[Otokoyama]

I'm getting back into machining after a roughly 8 year hiatus. I'm working on an aluminum project, having generated code with OneCNC.

I'm cutting a pocket that's rather deep using a long 3-flute 5/16" diameter 2" cutting length HSS end mill. I'm getting terrible inside wall surface finish. The program cuts layers 0.13" deep in .17" strips using conventional milling with Kool Mist, running 3000 RPM with a feed rate of 9 inches per minute.

Successive cuts appear to create a series of ledges, especially in radiused corners, where the end mill swings outward around the cut.

The end mill is in a collet chuck, since it wouldn't fit in a 3/8" shaft end mill holder. I'm not sure why because an identical end mill did fit.

The only thing that comes to mind is that for the length of end mill, I'm trying to take too big a cut. When the end mill bites into the aluminum, the end gets pushed away from the flute direction, outward into the the radiused corner.

Assuming I've described this problem adequately, does anyone have any ideas what might be causing this problem?

Thanks.

Paul

Showing radiused corner "ledges":
Attachment 225392

Showing generally uneven walls:
Attachment 225394

[AARONT]

try climb milling, conventional milling usually does not give the best surface finish. It also looks like you're not getting good chip evacuation.

[viking73]

Do a finish pass at depth with a new end mill. You may have to experiment with speeds and feeds to eliminate the chatter. Long end mills are obnoxious.

Sent from my SAMSUNG-SGH-I747 using Tapatalk

[Otokoyama]

Thank you.

I'll try climb milling, a finish pass, lighter cuts, and also a variable helix carbide end mill.

[sortafast]

Use a 3flute carbide endmill specifically for Aluminum (YG alu-power work well and are cost effective), Climb mill it, do a finish pass at full depth but like 0.010 into the sidewall or a little less. Also, on a 5/16" endmill, 0.13" DOC seems kind of on the high side. Might try scaling it back to like 0.050-0.080" but run at a faster feed (the carbide bits will allow this). On my set up I am limited to about 3200rpm on the spindle, but I run a 3/16" Alu-power endmill around 20-30ipm depending on the DOC and desired surface finish. Another thing you might check is the tram of the head on your mill. Make sure its perfectly aligned. If its a little out of whack it can do some of the stuff like whats going on with your sidewall. I would also run the shortest and widest endmill you can that will make that pocket. Stiffness is not underrated and bigger endmills tend to be able to live with higher speeds and feeds. Also, your HSS bit might be a bit worn.

[Tkamsker]

I Mill a lot in Alu what ever this " Means i recommend higher RPM high forward speed and less depth per layer. I use for instance an 6 mm Single Flute miller with extrem steep twist to remove the Chips. And flood cooling is mandatory ..

Gesendet von meinem SM-N9005 mit Tapatalk

[Otokoyama]

Thanks for the additional suggestions. I tried with the 5/16" HSS end mill at 3500 last weekend with less depth, and got a fairly good finish. I will try with the carbide end mill at 6000 this weekend.

I'm using 5/16" to avoid a tool change, though the vast majority of the work except for a small slot in the bottom can be done with 3/8".

When doing a full depth (1.25") finish pass, what is a reasonable cut? I've currently got this at 0.002". Sorta fast recommends 0.01" or a little less. Should this be greater than 0.002"?

Thanks.

[sortafast]

I usually do finish passes on the 1/2" endmills at 0.01" or so. Even do that with the 3/8" and get good results. But I don't have any parts that I do that have a 1.25" DOC so your mileage might vary. I could be totally wrong on this, but some designs need a minimum amount of material to be removed. My thoughts are as the size of the bits get smaller so should the radial and axial DOC. 0.002" seems kind of light to me. Perhaps go to 0.005" and see what happens. With aluminum specific carbide endmills I think you will be amazed at what you can get done. I have been running the YG's and they have served me well. I just got an MA Ford 138 series 1/2" endmill to try and seems good so far. I just ran an op with a Garr Aluma-Star 3/16" endmill and I wasn't terribly impressed with it but I haven't really had a chance to really figure it out and see what it can do. But there are a lot of options out there. Definitely worth the extra $$ IMO. You can run way faster speeds and feeds. I have 2.5" face mill that will absolutely murder 6061 if I need. Just be aware that, around here in NW Oregon anyway, most aluminum specific end mills are only available in 1/8" increments.

[Tkamsker]

Hi normally (Not Finishing ) the Cut sideways Maximum 1/2 Diameter and depending on length of Cutter and Type of machine you can do 1/4 of cutterdiameter. But at Alu i recommend sideways 1/2 Diameter - 10% and depth max 0,5 mm at Last Run for nice finnish use 0.3 mm and 0.3 mm and higher Speed the the Alu has no Time to get hot and a Good Chance to get away from cutting Zone i did an complicated Part on an 60x60mm Quader where i First started with an 6mm Single flute and 30mm Long (cutting length) Tool so clean and Deep was possible for Sharp Corners i used 3mm Dual flute 15 mm Long Miller and cooling is mandtory ,..


Gesendet von meinem iPad mit Tapatalk

[Otokoyama]

Yeah, I was concerned about a minimum cut, so will bump up from 0.002" and try 0.005", though will try two passes at half 1.25" each. Plus, I shouldn't be so concerned about a tool change and will try the 3/8" carbide that I got, which is aluminum specific. One way or the other, I need to get it done this weekend. :-)

[Tkamsker]

I recommend as more the Miller Looks from an Horror Film the better it Works for Alu ,..


Gesendet von meinem iPad mit Tapatalk