Compression Bit Details Please Help

[JimFabLabFulton]

Okay, I have tried many different cuts with the standard up and down cut bits like the ONSRUD 57-910 running at 14000 rpm and 3 ips.

I am running a prs alpha with a 5hp columbo spindle. Cutting 3/4 double sided pre uv finshed birch, maple or oak.

I see lots of guys talk about compression bits and after reading about 20 threads I have this question.

I want to use an onsrud bit.
Can someone give me the bit number they are using, the feed and speed and number of passes?

SPEED is not as important as finish.

[jTr]

Though I've disregarded your specific request for an Onsrud part#, might I suggest the Centurian brand. Very economically priced, rapid delivery time and fantastic, clean cuts:

https://www.centuriontools.com/router-bits-toolcase/solid-carbide-wood-router-bits.html?sku=14CR21.03&pcn=Compression%20Routers&pid=791&sat=1

I run 12,000 rpm 4.5 - 5 inches per second.

Note that this is a plunge bit - they also show a mortise style with a flat tip. For plywood, the plunge is what you want.

Be careful to adjust your depth of cut when using any brand of compression bit- the first .25 -.30" of the tip is upcut, so you'll want to bury it just enough to avoid tear out,- set first step to ~.35 and you'll be clean cutting on both faces of your sheet goods.

Jeff

[jTr]

I run two tool paths for a total of 3 passes:
1>.35, .60 CLIMB cut
2> .752 conventional cut, single full depth pass on second tool path

Bit will deflect a couple thousandths on the first two climb cuts. Final full depth pass cleans up any witness lines or "step" effect - shaves things off for a superior edge finish on any plywood.

jeff

[dlcw]

I have a 2009 60x96 PRS Alpha with 2.2HP spindle.

I have used a couple of brands of compression bits. I've gotten similar results from all of them. The one thing I did learn is, don't bother resharpening them. Not worth the money. Not as sharp as factory sharp and you will get about half the number of sheets from a resharpened bit.

I use a 1/4" bit on 3/4" plywood (11K RPM at 300 IPM). I make a climb pass first, leaving a 1/32" skin. I then make a conventional final pass going through the material by 1/32". Parts come off the CNC ready for the edgebander (other then cleaning off any dust).

I used a 3/8" bit for a few years and switched to a 1/4" and have not had a problem with breaking bits. The one thing I noticed is I get less part movement with a 1/4" bit versus a 3/8" bit. Not sure why....

I found I can cut between 25-30 sheets of REAL plywood per bit. When cutting melamine I use a bit designed for that material and I can get 25-30 sheets with the melamine bit.

If you are using Aspire or a program like it to design and create your toolpaths, you will need to plunge at least 3/16" before you start ramping down for your cut. The bottom, of the bit is up spiral. If you start your ramp from the surface you will get a bunch of chip out on your veneer. I use eCabinets for all my cabinet work and the Shopbot Link gives me the option to plunge before ramping. Very nice.

As far as bits, I have used Centurian, Onsrud, R&B Tool Supply and, like I said, have been happy with the results from all of them.

[garyb]

Recommend double flute over single for your aplication
60-113 Double flute Compression use chipload of .014
400ipm @ 14000rpm
340ipm @ 12000rpm
Gary

[BTP]

On my standard. prefinished birch is actually the slowest cut i ever cut.

3 passes.
14 rpm 2.9 IPS

.38 first pass
.15 the last pass.

[Bob Eustace]

Totally aggree with Jeff, Jim. Centurion are terrific and consistent bits and the most economical one can buy.

[JimFabLabFulton]

okay i just got some onsrud 60-124 3/8 double flute compressions


my plan is to try 3 ips @ 15000 ( chip load .006 suggested chip load between 0.16 - 0.180) first cut 2 passes first at .4 second at .72

I have a 5hp spindle so power should not be an issue


suggestions

[Ger21]

You'll burn it up at 3ips, imo. We have an industrial Morbidelli router at work, and with 3/8" compressions bits, we cut at about 12ips (700+ipm) full depth, at about 17,000 rpm.

[dlcw]

Jim,

When I cut plywood, my 2.2HP spindle with a 1/4" compression cuts at about 6ips at 11,000 RPM, two passes. One pass in a climb cut leaving a 1/32" skin. Second pass, 1/32" through the material, is a conventional cut. With a 3/8" compression, I cut at 6ips at 10,000 RPM, with the two pass method.

Depending on the quality of the plywood, I can go from CNC to edgebander without any sanding. Just clean off any dust. Some plywoods I have used, tend to be more ragged on the edges requiring a sanding block with 100 grit paper to make them ready for banding.

Yes, at 3ips you will burn up the bits. Doesn't matter who makes them.

One thing I struggled with when I started with the CNC was the whole concept of feed speed. On a router table, you tend to feed more slowly. On a CNC you can feed much more aggressively. I started with feed speeds around 2ips to 3ips thinking I was going to fast. But a former Shopbot owner corrected me and told me his feed speeds and I about fell out of my chair. What I learned was crank it up. If your hold down system will take it, run at a feed rate, at the correct spindle speed, that gives you good chip load. Slow feed is not better and won't give you a better quality cut. It just burns up bits. After cutting a sheet of parts, I can grab my bits, when removing them from the spindle (yes, the spindle is turned off :D), and they are barely warm to the touch. Room temperature is about the temperature of them.

[Brady Watson]

If your hold down system will take it, run at a feed rate, at the correct spindle speed, that gives you good chip load.

That point should be stressed & it should also be noted that if you have a Standard machine, it is possible to lose position by pushing the tool too hard.

-B

[JimFabLabFulton]

Thank you for the tips, it sounds like I need to bump up the feed rates

if I run 10 ips at 17000 that gives me a chip load of .017

so I think I will start there

[JimFabLabFulton]

Thank you for the tips, it sounds like I need to bump up the feed rates

if I run 10 ips at 17000 that gives me a chip load of .017

so I think I will start there


Quick follow up.

Okay a onsrud 60-124 3/8 double flute compression on cherry, birch prefinished plywood .72 inches thick

14k at 400 ipm .5 in first pass cuts very well, nice clean edges that do not need sanding