[Ferrarone]

Hello!

I've recently converted a G0704 to CNC using an Automation Technologies kit. I've got no CNC, CAD, or CAM experience under my belt, and am hoping the G0704 will be a good learning tool for the next year. I've designed a part using Fusion 360, but I can't seem to correctly plot a tool path with the correct speeds and feeds to mill it. I purchased HSM Adviser hoping it would help me, but I'm either using it wrong or entering that information into Fusion 360 incorrectly. The end result is usually me blowinga fuse on the machine, snapping a mill, or stall. Anyways, here is a picture of my mill:



And this is the part I am trying to make:



Right now I'm simply trying to mill the part out of stock with a flat end mill. I haven't started on how to drill and chamfer the holes in the part. The part is being milled out of 5" x 2.5" x 2" 6061, and I'm trying to use a 1/2 HSS flat end mill. I don't really know how to choose the RPM, and the speeds and feeds in HSM Advisor appear to be to aggressive for my mill, even after selecting G0704 as my machine in HSM Advisor (somebody created a profile, seems to overestimate the abilities of the machine). I'm still learning Fusion 360, but if anyone is interested I'm more than happy to invite them to view/edit the part via email. I'd really appreciate any direction anyone cold offer, or a starting point! I'm just frustrating myself for hours on end and blowing these terrible 5mmx20mm tube fuses doing this on my own.

[Jim Dawson]

Try about 0.050 depth of cut, 5 IPM, and maybe 1200 RPM. I would probably use a 1/4 inch, 2 flute, solid carbide end mill (router bit from Home Depot), at about 2800 RPM, for that job.

[zero_divide]

The endmills are breaking because the machine is stalling.
I would suggest decreasing the "Warning at" number (in the Machine Definition dialog) from default 95% to perhaps 50% and then see how that goes.

If you could provide more info in the kind of cut you are trying to take, I could come up with a better solution, perhaps.

[Ferrarone]

Try about 0.050 depth of cut, 5 IPM, and maybe 1200 RPM. I would probably use a 1/4 inch, 2 flute, solid carbide end mill (router bit from Home Depot), at about 2800 RPM, for that job.

Hey Jim,

Do you mean a .050 depth of cut, 5IPM, and 1,200 RPM with the 1/2 end mill I'm running? And what width of cut would you suggest?

[Jim Dawson]

Hey Jim,

Do you mean a .050 depth of cut, 5IPM, and 1,200 RPM with the 1/2 end mill I'm running? And what width of cut would you suggest?

Yes. Maybe about 40% (~0.20) cut width. It will require some experimenting to dial in the best combination.

[Ferrarone]

Yes. Maybe about 40% (~0.20) cut width. It will require some experimenting to dial in the best combination.

Thanks for the quick reply. Here's the tool path with those settings, I've thrown that information in HSM advisor just for a look.



Machine time is way longer than I thought this part would be, but I will fiddle around with it tomorrow.

Edit: My uploaded images seem to be getting resized to much smaller. Not the end of the world but it's hard to read off the data. Is it possible to make them larger on here? Machine time on this is 6 hours 10 minutes.

[fmfchop]

What were the recommended settings originally?

I would think that'd be in the ballpark of 3000-3500rpm and a feed rate of somewhere around 60ipm. For stepover I'd go 75% and leave a spring pass that would run at a slightly faster RPM.

That 6 hour figure is WAAAAAYYY high.

[Jim Dawson]

Thanks for the quick reply. Here's the tool path with those settings, I've thrown that information in HSM advisor just for a look.


Machine time is way longer than I thought this part would be, but I will fiddle around with it tomorrow.

Edit: My uploaded images seem to be getting resized to much smaller. Not the end of the world but it's hard to read off the data. Is it possible to make them larger on here? Machine time on this is 6 hours 10 minutes.

6 hours seems a bit excessive, even with the very conservative numbers I suggested. I can't read the specs on the picture, too small. You might need to edit the screenshot and split it into 2 pictures.

I would split the job into 3 or 4 separate operations, that way you can adjust your cutting parameters between operations. If the machine is not being overloaded at the numbers I suggested, then bump up the feed and speed for the next operation and see what happens. You need to get enough time with your machine to figure out what load it will take.

One thing is missing from the equation, how many flutes on your end mill? For aluminum you should be using a 2 or 3 flute endmill, and preferably one designed for aluminum cutting. Also, what coolant are you using? Kerosene is my preferred coolant for aluminum, applied with a anti-fog mist system. WD40 works also. Aluminum likes to instantly weld to the endmill if you are not using some kind of coolant, which instantly causes the spindle to overload and breaks the endmill.

What were the recommended settings originally?

I would think that'd be in the ballpark of 3000-3500rpm and a feed rate of somewhere around 60ipm. For stepover I'd go 75% and leave a spring pass that would run at a slightly faster RPM.

That 6 hour figure is WAAAAAYYY high.

That would be about correct if the machine would take the load, but the problem we are trying to solve here is stalling the spindle due to overload. The numbers I suggested above are just a conservative starting point, with a chip load of about 0.0015/tooth on a 2 flute. I would expect that they will be bumped up once Ferrarone is more familiar with the machine and CNC machining in general.

On my machine, I would profile that part in 4 passes, 2 full depth roughing passes with a roughing endmill and then come back with the finishing passes with a finishing endmill. But I have the HP and mass to do it.

[rowbare]

John Saunders has a decent video series on Feeds and Speeds. He is talking about carbide (the series was sponsored by Lakeshore Carbide) but the principles are universal. It is well worth the hour or so that it takes to watch it.

https://www.youtube.com/watch?v=Bupr...EDs1lbSoE6H2a6

He also has a few videos where he is testing feed and speed and DOC/WOC combinations. This one lays out the process.

https://www.youtube.com/watch?v=SzBFJ7oRo8c

For what you are doing, I would suggesting half or full depth cuts and reduce the width of cut to 10 or 20% of cutter diameter. This way you are using more of your endmill.

bob