Improving Bit Life and Performance Cutting Melamine on the CNC

This discussion of bit choices and characteristics also delves into how you can fine-tune your operational settings to suit the machine as well as the material and the tooling. March 13, 2014

I have been using a 3/8" mortise compression spiral. I am getting packing of chips in the kerf and therefore low bit life. I want to try a spiral bit with much more of an up-cut. Onsrud has one with .6" up-cut but it is a 1/2" bit. I know I can run faster with 1/2" but will I see more bit life for the extra dollars. All things being equal, does a 1/2" bit get better life than a 3/8"? I am cutting on a Rover 30 with a 10 hp dust collector. The Rover has such a big dust shroud I don't think it helps much in evacuating the chips.

Forum Responses
(CNC Forum)
From contributor M:
Take a look at the Vortex 3130XP. I am routinely getting 75 plus densely packed sheets of melamine with it. It would likely be a lot more if I did not have to switch to other materials occasionally in between runs of melamine. I switched a few years ago from Onsrud for exactly what you are describing. The extra upcut with this 3/8 tool is key for chip evacuation. The website does not list the upcut specifically, but it is much more than the Onsrud.

From contributor C:
Rover 30 and 3130xp Vortex user too. I was using someone else also and I get about 45-60 sheets with the xp and that is with melamine and double laminate sheets.

I went to a 15 hp collector. Getting ready to buy a RCN collet from BVC. Also, are you sure your port is shutting off for the drilling block? This might help, and I really don't think a 10 hp has the oomph to get over the monstrous shoe that is on the 30.

From contributor H:
The 1/2" bit will get you a little better life but you will be able to run a higher feed rate as well.

From contributor J:
Vortex 3184xp. Nested 4x8 sheets cutting 80% 3/4 mel 20% 1/4" mdf, I get over 200 sheets between tool changes. Over double what I have gotten from Onsrud (I have not tried the Marathon bits however).

From the original questioner:
What feed speeds and rpms are you Vortex guys running? I assume you're cutting in one pass?

From contributor J:
Yes, one pass for all but small parts. I run 2 flute, 18k rpm, 600ipm. I could push faster but it does not seem to gain me anything more than a few seconds on cycle time, which is not a big concern, as my operator does other things while the CNC is running, so it does not really affect my total throughput if a sheet takes 10 min to cut or 15 min. It only takes about 60 seconds between sheets to clear and sweep the table, load and press go again. There are other processes that are a constraint in my total throughput, but the CNC is not one of them.

On some of the bigger machines I ran a similar 3/8 tool at 900 ipm, even faster when it was sharp (Onsrud MW series 60-126 I think it was?). But had to watch for throwing parts more. Operator had to stay at the machine and still not the tool life I have now by any stretch.

I am cutting a nest of fairly regular sized cabinet and drawer system parts, not just a few large closet ends.

From contributor M:
2 flute Vortex 3130 xp 720 IPM 18K RPM.

Like contributor J, I am not concerned with cycle time overall. I onion skin all perimeter cuts not so much for holding power (although small parts need this), but for improved chip evacuation. Climb cut the first pass, conventional the second, parts come out perfectly sized and the kerf is pretty clean.

You could also choose a 3 flute at 1000 IPM and 16KRPM, but unless you have a really quick machine out of the corners the 2 flute is a better choice overall.

From the original questioner:
That is interesting. I used to use the same cutting method on the Shopbot. For me it was mainly because I had a weak vacuum.

When you say chip evacuation, do you mean cleaning the kerf after the 2nd pass? I am now cutting most parts in one pass. Chip evacuation might be one of my issues. I am using a RCN fan collet. Where the tool path is shared with another part we have a totally clean kerf. Only on the outside parts at end of a sheet are there any chips in the kerf. But those chips are packed really tight on the bottom.

I am running pretty much the same chip loads both of you are. I have tried cutting back at the speeds. I wonder if the climb cut, then conventional is somehow easier on the bit?

We are doing wholesale closet parts, so really would like to cut at the highest speed possible. Things are really starting to pick up here.

Would you consider a Biesse Rover 30 fast enough out of the corners to use a 3 flute bit? I might be able to accept a production rate at 1000 IPM in 2 passes? I might be able run at 1200 IPM on the 2nd pass. It would take me a bit to rewrite the post processor to this on non-square parts but might be worth it in the long run.

From contributor M:
For chip evacuation I do mean that it cleans out the kerf on the second pass as well as releasing the onion skin.

The passing first in climb is best for me since it biases all of the accumulated deflections away from the part while under load in climb. Then the light pass conventional trims the part very true. If I do both passes in the same direction I sometimes find a very slight lip on the parts after the second pass is complete. It took a while to figure this out and it may be machine dependent. What works for me may not work for you. All other things being equal, if I could achieve good results with 2 conventional passes, I would do that.

As far as the Biesse Rover getting out of the corners, I suspect not, and you may be best sticking with a 2 flute bit. To be certain you would need the acceleration curve for that machine. (Good luck getting that information from the manufacturer - I found it impossible.)

The reason I suspect the Biesse would be slow out of the corners is that it, like my Holz-Her, is a high quality overarm machine, sturdily built and durable. It carries a drill bank, tool carousel and lots of mass, especially on its x axis. Best I can tell it takes about 20 inches to reach 1600 IPM in the x direction, all the while spinning at constant 18KRPM. In the corners the 3 flute just gets too hot and wears prematurely. I wish it were possible to control the rotation speed in relation to the travel speed, but few controllers allow for this not to mention effects on the spindle.

In the end I have heard great things on the RCN and if I had one I would very likely do as you already do, single pass the large parts and only onion skin the small ones. For now, cycle times are not a great concern for me and I will sit pat with what I am doing.

From contributor J:
Contributor M has hinted at it, but each machine is different in how it deals with acceleration from corners. Some of it is physics, some is software and controller hardware/firmware, some is machine construction, weight, Z plate, all kinds of variables. The post needs to be able to take use any advantages your machine may offer as well. Several years ago I ran a Komo 5x8 Mach2, and a huge Northwood 5x12 (single table). Both had the moving table in the long axis. In cutting 5x8 3/4" melamine I could push the Komo at ~1200ipm through just about the whole bit life (3/8 mortise comp Onsrud; I think it may have been 3 flute but I may have changed to 2 flute by that time, I don't remember for sure now, but it was the same on both machines at that time). But to push the Northwood that hard, did not do as well, I'd bog the spindle down really bad and even snap the tool sometimes. I know they had different spindle motors (same Hp) with different power bands, but this should have been a sweet spot for both, but the Komo just did it where the NW, not as well. So I just set the NW at 950ipm and no big deal. I am not stating this as an endorsement for Komo over NW, but to highlight how each machine really is its own animal and you need to set things up accordingly (often by much trial and error for fine tuning and optimum performance).

I question the need to worry about chip extraction so much while cutting. I have my machine run a very short sweeping routine as soon as it pushes the cut sheet off the table. Then the next sheet is slid on and hit go while my operator moves parts to the next process (usually edgebanding) without the need for an intermediate storage step. I have a little dust at the edge of my machine, simply sweep over to the floor sweep every so often, but no airborne dust.

From the original questioner:
The reason for my concern about chip extraction is that with chips packed so tightly behind the bit, it does not allow the bit to throw off heat. I used to be able to touch the bit immediately after cutting on my ShopBot. Not with the Bessie at the same chip-load, even if I slow it down to the same speed I was running on the ShopBot. Not necessarily the issue, but one of the things I am looking at.

From contributor J:
Interesting. I guess with getting the type of bit life I do, and that I don't get a burnt end on the tool, I figure I am about where I should be. I may try touching it next time just out of curiosity. Because it is heat that degrades a carbide tool like this faster than anything else.

From contributor L:
I have only had my machine for 1.5 years now, but I recently achieved over 200 5/8 melamine sheets. This was with some 3/4 and MDF mixed in.

Basically you need to check how hot your tool gets while cutting. If the tool is too hot (can't touch for more than a second), you need to either speed up the tool or slow down your rotation. I am currently running 25 metres per minute with 16000 rpm on my Biesse skill.

From the original questioner:
What size bit and how many flutes?

From contributor L:
3/8 2 flute compression.