Cutting speed and depth in MDF

[andrewm]

I have finnally got my parts files all worked out but need to speed things up now. I am cutting 3/4" MDF with a 1/4" end mill bit. Trying both single flute and a downspiral Onsrot (sp?) bits. I am currently cutting the 3/4" inch with 3 passes at 1.7" sec at 17000rpm. This is way too slow and I suspect I can speed it up. Basically this is just slight modifications to the default setting in Parts Wizard.

1. How much can I push these to get my parts cut out faster without killing my quality?
2. Can I cut through 3/4" in a single pass? If so at what feed rate and RPM?
3. Which will cut faster, a single flute or down spiral?

Thanks,
Andrew

[barrowj]

Andrew
I cut 3/4" mdf with a 1/4" sprial upcut or downcut in one pass at 1.25" at 16,000. I use the onsrud and mlcswoodworking.com bits and they seem to last a long time.
Shopbot will also advise to cut in 2 passes at 2"/sec at 16k. You could cut most of the material in one pass leaving a minute amount for the second cut. This would also give you a clean edge.
Joe

[elcruisr]

I single pass 3/4" mdf with 3/8" tooling. 1/4" has too much flex for single passing. I usually prefer a single flute compression spiral as my parts edges need to be clean top and bottom. Onsrud makes one with a very short upcut so most of the cutting force is still pushing the part down to the spoil board. At 1.7" / sec I'd only be running at 11,000 RPM or so, more than that is just generating heat and dulling tooling. I do run a spindle so my rpm selection is very wide. At the feed speeds we can push a single flute bit is all the cutting edges we really need for most of our work.

Eric

[andrewm]

Eric,
Going to a 3/8" sounds like a good idea. Those compression spiral bits are over $60 a peice! Are they worth the extra money verses just a straight single flute 3/8" bit? (~$18)

Thanks,
Andrew

[elcruisr]

Depends on what the results are that you need. I need clean edges top and bottom and a smooth cut. If tooling price is a big concern on the job,I'd start with the single flute straight and see if it gets you the cut quality / lifespan you need. I have so many compression spirals on hand it's what I tend to use. We can get 8 to 12 hours of cutting life out of ours and then resharpen 2 to 3 times. They never last as long after sharpening but will usually go 6 hours. MDF is hard on tooling! The edge quality is pretty high with these bits and I just factor their cost into the job. The secret to making your bits last is to keep the rpms as low as you can without sacrificing cut quality. If you can hold down the parts an up spiral might be worth trying as well. It'll clear more material out of the cut faster which also can help cutter life a little. I've even known a few shops to use high speed steel bits on their MDF and particle board jobs, they don't last long but they're cheap and can be resharpened several times. A little experimentation will tell you a whole lot!

Eric

[elcruisr]

Depends on what the results are that you need. I need clean edges top and bottom and a smooth cut. If tooling price is a big concern on the job,I'd start with the single flute straight and see if it gets you the cut quality / lifespan you need. I have so many compression spirals on hand it's what I tend to use. We can get 8 to 12 hours of cutting life out of ours and then resharpen 2 to 3 times. They never last as long after sharpening but will usually go 6 hours. MDF is hard on tooling! The edge quality is pretty high with these bits and I just factor their cost into the job. The secret to making your bits last is to keep the rpms as low as you can without sacrificing cut quality. If you can hold down the parts an up spiral might be worth trying as well. It'll clear more material out of the cut faster which also can help cutter life a little. I've even known a few shops to use high speed steel bits on their MDF and particle board jobs, they don't last long but they're cheap and can be resharpened several times. A little experimentation will tell you a whole lot!

Eric

[garbob]

Hi Eric,

I buy my Onsrud bits from a distributor that tells me that spirals and compression bits can't be resharpened. The last time that I talked to Onsrud they said these bits could be resharpened.

Are you getting your bits resharpened from the Onsrud distributor that you purchase them from? Could you tell us who you deal with for purchasing and resharpening these bits?

Thanks

[elcruisr]

Gary,
your distributor must be boosting sales. From the Onsrud rep I'm told the only spirals not to resharpen are some of the spiral o-flute plastics bits. I've been buying from one of Onsruds central Fl. distributers and having them sharpened by a local sharpening shop that is equipped for spirals. I'd use Onsrud and get a little better job but I get free pick up and delivery from the local shop so I use them right now. The Onsrud people might not be real thrilled about one of their distributors passing out bad info. You are supposed to send them in to Onsrud via their distributor for resharpening. You might contact the company to see what's up with that guy.


We use Nu-Mark Distributing in the Clearwater area at:

727-561-0736

We resharpen through National Saw in Largo at:

727-532-9159 Ask for Tom Lewis

I think I pay around $16 for compression spirals but don't quote me on that, I just hand the invoices to the accounting dept. (My brother!)

Eric

[Jimmy Walker]

Mr. Eric Lamoray.

I am new to the Shopboting world, and after reading most of this forum, you seem to be the man to ask. My shopbot has twin "Z" axis's I was planing to use one to cut the shape and use the other to clean out the middle of my shape down to a set depth. What bit and router speed would you use to clear out a flat floor about 3/8" to 1/2" down into the MDF? Once the 3/8" cutter has created the inner and outer main cut.

Jimmy Walker.

[elcruisr]

Jimmy,
it depends on acceptable corner radius, edge quality and bottom of cut quality. I like to do clearing with the largest bit I can handle for the corner radius to save time. If top edge quality isn't an issue than I would use a 52-200 series in my shop. That should leave a pretty clean bottom with a little fuzz on the top edge. If the top edge is critical than the same bit in a down spiral or a compression spiral could be used. I've found the 60-100 series is still hard to beat as it is a true mortising design that can be plunged in. I still do ramped entries whenever possible though. According to the Onsrud rep there is also a tool designed just for MDF that I haven't run yet myself, It's a 48-700 series straight flute carbide tipped tool. Feeds and speeds for the different tooling can be found on Onsruds site as well as chiploading info. It's really all about chiploading in the end. The basic formula is:

(Feed speed in inches per minute divided by RPM)
divided by number of cutting edges=chip load

The reccomended chip load for MDF is a minimum of .008 and an average of .015 from my spindle manf.s specs. This gets you in the ball park on feeds and speeds. You can fine tune from there.

Eric