Stepdown for 1/8" Compression Bit

Hello everyone!

I have a 2 part questions I am hoping the community can help me with before I end up breaking the brand new bit I just purchased. The bit is an Amana 1/8" Long Reach Compression Bit (#46176). Amana website shows the B1 dimension as 7/32.

With this information I am setting up my CAM for cutting out an item in 3/4 inch plywood (radiata pine right now for testing, eventually will be transitioning to baltic birch). My questions is, to take advantage of the compression bit, and allow the downcut portion to act on the top face of the plywood on a contour pass, it seems like i will need to make a 0.25" DOC with this bit so the bit will engage the downcut flutes on the top layer.

Does anyone have experience taking such a deep cut with contour cuts (full width of cut) with a 1/8" bit? Amana recommends a 40IPM speed which is significantly slower than i have been using on other 1/4 inch bits but thinking that’s due to the need to take such a deep pass with this bit.

any recommendations or experience with this? Any tips for setting up CAM in fusion 360 for this? Is there a way to program fusion to take a deep first pass and then take a shallower step down after the initial cut and the top layer of the plywood is cut?

Thank you for the help!

If you are using a bit setter, try starting with a shallow pass using a down cut endmill to get to or just below the transition point of the compression bit. Then a tool change and finish the cuts. It is a lot less stressful than a large DOC with a long fragile bit. It might not make sense for production but as a hobbyist I’d take the hit in time rather than the wallet or extra stress (I’m doing this to relax :wink:).

Another way I deal with cases like that is using a roughing pass with [any suitable endmill] to cut to final depth, BUT leaving some radial stock to leave (say, 0.03" or less), and then follow-up with a single contour finish pass at full depth with the compression endmill that will just shave off the remaining material: there will be very little force on the tool then, and you still benefit from the compression endmill geometry in that the bottom edges of the stock will get cut by the upcut portion of the endmill, and the top edges by the downcut portion. If that makes sense.


Thank you for the replys!

Lester - I am trying to do the job without a tool change. If I cant figure out how to use the 1/8 inch tool, i will probably just change to complete the job with another tool. My goal for the 1/8 inch tool was to allow tighter nesting of parts in production and have less material being removed to be cutting out parts. Seeming like the challenges of the 1/8 bit might outweigh the positives.

Julien - This was my initial thought as well. I am attempting to do this without a tool change, but i was going to leave stock with roughing passes and then do a final finishing pass. However the part I am milling has curves on it that are preventing fusion from allowing me to leave radial stock on the contour CAM to then add a second contour CAM for finishing.

Update: I was setting up the roughing passes and finishing passes incorrectly in Fusion. I now have a CAM modeled which does as Julien suggested and takes roughing passes with .06 stepdown and then takes 2 finishing passes at full depth of cut with .0125 stepover. This process will work but will definitly take a long time. I am cutting out of plywood, now I am leaning the other way and thinking I am being too conservative with my stepdown. Thoughts? I dont want to baby the bit and end up burning it out because of rubbing. The CAM is going full WOC for roughing (slotting) and it is set for 40 IPM feed with 16000 RPM.

1 Like

With adaptive clearing toolpaths, you can choose to have a very deep depth per pass, and very low radial stepover such that the tool engagement is similar to having a low depth of cut but large stepover (the DOC/WOC balance strategy). On a Shapeoko, high DOC and low WOC is not often the optimal solution though, so if you are concerned about cutting times / material removal rate in addition to minimizing the tool breakage risks, you probably need to study the various combinations to optimize things, i.e. cutting parameters that will both limit tool deflection to a given limit while maximizing MRR.

@gmack came up with a cool spreadsheet that computes MRR and deflection (among many other things)

I can’t quite picture your project and toolpaths. If you can upload your f3d file, we can probably collectively have a look at it and see if we can propose optimizations, or at least brainstorm together around it ?