What's new
What's new

how do you calculate finish passes with endmills?

lowCountryCamo

Stainless
Joined
Jan 1, 2012
Location
Savannah, Georgia, USA
how do you calculate finish passes with endmills? Of coarse different for different materials. Do you use standard ipt and calculate for radial chip thinning? I feel like I could increase feed of my finishes passes. How about rpms? Slower or faster?

Thanks,

steve Austin
 
add or subtract feed/rpm as needed!

jk, i'm also interested in the science behind deciding finish pass parameters.
 
I'm sure you will get any number of answers. personally I leave between .01 and .02 for cleanup on both walls and floors. I generally run a rpm of 6800 in aluminum. if it's a long cutter I may drop it to below 4000. 1 thing you dont want is squalling in the corners. I generally run a .002 or less chip per flute in aluminum as my finish pass. play with it and see what works for you. In hard metals like 17-4 I run that at about a 1/4 of aluminum.
 
I run 16k RPM for finishing unless I have a L/D challenge, then slower to avoid chattter.

.002" IPT for workaday parts in Al with 3/8" & 1/2" endmills, and .001" for smaller. At higher IPT's, I can start to see the scallops.

If it's something precious or high-precision I might cut the IPT in half.

Regards.

Mike
 
For aluminum and steel I tend to leave .01 - .005 to clean up. On plastic I usually go .02...when surpacincg steel I leave .01 and aluminum and plastic usuly .005.

I run most of my finishing passes at 100 or more ipm using ramps on 2d stuff steel around 5000-7000 rpm and aluminum and plastic 12k.
 
the most important factors are
.
1) stickout length to diameter ratio
2) tool holder length
3) machine rigidity
4) part rigidity
5) work holding rigidity
6)if circular milling a bore, the cutter dia to bore dia ratio. for example 3" dia cutter on a 3.100" dia bore
.
obviously there are cutting parameters specific to tool stickout lengths and tool holder length. if depths are 0.5" its different than 5" or 15" depths
.
obviously finish is not good til you can see reflection like its a mirror in finish. end mills in general dont give as good a finish as facemills
 

Attachments

  • ShinyMilling_cropped.jpg
    ShinyMilling_cropped.jpg
    17.9 KB · Views: 253
I is HSM for roughing. Does it have a setting for finish passes? I have feel like a spend more time finishing parts than I should.

In HSMAdvisor you can just enable the HSM, disable Chip Thinning and set the feed override to 50%
Seems to work fine for most cases.
 

Attachments

  • HSMA_finishing.jpg
    HSMA_finishing.jpg
    96 KB · Views: 144
In HSMAdvisor you can just enable the HSM, disable Chip Thinning and set the feed override to 50%
Seems to work fine for most cases.

Not using HSMAdvisor, but this is basically what I do. I will utilize bonus SFM when good tooling and working setups are available. Typically when finishing from a dynamic path in Ti I will take a .025" semi-finish with chip thinning, then .005" finish pass without chip thinning, usually somewhere between .001-.002" per tooth feed for the finish path, tool size dependent. If the semi-finish is with the finish tool, I won't typically exceed the book recommended feed per tooth after chip thinning, if it starts to chip the flutes, I will increase up to 40% more on the ipt until the condition goes away, if it doesn't go away, then typically an increase in surface footage is needed. This of course is in stable conditions. Unstable parts, machine, or whatnot, you can throw all this out the window, and just have to play with it to find the best tool life or finish. Typically they will coincide with each other. Also, in these cases it never hurts to throw anti-logical solutions at the problem. Sometimes you get lucky and they just work better than what you would consider to be the best practice. The key is to figure why it worked and capitalize on it.
 
I generally leave between .020" and .005". This depends on how aggressively I am roughing (surface tolerance, roughing tool, corner chatter etc). Then I try and take a full depth finish pass when possible. I generally slow my rpms down to about 6k and a federate of about .002" IPT. This seems to give me the best cosmetic finish on my machines. I'm sure I could run the RPMs higher and the feed higher, but the above conditions coupled with my tumbling and anodizing processes yields very consistent and appealing results.

I also strive for absolutely consistent radial depth of cut on my finish passes. If I leave .005" on the wall, I want that exact amount all the way around, and I also want the cutter contact angle to stay consistent. This means that on some internal radii, I will do a quick high speed toolpath with the finish cutter to ensure that there is .005" all the way around, especially if I roughed with a larger cutter or had my max internal radius set high for roughing speed. I like the end result to be an absolutely consistent sounding smooth cut all the way around the finish cut. Any change in sound will show up in the finished product.
 
I don't think there's a good way to calculate a finishing pass. Finishing passes are inefficient because they're driven by the result and not the tool. You just have to use whatever ipt gets the finish you need at whatever the highest reasonable sfpm is, which will probably be determined by tool life.

For aluminum I leave 0.005-0.020 for the finishing passes, I take two identical finishing passes to reduce deflection, I use max rpm and ~0.005ipt (depends on cutter size and desired finish but I don't use more than 0.005 and I've been trending towards 0.004 and less lately, even with larger cutters, because it looks a lot better).
 
I'm surprised you guys are increasing your spindle speed for finish passes. I assume you are machining hard materials (steel, titanium, stainless...). In aluminum I generally slow down the spindle rpms and try and load up the cutter and get that low hum sound (scientific, I know). In hard materials I usually increase my RPMs by about 25%.

I guess it is still better than lathes... slow it down, take a big depth of cut, do some witch doctor dance and get a good surface finish
 
Using high helix end mills.

20-27K RPM depending on a few things generally part geometry related. .002"-.005" Finish pass. Feeds set accordingly for low side of chip load. 200 block look ahead.
 
To add to (or siphon from LOL) this discussion; the programmer I have been working with and learning from lately always repeats the finish pass. I understand why, as there is always a chip being taken the second go around due to deflection. Is this very common? It seems to me that tool life could decrease greatly in some materials if you aren't taking enough chip load? In the low volume production environment it did save us from having to lose a part or two developing the cutter comp to hit tight tolerances. Maybe that was the intention more than the finish quality.

I always hated to see a finish pass repeated since it was always the slowest part of the cycle. I could rough a part in 30 seconds, and then it could take three times that to finish and chamfer. I might save 20-30% total cycle time by skipping the repeat passes on some parts.

My biggest problem getting great side wall finishes has always been the radial moves in and out - I usually run a small bit over overlap to ensure there is no cusp but that means you can see much more of a blend line. I always just tried to get the CAM to move it to where it was the least innocuous.

One thing I found is finishing size on size inside corners, I leave as little stock for the finish pass as I can without over cutting during roughing (Like <0.005" if I can). The lower the rpm and less total radial cut in those corners seemed to do a good job at avoiding chatter.
 
I'm surprised you guys are increasing your spindle speed for finish passes. I assume you are machining hard materials (steel, titanium, stainless...). In aluminum I generally slow down the spindle rpms and try and load up the cutter and get that low hum sound (scientific, I know). In hard materials I usually increase my RPMs by about 25%.

I guess it is still better than lathes... slow it down, take a big depth of cut, do some witch doctor dance and get a good surface finish
Well, this is how I finish-face-mill. Super scientific too.

 
So today I inadvertently did something different on my finish path...I left cutter comp off by accident. Took a bit more than the .005 I left from roughing...I don't suggest doing that :)
 
To add to (or siphon from LOL) this discussion; the programmer I have been working with and learning from lately always repeats the finish pass. I understand why, as there is always a chip being taken the second go around due to deflection. Is this very common? It seems to me that tool life could decrease greatly in some materials if you aren't taking enough chip load? In the low volume production environment it did save us from having to lose a part or two developing the cutter comp to hit tight tolerances. Maybe that was the intention more than the finish quality.

I always hated to see a finish pass repeated since it was always the slowest part of the cycle. I could rough a part in 30 seconds, and then it could take three times that to finish and chamfer. I might save 20-30% total cycle time by skipping the repeat passes on some parts.

My biggest problem getting great side wall finishes has always been the radial moves in and out - I usually run a small bit over overlap to ensure there is no cusp but that means you can see much more of a blend line. I always just tried to get the CAM to move it to where it was the least innocuous.

One thing I found is finishing size on size inside corners, I leave as little stock for the finish pass as I can without over cutting during roughing (Like <0.005" if I can). The lower the rpm and less total radial cut in those corners seemed to do a good job at avoiding chatter.


I try and never do a spring pass. Sometimes you get a better finish, sometimes it does nothing but weld chips to the part. I never have felt that it is healthy for tool life.

I used to work with a guy that was in the habit of taking a conventional spring pass. He claimed that it "squared up" the part. He was a pretty smart guy, but I always found that it left a shitty surface finish.

I also worked with a guy that would run the cutter backwards on the spring pass to "burnish" the surface... he was an idiot and decided that machining wasn't his cup of tea.
 








 
Back
Top