What's new
What's new

Surface Finish Issues With Extended Length End Mills

F35Machinist

Plastic
Joined
Nov 3, 2021
I'm trying to machine a 1.25" deep pocket in 6061 Aluminum with 2 degree tapered walls using an extended reach necked down 3 flute .25" ball endmill with a 1.25" reach. I am currently machining with 5000RPM (~330SFM) 120IPM (.008 per tooth)with a .01" depth and width of cut. The machine is a Fadal 3016 (10k RPM max) and the setup is rigid.

In my experience with extended length cutters, I usually just reduce the speed and up the feed until the chatter stops. In this case, I need the walls to have a finer finish than the stable feed per tooth will allow. I would like to have a feed rate of around .001" per tooth, but I don't want to have to run this at 1000 RPM. Is there some trick to getting a good finish with reasonable productivity?

I am looking for some suggestions for: speed, feed, depth of cut, width of cut.

Thank you all and any help is much appreciated.
 

mhajicek

Titanium
Joined
May 11, 2017
Location
Minneapolis, MN, USA
Run it at max RPM. .008" per tooth seems on the heavy side. Try .004", and maybe do another finish pass with .002" stock. Is the cutter designed for aluminum (not steel)?
 

TheBigLebowski

Aluminum
Joined
Sep 9, 2018
As mhajicek said - feed is way to fast for a contour operation. When finishing like this you don't need or want to account for chip thinning. Rough as fast as you wish with the biggest endmill possible leaving approx 10% (~0.0025") of your finish tool diameter for stock. If I was going for a good surface finish I would run it at 0.002" per tooth feedrate. If you have a number of them to do, I would invest in a tapered endmill to do the finish pass in one go instead of 3x milling.
 

MaxPrairie

Hot Rolled
Joined
Jul 9, 2015
What is the corner rad on the pocket? I think it will be tough to get a good finish and maximum productivity on that.
 

F35Machinist

Plastic
Joined
Nov 3, 2021
Thank you for the responses. Unfortunately, simply lowering the feed will not work. Also, lighter depths of cut don't work on extended length end mills. The endmill bounces off the workpiece and chatters very badly without enough width of cut. The feedrate is set to where the cut is stable and doesn't chatter. Lowering the feedrate causes the tool to chatter.

The corners are .125 radius, but I don't have any issues in finishing those. The reason I can't just use a tapered endmill is because the bottom of the pocket also has a radius of .125 that needs to be finished with this same tool.
 

F35Machinist

Plastic
Joined
Nov 3, 2021
I didn't take a picture, but it looks exactly like what you would expect a .008" per tooth cut to look like (.008" scallops on surface). I ended up smoothing it out with some sandpaper, but I don't want to have to do that next time.

I'm just looking for some advice from someone who has some experience with extra long endmills and mold making. A lot of the suggestions make sense for regular length endmills, but extended length requires a different strategy and many of the typical ideas like taking lighter widths of cut are the exact opposite of what works.
 

MaxPrairie

Hot Rolled
Joined
Jul 9, 2015
I didn't take a picture, but it looks exactly like what you would expect a .008" per tooth cut to look like (.008" scallops on surface). I ended up smoothing it out with some sandpaper, but I don't want to have to do that next time.

I'm just looking for some advice from someone who has some experience with extra long endmills and mold making. A lot of the suggestions make sense for regular length endmills, but extended length requires a different strategy and many of the typical ideas like taking lighter widths of cut are the exact opposite of what works.

I reread your original post. I was thinking you were using a tapered endmill. Sounds like you are ballnosing the taper on the pocket. I would typically leave 2 thou for a finish pass but I see that was already suggested. Lighter cuts are working because your tool is deflecting and you need pressure on the tool to keep it from chattering. I would try a ballnose with 3/8 LOC like what I’m looking at and see if that adds enough rigidity to take a light finish pass.
 

IamBob

Plastic
Joined
Aug 29, 2021
Location
Minneapolis, Minnesota
I guess I'm not surprised either you aren't getting a great finish with that high of feed and that length tool. I do lots of 10-15x D surfacing. I usually use a 1/2 tool and leave 1-5 thou going fast then finish going nice and slow with the finishing tool
 

zero_divide

Stainless
Joined
Feb 2, 2012
Location
Toronto
I must have machined thousands of cavities with ballnose endmills.
My go-to numbers for finishing aluminum with that cutter would be 10000 RPM, 150ipt, 0.005" step down. 0.003" width of cut.

Do make sure you semi-finish first.

You should get a good surface. Depending of how clean is required, might want to drop ipt and step-down to 0.003" but then you can actually see your face in it.
 








 
Top