Thread: Router Bits

Some compression bits are available from Carbatec tools.

These bits are really only suitable for if you want to cut material that keeps lifting when you try to cut it.

They are, generally speaking, more expensive that standard bits as not so many of them are made.

Nick, you haven't said what you want to machine, or the size and capacity of your machine.
Compression bits are primarily used for cutting materials with thin brittle surfaces, such as melamine sheets and plywoods with thin furniture grade veneer faces.
A compression bit has an upcut spiral at the tip, transitioning to a downcut spiral 3-6 mm up from the tip. When making a through cut in materials with brittle faces, the bit compresses the two faces toward the core minimising the chance of raising or chipping the faces. They do not offer any advantage for non through cuts, or through cuts in materials not prone to face chipping.
They are generally intended for industrial situations with large high speed CNC's, and are solid carbide, so that the shank diameter is normally the same as cutting diameter, and they are typically made in 1/4, 3/8. and half inch sizes, 3/8 being the most common. The spindles that drive them either use interchangable toolholders with ER collets, or direct mounted ER collet chucks to accommodate the shank size that is odd for conventional routers. I haven't seen a commercial machine run 1/4 comp bits, I suspect because they are not strong enough to cope with the feeds used commercially, and the 1/2 inch units generally are not used because of the waste in nested cuts and the greater volume of chips to be extracted. The only chuck system I know of for hand held or table routers to handle the 3/8 bits would be a Muscle Chuck extension and 3/8th adaptor.
The 3/8th bits are available from industrial tooling suppliers, they were typically $55-60 each a couple of years ago. Sounds dear, but typically last 3-5 weeks on an industrial high speed machine cutting kitchens, faces and panels, forty hours per week.

I just bought this one the other day from McJing Tools On line .. should be here soon in the post . I cut a lot of thin ply so will be interesting to see how it goes.

They are in Yagoona NSW

JR5175

5/32" x 9/16" x 2" x 1/4"Shank

70

$25.00

https://mcjing.com.au/categorybrowse...IRALDOWNCUTBIT

cheers
Peter

Thanks to all who replied, I was only going to use them for cutting plywood ... about 6mm thick on a home made cnc router, but they may be out priced for what is intended,, a little sanding will probably be good enough after cutting out the shape.

Regards

Nick

Naijin, The one thing I didn't mention about compression bits yesterday was that in the 3/8th diameter at least, there are specific bits for specific material depths, this controls the point where the transition from upcut to downcut occurs. The thinnest material that the 3/8 units are specced for is 10mm. At 6mm sheet, the top veneer would be in the transition zone and would suffer tearout and chipping anyway. Obviously you may get the transition lower on the bit in a 1/4 dia bit because the flutes would be smaller, but I haven't dealt with them to enough to comment.

Pedro, I wasn't aware that McJing's supplied compression bits so followed your link. It leads to their section for downcut spirals and the comments section there states that they reduce tearout for the top surface. A compression bit uses upcut at the tip for reduced chipping at the bottom surface, transitioning to downcut for the top surface, so the two shear cuts compress each face toward the core and use the core to back up the cut and minimise face chipping.

We have a Zund G3 Digital Cutter at work, its a 3-axis CNC designed for the signage industry, so fairly light weight work. Along with various drag knives and an oscillating tool we have a 1kW spindle with 3mm and 6mm collets. I was looking into compression bits in order to cut some 19mm melamine sheets but I've just realised that they only work if you're performing a through cut in one hit. I'm concerned that our little spindle doesn't have enough grunt to do this, we often cut 10-20mm thick acrylic & aluminium in 2-4mm increments so as not to overstress it, we're still learning how far we can push it.

But I'm wondering if I can work around this by doing 1 pass with a downcut bit through half the depth, theeby preserving the top laminate. Then changing the tool and doing a second pass through the remaining depth with a upcut bit to protect the bottom laminate? This would be for small one-off jobs, so changing tools and re-zeroing each sheet isn't an issue.

Separate up and downcut bits with 6mm shanks and suitable depths may be easier and cheaper to find than a compression bit anyway. I have found these "Viper" bits from Vortex but not in Aus: http://www.vortextool.com/index.cfm?...category_id=30

Experts, please poke holes in my idea.

cray, you could use the 2 different cutters. it will be time consuming. But one thing you would be advised to do would be to make sure that the downcut spiral bit (the first bit that u use) is either slightly larger diameter than the upcut spiral, or you offset the upcut pass away from the downcut pass by atleast 0.1mm. This will leave a step in the edge face, but it prevents the upcut spiral from being in contact with the already cut edge from the downcut pass. If it does touch the top edge, it will begin to chip it out.

Ideally, if you can do it in 2 passes with your machine, i would find a compression bit with an 8-9mm upcut portion. Look for 8mm, the upcut section should be one diamter in length, though i found often its more like just 10mm or 3/8th inchs as standard...
If you did find a 6mm-8mm upcut section, just make your first cut more than the upcut length which will engage the downcut section of the cutter onto the melamine surface.

Hi cray-,
I commented earlier about compression bits for the original poster, and now will toss a few ideas around for you.

I followed the link to the machine you have access to, and it seems to be an interesting and versatile machine, but possibly underpowered for cutting melamine efficiently. The machine I worked with for three years was a cabinet making machine, 2400 x 1800 table work area, 10HP spindle, 20HP table vacuum system and 10HP dust extractor, 1HP DC servo motors for x and Y axis feeds, and 14 tool tool changer. I know from your post that your machine has a 1HP spindle, and from the web link that it can mount multiple work heads, but do not know what you have as feed motors, or whether you can access multiple router heads.

From using handheld 1200W-2400W routers that there would be no real issues with cutting through melamine in staged cuts, say 1mm depth for pass through the top skin, then 3-4mm steps until you are just above the lower skin. If these passes where done 0.1mm to the waste side, and you could then change to a matched size comp bit, a final pass penetrating through the lower skin and cleaning up the edge left by the multi pass cut. The two limiting factors machine wise would how much grunt the feed motors can safely provide and the dust extraction available.

With such an approach, automatic tool changing is very helpful, but if your machine was able to operate with twin router heads and independent z feeds, it would be reasonably efficient if one head was set up with a down spiral for the initial cuts and a compression for the final cut. Failing that, you would be left left with a tool change and resetting Z zero point to work multi bit.

We used to use our machine in this way often, with a downcut spiral to rough out a cut, then the compression to finish when working with speciality materials, and used to use a diamond roughing bit and compression finishing bit for roughing out 38mm benchtop substrates also, so it not an uncommon approach in industry, but a 5 second tool cycle is a lot more efficient than manually changing cutters and rezeroing the machine for each tool change.

I am not sure how much mel you wish to cut, or how frequently you need to do it, but for a one off it would probably be cheaper to get a custom cutting place to do the job for you.

Thanks both for the suggestions, definitely sounds doable, not ideal, but achievable.

To fill in some of the blanks, no auto tool change but it's a 3-5 min process at best and I'd only be cutting a handful of sheets at a time not running an industrial scale operation. Although it can take 3 different modules at a time, we only have 1 of each type, so can't run dual router spindles.

Not sure about the feed motors, I thought feed rate was more about the material being cut vs. the power and rotational speed of the spindle? It does 50,000 RPM with the smaller balanced tools, down to 20-30,000rpm for the larger 6mm diameter tools. For routing we're usually around 80-150mm/sec, but at full whack with a drag knife it pushes 4000mm/sec. Basically I can push the head around much quicker than the spindle can cut resulting in big trouble.

Dust extraction is provided by a Festool vac plumbed in via gantry, all factory spec, not DIY. It works incredibly well for it's intended usage, easily able to overcome the vacuum table with smaller pieces if you don't put bridges in or reduce suction.

I was hoping to use it for a bunch of personal jobs around the house. Not happy with the lack of accuracy using a skill saw & straight edges on the gatage floor when I'm used to achieving 0.1mm precision at work. We've had a few commercial enquires about cutting melamine, so if I can get work to pay for a couple of tools and write it off as R&D then I can basically use them for personal jobs on my own time. I haven't had much luck finding someone in Perth to cut a few sheets for me, may a well try and make use of the perfectly good tools available to me and retain control of the job. Thanks again for the advice.

Hi Cray
We have a small 700 Watt CNC that takes up to 1/4" bits in ER11 collets.
We use 6 m compression bits from China and except or the price we are very happy with the results on solid wood 10 o 20mm.
From memory they cost about $35 each but they are well worth it. Great for curved work.
Search Aliexpress for up down cutters.

Good Luck
BobT

Thanks Bob, I found a few on Aliexpress, will give them a crack.

Out of curiosity, are you cutting through 19mm laminates in a single pass with your 700 Watt router? If so, at what kind of feed rates?

Cheers

Yep, as everybody else has said there is no such thing as a cheap compression bit, even if you buy in quantity direct from the manufacturer. For hand held or table mounted routers there are very few compression bits available (McJing does have 2 - 1/4" at $42 and 1/2" at $85) without converting to er chuck and collets. If you convert to er you need at least er20 to get back to a conventional 1/2" shank bit and if you want to use the full range of metric CNC bits you have to buy a full set of collets. The all up cost for a home user is not attractive.

There are some options available to use a limited range of metric shank sizes (4,6 & 8mm), but they're not easy to find. I think compression bits are out of the question for most home users.

Originally Posted by cray-

Thanks Bob, I found a few on Aliexpress, will give them a crack.

Out of curiosity, are you cutting through 19mm laminates in a single pass with your 700 Watt router? If so, at what kind of feed rates?

Cheers

Hi Cray
I use the compression bit for solid wood and ply.
I use 6 mm JeeFoo bits at a bit over $20 each delivered.
They give a nice clean edge ie no furry top or bottom edge. A great time saver
As I said we reserve it for curved profile cuts.
I trim the job on the bandsaw to about 3 mm waste then into the machine to shape the job. Speed depends on the wood but it is definitely worth the money.
BTW my router has a Chinese water cooled spindle and takes ER11 collets.
These are cheap US$33.50 for a full set including 1/4" and 1/8".
This allows me to use any bits from 0.8 mm to 1/4", if your not using the metric bits your paying too much.
Just checked and 10 off 3mm two flute spiral bits can be sourced for US$26.34.

Yours
BobT