed speed I will hopefully get the result I am looking for. Will let you know how I get on. Steven

Quote:

---

Originally Posted by richie00boy

You might find you have to slow the CNC down to a snails pace.

---

No quite the opposite.!! . . .Chances are your not cutting fast enough or deep enough.

What speed & feeds are you using and what DOC.

Also what machine is it.? If it's the 6030-40 type machine then chances are you'll never be able to cut MDF without flufff has it's not upto the job.?

Jazz - just tried Medite MR mdf at a feed speed of 20mm/sec and this has stopped the fluffy core. Not sure what the spindle speed as its reading a frequency number (3000) not rpm. DOC was 3mm through an 18mm board. Its a beautiful finish even better than the manual router finish which I was pleased with. The issue now is it takes a nation to route so next trial will be to step the feed speed up a bit and maybe try and increase DOC. Not sure how much life I will get from the cutter
Thanks for everyones input on this one as I was giving up hope. Hopefully this will be of use to anyone else with the same problem.
Attachment 9536

3000 won't be the frequency as it's far too high. It's probably the RPM!

Unless the MDF is damp you shouldn't get fluff no matter the manufacturer. If you getting fluff then your cutting wrong for the density of that material, the Medite MR will just be a different grade or density and you've got lucky on Feeds etc.

20mm/s is far to slow for MDF not matter what size cutter or DOC and even if you were cutting at 3000 Rpm which again is ridiculously slow for MDF or wood it's all wrong.

Every machine needs feeds & speeds tweaking to suit it's build but even allowing for that these feeds are way off. I think you'll find the cutters will wear very quickly.

Give some details of cutter and an idea of the strength of machine, also spindle your using IE: picture and will suggest some feeds to try.

Just to give an idea.
With my DIY cnc router, I can do 18mm MDF cutting at around 3-4m/min, full doc @ 24k rpm, with a 10mm twin straight flute TCT cutter.
I am left with clean cuts, no fur's etc.

Quote:

---

Originally Posted by Mad Professor

Just to give an idea.
With my DIY cnc router, I can do 18mm MDF cutting at around 3-4m/min, full doc @ 24k rpm, with a 10mm twin straight flute TCT cutter.
I am left with clean cuts, no fur's etc.

---

Ye but that's only because of them brackets I cut for ya . . .:hysterical:

Now that's more like the speeds and with a decent sized cutter, thou I would suggest doing faster in 2 passes for increased tool life.
I always work on 50% cutter Dia has max DOC thou in soft stuff like this I'd do 100%.

I think a lot of people under estimate the importance of speeds and feeds and how they affect tool life.

Mad Profs calc are to run at 50 to 60mm/sec. What would you recommend with a 6mm twin straight fluted bit. Also would it be possible to do this in say 3 passes? Still not sure what the VFD readout at 3000 means. The readout can go to 4000 when up full. The max spindle speed is 14,000rpm according to the spindle spec.
I agree that speeds and feeds will have a big influence on tool life. Obviously I am looking for the best running conditions for longest tool life on this type of mdf

Maybe the VFD is not setup correctly?? It could well be that your cutter is only spinning at 3000RPM! Have you got a tacho so you can check the ACTUAL spindle speed? Or maybe it's Watts? Is it a 4kW spindle?

Had a look at the VFD display and its set at Hz. There is a light to read in rpm but haven't figured out how to display this yet. Not being electrically minded I have assumed that 4000Hz is 14,000 rpm. Right or wrong

With 6mm cutter at 6mm DOC 13,000RPM the minimum I'd be cutting at would be 4mtr/min and that's allowing for a weak machine. If your machine is strong-ish then you'll be wanting to be around 5-6Mtr/min and could go much higher if wanted 8-9mtr/min with 14-15K rpm.

The VfD could be showing Hz but it may be 400.0Hz not 4000Hz and it's not showing the point. What make of VFD is it.?

Thanks for that. Will try tomorrow. It's a Chinese machine so no idea what make the vfd is

Still no mention of the type of cutter used? I have better results using a single or two flute cutter. Using a three or above cutter results in fluffy edges on cheap MDF. Rules here is always cut your material as soon as you buy it as well, MDF that has been laying around is not good unless you buy premium material.

I have been using a 6mm two fluted bit. Bought the material today that ran well. The cheap mdf had been in my store for about 6 months. Definitely the quality of board makes a big difference. It's finding the optimum speed and feeds rates for it

Quote:

---

Originally Posted by Steven W

The cheap mdf had been in my store for about 6 months. Definitely the quality of board makes a big difference. It's finding the optimum speed and feeds rates for it

---

That will be your problem.? It's soaked up all that Scottish air. Bet if you measure it accurately it's thicker than the new stuff.?
Bloody hate MDF it's not even fit for burning.!!!

Hear what you're saying. If I remember correctly its expanded by about 0.3mm since I bought it. It suits my purpose for the types of model I make but there is nothing better than working with real hardwood

Just to update. Cut a few models yesterday with a feedrate of 40mm/sec at 6mm DOC. The spindle was running a 6mm two fluted bit at 24,000rpm (flat out according to the dial). The cut was just as good when running at 20mm/sec. When I went above 40mm/sec there was like chatter marks on the cut edge. Is this due to the feed speed being too fast for the cutter speed or is it that the cutter is getting blunt. I have never seen this before

Quote:

---

Originally Posted by Steven W

When I went above 40mm/sec there was like chatter marks on the cut edge. Is this due to the feed speed being too fast for the cutter speed or is it that the cutter is getting blunt. I have never seen this before

---

This could be a combination of things.? Basicly what it's showing you is the limit of your machines strength.
The main issue will be a combination of Z axis strength or extension if overly extended and cutter extension from spindle. Then there's the machine structure it's self. . . .This is why I asked before to see a picture of machine to get a gauge of how well it's designed and built.

It's a basic Chinese machine. I didn't want to spend a lot of money on something that didn't suit what I was doing. The table is 300x400 and the models I cut are from a blank 300x300. The spindle is 1.5kw water cooled. One of the issues I have is getting the 6mm cutter Far enough into the Collet. The cutter that came with the machine is exactly 6mm and fits great but bits you buy in the UK are quarter inch. I struggle to get the bit far enough up the collet to screw the lock nut on. This may be causing the chatter?

Quote:

---

Originally Posted by Steven W

The cutter that came with the machine is exactly 6mm and fits great but bits you buy in the UK are quarter inch. I struggle to get the bit far enough up the collet to screw the lock nut on. This may be causing the chatter?

---

If your spindle can take 8mm collet then buy 8mm shank tooling this helps with reducing chatter, you can get 6mm cutter with 8mm shanks. Look here. . Wealden Tool Company Limited Up Cut


To use 1/4 tooling you really need a 7mm collet. Trying to force 6.35 into 6mm will reduce collet life.

I got my 1/4 inch collet for my spoil board surfacing cutter from Arc Euro Trade.
ER Collets - Arc Euro Trade

And the collet nut from ebay seller onlineseller68.
Collet Chuck holder, Cutting tool Endmills items in YSTOOL store on eBay!

silly question but you are going the right way,i mean the spindle is actually turning in the right direction to the tool

Quote:

---

Originally Posted by Steven W

It's a basic Chinese machine. I didn't want to spend a lot of money on something that didn't suit what I was doing. The table is 300x400 and the models I cut are from a blank 300x300. The spindle is 1.5kw water cooled. One of the issues I have is getting the 6mm cutter Far enough into the Collet. The cutter that came with the machine is exactly 6mm and fits great but bits you buy in the UK are quarter inch. I struggle to get the bit far enough up the collet to screw the lock nut on. This may be causing the chatter?

---

You should never force a 1/4" shank into a 6mm collet or clamp down a 1/4" collet onto a 6mm shank... You'll either damage the collet, the bit won't run true, damage the spindle with the out of balance load or all the above.

Routing - Some Beginners' Tips

Router Bit Trouble Shooting

I think you probably have an ER11 or ER20 collet on the end of that spindle. Extra collets aren't very expensive (take a look at Arc Euro Trade, for example) and it's well worth using the right ones. In theory, one collet will handle nominal size shanks or up to 1mm smaller but especially in the smaller sizes they don't like compressing that easily so I also use a mix of metric and imperial size collets. 6mm shank cutters go in a 6mm collet and the 1/4" cutters (nominal 6.35mm) go in a 1/4" collet rather than using the larger collet for both. You only have to save one broken cutter to make up the cost of a collet!

Yes, Arc Euro is a good place to get individual collets. I got a set in 1mm increments off eBay, then got 1mm, 1/8" and 1/4" collets from Arc. You can put a 1/4" cutter in a 7mm collet, but it'll wear out the collet faster and takes longer to do up the nut!

With the ER collet system you should never try and clamp a cutter that's bigger than the diameter of the collet, even if it's just 0.1mm bigger. Depending on the size, they can clamp 0.5-1mm smaller than the nominal diameter.

I'm a bit late to the party here but do have a long running love hate relationship with MDF. Love it because its cheap, hate it because its cheap! lol

As others have said, the furring is because B&Q supply cardboard badged up as MDF - yes its really that bad. Complete junk and I'd avoid it at all costs, I've never got a decent edge finish from this stuff yet.

Medite is ok at the budget end though thickness's above 25mm do have a rather mushy core and again you'll get some furring but nothing like as bad as B&Q rubbish. At the top end you have Valchromat and I love this stuff. Zero furring, retains very small details and can be sanded smooth - almost like plastic when sanded upto 1200 grit. Its expensive though at £80 for 25mm thick 8x4ft sheet.

For reference I mostly cut at 7m/min 11,000rpm and 100% cutter diameter for DOC. Use carbide tooling and you can get amazing tool life, not sure how long exactly but a few months of use almost day in day out for me in MDF. Key to increasing tool life is keep your rpm low and your feedrates high.

I have cnc and manual routers. to do away with fluff on any material, I use down cutters whenever I can. feed speed max my cnc will do is 70 in per min.

Old discussion but here is my experience. Yes there is a kind of cheap MDF which is fluffy and generally very bad quality for work. I would say impossible.

Once i did 100 pieces , some lamp bases, for a friend and all was ok. Next time they bought the crappy material. OMG, it was a disaster.

Side by side before machining it was lighter in color and not so glossy as the real MDF. In short the best MDF i have found here in Spain is the darkest in color and the smoothest to the touch that gives you a glassy like feeling. And yes, from MDF to MDf there is a big difference even in one shop