Compression bit selection

[Aerojunkie]

I have been searching on here and centurion cutters seem to be very poplular. I want to try some just cant decide on the plunge end or the FEM(flat end mill) end. Any suggestions? I have been using whiteside 1/4" compression bits in my 2.2kw spindle so far but want some 3/8" cutters.

On a side note what would be a suggested feed/rpm, cut depth for a 2.2kw spindle on a machine similar to a prt standard? Its actually a cnc routerparts pro with nema 34s and an atc spindle. Right now I can run a single pass in 3/4" maple plywood at 350ipm and 13,500rpm with the 1/4" compression. I want the 3/8" for a better edge finish.

[EricSchimel]

I use those same bits and I really like them. Do one pass like you're doing now, but leave an onion skin and make the part about .005 larger (you can do this in Aspire). For the last pass come in the opposite direction and tight to the part (no offset) and you'll get great finish quality on plywood.

[jTr]

Point #1 Having plunge end is in harmony with the plunging of the bit into material. Unless you ramp your cuts, Flat end mill will be stabbing straight into material, heating faster and hastening it's demise. Centurion refers to this geometry as a mortise compression bit.

Point #2 - What Eric said, though I recently switched to 3/8 for general plywood cutting, simply to reduce number of passes. On a 4x8 sheet full of cutouts, this makes a noticeable reduction in processing time. As for better edge finish, I think you'll find as I did that the difference is not very perceptible. Others will note 1/4 bit allows you to squeeze more parts on each sheet. I've not had any such problems since up-sizing to 3/8, though sometimes that 1/8" wider kerf can add up.

As for brand, I've been happy with Centurion, especially with pricing. Recently purchased a 3/8 of theirs and equivalent in Onsrud, and they appear almost identical. Time will tell if any difference in longevity, though they are both the "extended" / "Max Wear" varieties. Note part numbers in image.

Pay attention to length of up-cut tip on your compression bits. Image shows a regular 3/8 compression at the bottom, with the Onsrud and Centurion above. Note the top two have half the length of up-cut tip. This is ideal for plywood, as you're less likely to plunge too shallow, resulting in tear-out of veneer , or worse yet, melamine face.

33260


Jeff

[dlcw]

A very important thing to consider with compression bits is that the upcut portion will cause chipout until it gets below the surface of the plywood. Because of this, you need to plunge a compression below the depth of the upcut portion then start your ramp. I've worked with 3/8" and 1/4" compression bits. I cut hundreds of sheets of plywood a year. The 1/4" does allow more parts per sheet, but at the cost of speed. You can run faster with a 3/8" bit because there is less bit flex. But, if your machine is not REALLY tight, the 3/8" bit can cause more machine flex. I compensate for this with 1/4" bits by making my first pass a climb leaving a 1.32" skin. The second pass is a normal direction cut. I plunge the bit 1/4" down then ramp all the way thru the material cutting 1/32" thru. This leaves a very clean edge ready to go straight to the edgebanding machine and the second cut is dead on the line.

[Brady Watson]

The best, of the best, of the best (https://youtu.be/OXRi28W-ENY?t=62), sir...yanno...with honors: ---> Vortex <--- (https://www.vortextool.com/wood-tooling/compression/series-3100xp-two-flute-xtreme-performance-compression-spirals.html)

[EricSchimel]

Brady, how much better are those than something like a Onsrud, Whiteside or a Centurion? I tend to get a long life out of my Whiteside compressions... Is it just the time that they last, or is the cut quality that much better?

[dlcw]

I've been using RBTools compression bits for several years. I went from getting 20 sheets of 3/4" plywood to 25 sheets before I had to change bits. I also went from 5IPS to 6IPS with the same cut quality. The tool seems to last longer then others I've tried (Onsrud, Centurian, Whiteside, Amana). The cut quality is VERY good over the course of 25 sheets. After that, it starts to degrade a little. I donate my "duller" bits to the local highschool woodshop for two reasons, one, the kids are very hard on these bits and drop them on the concrete floor and slam them into screws and nails. Two, at the rate they butcher bits, giving them my used bits saves them a LOT of money. I do the same with 1/4" two-flute down cut spiral bits. I use lots of these bits too.

[Brady Watson]

The Vortex bits give a cleaner edge and last about 3x longer than the Centurion ones in my testing. If you crunch the numbers, they are a little bit cheaper if you gauge the linear cutting distances of each...but let's not forget that the edge quality is better, regardless of life.

A friend of mine with a Thermwood recommended them years ago and his machine, being a real CNC (aka not bolt together aluminum), can blaze through material with the Vortex bits - way faster than an Alpha with 5hp spindle could. I was only able to average about 60-70 sheets max. He could get in the neighborhood of 90 sheets on his machine since it doesn't flex, bog and can run a heavier chipload - which means the bit stays cooler and isn't rubbing more than it has to.

For most people, the Centurion ones are fine...they are a good bit for the price. Like any consumable...find something that works well for YOU and your material...and stop buying your tools from Ebay, Amazon and TToday. You'll get better tools and pricing from a tool dealer you establish a relationship with. That message is for the professionals...who probably already know that. If you are a hobbiest - it doesn't matter because you aren't really building tooling costs into a paying job. Just as a yardstick...TToday had an Amana bit for $137.00...my dealer's price for the same bit was $87. Do the math. That's money back in your pocket.

[Aerojunkie]

Thanks for all the info. Right now the vortex cutters are a little bit steep for this machine, but when I outgrow this one Ill be into a lot heavier machine and then new level of tooling to match it. Tempting to try a couple right now though and see how they last under my conditions. All I have been using is the plunge style cutters so far, any issue plunging a flat end mill style around 1/4" before ramping to depth? Or should they be ramped in the entire way? Cutting maple veneer plywood for cabinet parts, no melamine.

[woodshop]

We cut 3/4" plywood with 1/2" straight fluted bits from Lowes ($17 each).
We ramp with 5 passes at 60 ipm and 16k rpm.
Great results!
We are not creating edges which require superior finished cuts. More like rough cutting.

[woodshop]

We cut 3/4" plywood with 1/2" straight fluted bits from Lowes ($17 each).
We ramp with 5 passes at 60 ipm and 16k rpm.
Great results!
We are not creating edges which require superior finished cuts. More like rough cutting.

[Kyle Stapleton]

Not to get off topic but what cnc are you running because you numbers sound way off.
We run cheap cmt 1/4" downcuts (kids brake them to often to buy anything better) @ 4 ips with 2 passes 12000 rpms, and get nice edges.
So 1/2" straight fluted bits for 5 passes at 60 ipm and 16k rpm seems really odd.

[woodshop]

ipm (inches per minute)

Pretty darn fast (IMHO).
Shopbot Desktop with router.

We go through 10 sheets of 3/4" ply every month.

[Kyle Stapleton]

Desktop... that is still a little off.
Try a down cut 1/4" 2ips (180 ipm) @ 12000 rmps 3 or 4 passes. (This is what we use on our desktop)

[woodshop]

180 ipm is too fast for our comfort level.
Don't want to tear up a $6k machine.
Anything we cut in our shop ranges between 60-75 ipm's.
We bid our jobs at 60 ipm's.

[EricSchimel]

I agree with Kyle, that's far too slow. You're leaving time on the table. 2-2.5ips is fine for a Desktop. You won't tear up that machine at all. If you cut too fast (which 2ips isn't even close to too fast) at worst you'll just stall the steppers. No damage will happen to the machine.

[robtown]

I agree with Kyle, that's far too slow. You're leaving time on the table. 2-2.5ips is fine for a Desktop. You won't tear up that machine at all. If you cut too fast (which 2ips isn't even close to too fast) at worst you'll just stall the steppers. No damage will happen to the machine.
60ipm = 1 inch per second x 5 passes
That's a glacial pace.
You should easily be able to cut at 160-180ipm at 3-4 passes with those big box straight flute cutters. I do it on my older PRT with a PC router with no issues.
I'd at least consider going to 100-120ipm (approx 1.7-2 inches per second) and cut it 4 passes.
You will not tear up your machine, and you'll double your output (or better)

[woodshop]

We get paid well at 60 ipm. (We see no economic benefit to going any faster than that.)

We are cutting hard wood layered together with exterior grade glues using a half-inch cutter. (Hard wood, hard glue, big swath.)

We hate those hidden surprises in today's sheet goods... knots!

We don't need unsafe speeds in our shop or with our expensive equipment.

In all honesty, we have learned that we don't need those higher feed rates to make money and being SAFE is extremely ECONOMICAL.

[EricSchimel]

You can go faster safely, and if you do your bits will likely last longer so there's your economic benefit! :) . I often bid my production jobs at lower speeds and then as I get more experienced with the job/material I'm able to push feeds and speeds. That allows for a cushion of down time, and also has allowed me to re-invest in my shop and equipment.

[woodshop]

ok, we'll give it a shot. Maybe try 100 ipm today. Thanks.

[woodshop]

We doubled our feed speed to 120 ipm.
That saves 1.7 minutes cutting time per piece.
That's a saving of 30.6 minutes per 4x8 sheet.

Maybe we can double the life of our $17 bit?
If we can do that, we will find another savings of $8.

In all honesty, I think we can kick up the feed speed to 180 ipm safely.

Thanks, gentlemen.

[EricSchimel]

Another time saving method changing rapids to be a bit faster, and looking carefully at the travel moves. Those are pretty simple to see visually in Vectric, but the one that people overlook a lot is the ramping. I'm not sure what you're cutting, but if it's anything with a fair amount of detail you can dial in the ramping so the machine is a little more "snappy".

If you have tight corners and that sort of thing, you can reduce the time that the machine "hangs out" in those corners so it won't burn up the bit as much (or if you're using spirals it'll squeak less). If you have a lot of Z moves you can make that a bit snappier to. You don't want the machine "jerking" back and forth, but just a little snappier.

http://www.shopbotblog.com/2008/03/a-ramping-the-vr-command-and-how-to-tune-your-tool-for-maximum-performance/

[erniek]

I like to use 1/4" compression bits on my PRT. Cutting speed I use is 4-4.5 IPS with at 10800 rpm. I'm sure it the bits could be faster on an alpha machine but any faster and I'm risking losing positions. I used to spin them faster but find that they last longer at a lower speed. I use 2 flute cutters on melamine and 1 flute cutters on plywood. I use a two pass system where the first pass is the full depth less .03" in the climb cut mode then the second pass in conventional direction. Dont think a PRT or PRS would be able to go faster with a 3/8" bit. The 1 flute cutter can cut faster though.