CNC Bit Life in Baltic Birch
Eating up carbide fast and want to look at Diamond. Hope to keep the tool off the shelf. Right now, the 3/4" I take 3 passes to cut through and 2 passes on the 1/2". This is mostly because the tool becomes dull fast where the glue in the plywood is, but birch is also pretty tough. (Cutting edge becomes serrated.)
Looking at bits like the Amana DRB-200 or Freud 78-116. Any experience out there? Can you plunge with these bits? Will they last? Any other options? I do not really need the compression technology. I have used custom diamond profile bits in the past with good results on MDF, but no real experience with straight cutting plywood. I hope to use one cutter for all the material and do need to plunge the 3/4" material.
From contributor M:
Can you speed up your IPM? Those bits must be as black as coal after a few passes. I cut 12mm BB all day using a 1/4" solid carbide 2 flute compression spiral with a mortise tip with 18500rpm at 700IPM+ -. I ramp all start points and can average anywhere from 40 sheets to 100+ sheets per bit before it starts to get fuzz. I also use a 3/8 bit with the same configuration as above and it does as good and better than the 1/4". I do run the 3/8" bit at around 750IPM. I like the 3/8" bit because it makes it easier to clean when I do not have to have 1/4" slots or an inside radius of .125". I have not used a PCD on BB because they only come in 1/2" or bigger and I need the above specs for 80% of our work with BB but use it all day on MDF core melamine. It averages around 150 to 275 sheets per bit.
Contributor G has some good bits and I have thought about insert, but as I mentioned above, they also do not come in less than 1/2" as of the last time I checked at IWF. I heard some were trying to get a 3/8" bit both insert and PCD, but that is a skinny shank to cut away that much meat and have it not bend or break.
I have tried Courmatt, Vortex viper, I think it's Whiteside, Amamna, Onsrud, and several others but right now I am using Atlantic. Fair price and great service. He actually comes by every other week with tooling in his SUV, so I get it on location with no extra shipping costs or delays.
From contributor O:
I have cut quite a bit of Baltic birch ply as well and feel your pain about killing carbide cutters in a hurry, so many hard glue lines. When I can (when I don't need a small radius in the corners), I use a diamond bit from Royce/ayr. It's one of their eco-spark series tools. I run it at 18000 rpm 12-16 meters/minute. It will leave a perfect cut on the top edge (and bottom if you are through cutting).
We cut a lot of different materials and do a lot of different types of work, so it's hard to get an accurate sheet count per tool, but that tool will last 6-8 weeks running one shift.
From contributor T:
Can you feed faster than 100 to 200 IPM? I think you may be feeding way too slowly. If you cannot speed up your feed or slow down your RPM's, then you might try using single flute router bits. Run them at 200 IPM which is almost their recommended speed.
If you can feed faster, you might try starting your feed speed at about 350 IPM for a two flute bit and slowly increase the feed rate until you get a bad cut. Then reduce the feed to just below this point to get the optimal speed for your tool.
Carbide can break down due to excessive heat and running a tool too slowly can generate a great deal of heat. If you follow the above instructions, I believe that you will see an increase in your tool life.
From contributor L:
Is there any way you could mount a VFD somewhere close and get control of your rpm's?
From the original questioner:
This is an older CNC machine and there is no easy way to control the RPM. My programs call out for 300 IPM, but then I usually have to run at 30-50% to keep from bogging down the motor. If I increase the speed, the motor just bogs down more and more.
We usually only cut 3/8" MDF on this machine, so the BB is a new venture. With a new tool, I start high and then reduce it as the tool wears, but we are talking one day here.
I also am only taking max depth cuts of 3/8". I have to step my cuts because going all at once will either stall the motor or break the piece free from the vacuum table.
Contributor T, can you explain to my why a single flute would help out? Seems like it would only increase the load on the cutter since there is only half the cutting edges.
From contributor T:
Based on your feed rates, a single flute tool is correct for chip load. Proper chip load for your application is about 0.0125". This is not an exact science, as wood densities and contents vary. Use this as a starting point to adjust from. All calculations are based on a 1/4" diameter bit. For larger diameters, increase the feed rate.
Feed rate = RPM x Number Flutes x chipload
A single flute bit only has one cutting edge, causing drag through the cutting area. This will reduce heat since the friction developed by the tool will be half. My main reason to recommend the single flute tool was your limited feed rate ability. A double flute tool will spend too much time in the cutting area and generate a great deal of heat. This will cause a premature break down of the bit's cutting edges and a shorter tool life. You should always feed as fast as is possible for the application, as it will improve tool life and even cut quality.
Now about the bogging down of your machine. Contributor L has a good idea. You should address your spindle speed. If you keep your RPM's consistent throughout the cut, you may improve tool life and overall operation of your machine. I have heard of some people replacing the motors on their machines or using PWM (Pulse Width Modulation) systems. A PWM system will allow you to adjust the spindle speeds almost infinitely and when the system senses bogging, it increases the power to keep the RPM's the same. By lowering the RPM's, you can run at the lower feed rates and use multi flute tools.
From contributor C:
That is very slow. If you heat diamond up, the diamond will release from the carbide and fall out.
The comments below were added after this Forum discussion was archived as a Knowledge Base article (add your comment).
Comment from the original questioner:
Would you like to add information to this article?
Interested in writing or submitting an article?
Have a question about this article?
Have you reviewed the related Knowledge Base areas below?