Here’s something I don’t understand. In CC, I can use a pocket op to “drill” a 5.5mm hole .25 inches deep into a 1.27 cm thick piece of wood using a 0.125 inch flat end mill. If I try to do the same operation in Fusion 360, it won’t let me because it says there is insufficient room for ramping. I’m still trying to get the hang of the terminology in the art of milling, but I could use an explanation of why the same operation with the same tools on different pieces of software should be different.
Different algorithms and tolerances.
Perhaps it’ll work better if you plunge cut rather than ramp in in Fusion 360? (Carbide Create doesn’t do ramp entries — maybe if it did that sort of toolpath would have the same limitation).
Anything here help?
I use the post process setup as noted in the link. And I found the place where you can set the ramping (under Linking). There are lots of ramping options. Once I changed that to plunge, it worked like CC. F360 has context sensitive help but in a lot of ways it reminds me of the old days of running IBM computer equipment. The only people who could understand the IBM documentation were the people who didn’t need the IBM documentation.
You are generally better off leaving the ramp as a helix and reducing the helix size. For a 0.125" (3.2mm) endmill in a 5.5mm hole, the maximum helix diameter is 2.3mm without the hole being oversize (and the software refusing to generate it), and 1.8 to 2mm is what I would go with to leave sufficient material to prevent rubbing as the inside surface of the bore is cleared. Also be sure to specify the “stock to leave” as 0. It defaults to something like 0.5mm (0.020") IIRC. On a hole smaller than about 4.2mm, a 3.2mm tool will fail, and on the 5.5mm, the maximum helix size will be reduced to 1mm without reducing this.
The helical ramp is very good for getting the chips out and controlling the engagement of the side of the cutter without rubbing on the way in. Plunging, even with a center cutting endmill, can lead to issues with clogging. This isn’t a particularly deep hole for this tool, but at twice the diameter, clearing the chips is a concern. A helix diameter smaller than half of the tool diameter begins to lose the benefit of the helical path. When there is room, a tapered helical path is better, but in this case, there isn’t.
I think I get it. Let me see if I envision this correctly. If I were to do a pocket with plunge, the bit would plunge to the set depth and then follow an inside path around the hole?. With the helical, it would gradually spiral down into the pocket to the bottom of the hole? Outside of chip clearing, does the helical path (if I’ve envisioned it correctly) cause less tool wear and pose less of a breakage risk than the plunge because less of the tool length is cutting?
Depending on whether you enable multiple depths, yes.
The helical allow better chip clearing, which reduces risk of tool breakage and reduces power requirement. It also can reduce wear, depending on the material.
For any hole, no matter the strategy used, leaving 0.1 or 0.2mm for the finish cut, then finishing with a bore operation will give a much better result by reducing tool deflection.
For the hole you are doing, in wood, I would helical entry pocket or adaptive with 3mm per pass to final diameter and call it a day. In aluminum or similar, I would helical about 1mm per pass to 0.2mm undersize (on diameter, 0.1mm stock to remove) then run a bore operation (helical constant engagement) to finish size.
Depending on the need for the bottom finish, I might run the initial cut full depth or leave 0.1mm for the final cu. On a larger bore (more than twine the tool diameter) I’d leave 0.1 or 0.2mm and run a finish pocket cut for the bottom to leave it clean.
1 Like
Listen to the others (regarding the helix ramp editing) OR try the BORE function in F360. Someone recommended it to me and I haven’t use the drill function since.
Note; It WILL leave a core if the hole diameter is large and the cutter is small. If you don’t like leaving a core, start off with making a smaller hole first.