Who is currently successfully cutting aluminum with their Lead 1010. My Lead is stock with a dewalt 611 router. Looking to cut out a mounting plate for a 3d printer build from 6061 aluminum. There is a decent flat area that needs to be milled down a few mm would I want to use a fly cutter or just stick with an end mill. Lastly if you are successful could you recommend a few end mills and starting feeds and speeds (i know they are just a starting point) thank you!
First of all, I'd suggest you never use router bits designed for wood on aluminum, so unless you have a fly-cutter meant for metals, just use endmills for your facing operations and finish by grinding or sanding, if neccessary. Also, remember a cutting fluid may help your cuts on alu significantly. As for the selection of endmills: Your DeWalt has a very high minimum speed, which already limits the suggested diameter of mills. I'd say stick to smaller mills, in the sub- 3/8" (about 10mm) area. If possible, go for endmills designed for aluminum and use one or to fluted endmills. Three and four fluted spin too fast on your router and are highly likely to rub. And for speeds and feeds: Check Carbide3D's video on the subject: It's made for their Shapeoko machine, which is quite similar to the Lead and Workbee machines, and those parameters will get you started. Regards, Will
I agree with the statements provided by Will. For bits you can try the new SharkBits on the OpenBuilds Store -> O Flute / Up-Cut like the ones here are recommended for milling or surfacing aluminum CNC Router Bits - Pocket/Cut Out - OpenBuilds Part Store
OpenBuildsPartstore now stocks specially selected endmills - tested to work well with our machines and router setups (See our Instagram for glamour shots of the SharkBits in action) Buy them here: CNC Router Bits - OpenBuilds Part Store
Hi, I know this is an old thread, but recycling is good for the soul. I have had great success milling 6061-T6 aluminum as follows: Bit: 3mm, straight cut, 2F Router: Makita RPM: Makita position 3 Type of milling: Trochoidal Trochoidal settings: Stepover 10%, Width 50% Feed rate: 2480 mm/min Plunge rate: 480 mm/min DOC: Full depth Finishing pass: .5mm Pass feed rate: 480 mm/min Be warned, even with 3mm stock, the Workbee X-axis deflects quite a bit. But the cuts turn out very nicely nonetheless. Here's a screenshot of Estlcam: Regards, Duncan
Thanks. I really need to try this. I have just been cutting with slots, but it has been working for me.
