Question
I'm looking for tooling suggestions for cutting 1/2" and 3/4" Baltic birch (5'x5' Russian BB). Also cutting 1/8" hardboard and 1/4" MDF. ~20,000 RPM @~100-200 IPM. (I can not change my RPM - older machine.) I'm cutting both profiles and pockets all using the same cutter.
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.
Forum Responses
(CNC Forum)
From contributor G:
Going that slow may work with a PCD tool. Forget solid carbide, as the tool would need slower rpm's. Our PCD tool has a plunge point, so it can plunge, but if you can ramp, that's the best solution. An insert tool may also come into play.
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.
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.
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.
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.
Feed rate = RPM x Number Flutes x chipload
Feed rate = 20,000 x 1 x 0.0125"
Feed rate = 250 IPM
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.
Comment from the original questioner:
Thought I would give an update since I went ahead with the Freud 78-116 bits once I started this thread. For the money the bits have lasted me a long time. I only cut every 3-5 months and probably 15 sheets of birch mixed in with MDF and harboard but they have done well for the price. I did get build-up on the back side of the bit. It was probably glue from the plywood but I did not notice excessive heat or any other issues. I now need to add a plunge tip to this style bit.
