I want to cut a shape out of a board that is 3/4" thick. I am considering a compression bit to do this. Let’s say for example this one:
My small understanding is that the initial cut has to go deep enough to get past the 7/32" tip of the bit (which is upcut) to be effective at reducing tearout.
How do I set that up? Do I make my depth of pass 7/32" (roughly 5.6mm), that seems like a LOT. I guess I’m not sure how to properly use it
That’s my understanding as well. The 1st pass has to be at least 1x the diameter.
Yep, that’s exactly right. I use 1/4" and 1/8" Jenny bits (https://www.cadencemfgdesign.com/product-page/the-jenny-bit-8675309) and set my cut depth to either bit diameter or more. On the SP5 and 1200W VFD spindle, I have no problem with this cut depth. You can experiment with scrap and it pays to do so as you can generally cut a lot deeper per pass (for roughing/etc) than the defaults, but it does require being cautious and changing settings progressively if you want to avoid accidents.
Zillion edits, but I checked the specs, the 1/4" Jenny bit has a transition at 0.070", so you don’t need to go full bit depth with their bits.
Yes, for this bit you are correct. This much upcut section might be too much for Shapeoko class machines - this bit is likely for larger, more rigid, more powerful machines.
I have had good luck with bits that are specifically designed for smaller machines. The ‘Jenny’ compression bits have very short upcut sections, and I have used them successfully in both hardwoods and softwoods.
I have also had good success with the ‘Groovee Jennies’ - V Bits with a downshear geometry.
Compression bits are designed to make full depth cuts so you have an upcut at the bottom of the bit and a downcut at the top and the center is there to remove material. Unless you have a CNC powerful enough to make a full depth cut the compression bit is useless. It cuts like any other bit but the its function is lost without the full depth cut the bit was designed for.
A compression bit works just fine in multiple passes, just so long as you are deep enough to pass the upcut section.
I get all the benefits of an compression bit in 3/4" stock, using 1/8" passes.
3/4" is what I’m looking at operating with. I think that’s the info I needed to at least get me to try it, thanks.
While a full depth cut takes the pass depth out of the equation it is not required for compression bits. I use plenty of them, you just need the first pass to be deep enough to engage the downcut portion of the bit, the diameter has no relation to it. As an eample I have .25" bits with a .1" upcut so a .125" first pass takes full advantage of the compression, which is half the bit diameter for that one. If you pay attention when you order bits you can avoid ones with high upcuts, which would need correspondingly deeper passes.
Something to keep in mind is that they need to be run slower than upcuts, more in the range of downcut speeds. And deep slotting is challenging when the bit starts as, like a downcut, it has no way to excavate the chips. If you can start it off material instead of ramping or plunging in it helps. They really shine running contour finish passes as excavation isn’t a problem and deeper depths aren’t as big a concern.
It’s also worth noting that if you take roughing passes first you can then take a full depth finishing pass with minimal width of cut (stepover) with the compression bit and therefore get the clean edges they deliver top and bottom.
I fairly regularly use an older upcut bit to make the majority of the cut but with 1mm or so of stock remaining (depends on the material), and then swap over to my nice sharp finishing compression cutters to make the final cuts at full depth with 0.5mm stepover to get that really clean edge.
Wait am I the only person with a 5 pro that will take deep cuts? I will run a 1/4" compression bit at 1.5D 3/8 DoC. Don’t be afraid to try things out what’s the worst that happens, you stall or in the case of a 1/8 bit maybe break it but doubtful unless there is something else wrong. I’ve seen this thing take a 3/4 doc (definitely didn’t like it but it made it 2 inches before I hit the Estop [faulty controller board that got warrantied])
I also do full-depth (usually 3/4") contour cuts on plywood with my 5 Pro and the only problem I get is some burning at the plunge location. I usually use 1/8" compression bits though since they are cheaper and I imagine that the heat from these cuts aren’t great for bit sharpness. I add one cleanup pass to account for bit deflection.
I can tell you this, I am not impressed for the money in the Amana bits. I know that is not your question here but there are cheaper bits like 1/2 to 1/4 the cost of these bits that do just fine. I like the 1/4" shank so I don’t have to keep changing out my collets and I can use just one size. SpeTool is a nice bit and I also use Sharpro and most of all my bits I use compression bits now. Also, you are on the right track here, with these bits you have to cut a little deeper but especially if you have spindle on a SP 5 then you will be good to go. I run my bits a little higher speed where some people run them too slow. The Sharpro came with some nice charts to show how to make the calculations.
Oh and i also tried the XDENGP bits they are ok I have some of them 1/4" and they scream a bit lol but they work ok for the price.
The one bit I was not impressed with were the EANOSIC, they are cheaper but they are pushing their limits.
However, I did the math for the price of one Amana bit as comparing to some of these other bits. I can buy 3 bits sometimes 4 for the price of one Amana bit. The Amana bit does last a little longer than the cheaper bits I listed here but gathering them all up I save a lot more down the road.
So on these compression bits, you do have to go past the spiral so when I am cutting with a 1/4" bit I start my first cut at .125in, through MDF and Baltic Birch and I have no tare out. Like I said I like to run my spindle a little higher than what the charts say on Plywood and I find I get nice smooth cuts. I am talking they are so smooth I barely had to sand. I was going to do some videos on this but I just had not gotten the time.
Ramping is great for this.\
Also for bits SPETOOL really does make a decent quality for your buck and goes on sale pretty often. Even for aluminum I can pick up 5 .25" O-flute bits for 45$ CAD after tax on sale
Ah yes…ramping…I just couldn’t bring myself to pay for Carbide Create Pro to get ramping so I just usually make lead in/outs manually in the free version or do it in FreeCAD…neither is ideal so I’m playing around with SOLIDWORKS since that’s what the Mech Engineers use at work and I can pick their brains.
I also use solidworks but the cam is so unintuitive. Have you looked into mastercam?
Not really…the allure of people at work available to help me is hard to beat. Plus they have a maker version that’s only 48USD/year.
I generally go .25 in DoC for 1/4 and 1/8 inch bits at 150-200ipm. Stalls do happen in hardwood at these speeds when cutting at 100% stepover.
But I do notice a lot of people are babying their machines and likely wearing out their bits a lot faster than needed.
Yeah I’m seeing that, to a degree I mean im currently observing the harmonics of center drillings 2300 .08" pilot holes and the rigidity of the machine and harmonics of the workpeice arent as simple as i thought. additionally the homing cycle issues being not the same every time are just the worst. I wish ida known before i started a project this costly and large
I have noticed slight variances in XY between power cycles. I assume that quick actions to reposition wouldn’t solve that either since those would be impacted by those variances as well.
Some time back I read a post where from someone indicating that they would use the machine to drill a small hole at the start of a job. Then later if they had to initialize they would mount the drill bit and manually jog to the hole and then rezero.
That is a bit of a fringe case but would work sometimes. youd probably want to mill a hole and use a locating pin because if youre worried about precision might want to be precise