cutter leaving feed lines at high feed rates-walter prototyp end mill

shimmwagen · Jan 23, 2014

trying a new cutter out, walter prototyp AH3021138-3/4, 8 flute solid carbide endmill. cutting a 16" half circle/8" radius in a cast iron part, machine is a daewoo dhm500. approximately .200" of material coming off. manufacturer recomended this-----S= 4400 RPM... sfm of approx 860 based on structural steel 44W / A36 / 1015 F= 352 IPM... ----- we ran it at this and we could barely hear the cutter, nice chips coming off and the size was dead on. the strange thing is that we got feed lines on the surface, almost looked like a zip tie/zap strap! we slowed down feed into the 100's which shortened up the lines but they were still there... any one have experience with these endmills?? all the math works out for depth of cut and speed/feed. the tool rep thinks maybe the machine can't keep up with the code but i am just using a g3 to make the arc...

this is the current solid carbide code im using, i just changed speed/feed accordingly for the walter endmill...

(FINISH 7.811 RADIUS)
(HOLD SIZE TO 15.62 +.01/-0)
N3T53M6(T3-H194)(.75 FINISH ENDMILL)
T55
G54G90G94G0X-3.1Y-6.4375B0
S800M3
G43Z3.0H194
Z1.
M8
G1Z-1.1F40.
G41Y-7.4375D194
X0.F13.
G3Y7.4375J7.4375
G1X-3.1
G40Y6.4375
G0Z1.
M9
G91G28Z0.M5
G91G28X0.Y0.
M1

any thoughts/suggestions would be appreciated.

glenn

exkenna · Jan 23, 2014

Hi Glenn

8 Flute end mills have an extremely narrow sweet spot. You're not in the sweet spot.
They are intended for very light radial depths of cut. I know you said .200 material coming off but is that your true step over? If so, you've got at least three flutes in the cut, depending on the helix angle of the tool. If its a high helix (50 degree or better) you could have 6 flutes in contact with the material. Lots of tool pressure.
Try a 6-flute 40 degree helix with eccentric relief. Should solve your problem.

DMF_TomB · Jan 24, 2014

some roughing cutters for cast iron are rated for over 0.012" or even 0.015" inch per tooth feed. obviously they leave a rough finish.
.
i have seen carbide insert cutters where 1 out of 8 inserts was a wiper insert to clean up the surface. these mills at 0.005" ipt feed left a moderately fine finish.
.
we use 6" dia face mills at 15 to 35 ipm feed. one pass instead of at least 12 passes and the machine is more accurate at slower feeds. we hold 0.0005" flatness, straightness, perpendicularity tolerances over 6 foot distances verified by a CMM in the inspection lab

Red James · Jan 24, 2014

Glenn, even though you program with G3, your servo motors don't understand what that means. The control will convert the G3 into short straight line moves to machine the arc, so it could be true about the speed of the control " the tool rep thinks maybe the machine can't keep up with the code but i am just using a g3 to make the arc..." No comment is intended about your control, I have no knowledge / experience with daewoo controls.

upnorth5axis · Jan 24, 2014

slow the feed down to lets say 50IPM and run it to see what it looks like and also add a straight line move for 3 or so inches to compare the radial cutting to the straight line cutting (make straight line move using only X or Y not both). Then try 100ipm , then 150 , then 200 look at your finish each time you may be able to see the finish slowly getting worse on the arc compared to straight line. this will tell you the machine isn't keeping up. As far as the cutter goes it should give the same finish when cutting a large arc like you are or a straight line move.

Speedie · Jan 24, 2014

It should be pretty obvious your either not getting good resolution from your motors or your not holding the endmill on center. My guess it your holding it off center.

shimmwagen · Jan 24, 2014

there is a 3" straight movement in 'x' at the beginning of the pass and still leaves the "feed" marks. the cutter is being held in a er40 holder and is running true to less than .001". our maintenance guy here wants to check servos when running the machine at high feeds to see if they fluctuate at all. im not sure when the job is coming up again and with the shop super busy right now i haven't had much opportunity to play with speeds/feeds. thanks for the comments and ill keep you posted as to how it turns out. worse case scenario is that i use it as a roughing tool only which will still save huge amount of machining time.

allloutmx · Jan 24, 2014

how much weight is on the table? I had a similar problem this week. the machine Im on has a 1-1/2" subplate the length of the table, two indexers a cradle and three vices. Had a F of a time trying to figure out my issue, but Im almost 100% certain the machine is having a hard time starting and stopping with all that weight up there.

Mtndew · Jan 24, 2014

Can you post a picture?

shimmwagen · Jan 24, 2014

i wish i had taken a picture but did not. the lines did get shorter when we slowed the feed down into the lower 100's but still too much for the specs required. im running the part on a horizontal mill, part is fixtured up on a tombstone, so i don't think weight is an issue. the part is quite light too. i was given some new speed/feed numbers that i will try next time i run the part...

this is what i got from the tech guy...

1) ROUGHING:

use 660 sfm and 0.005" Hex as we did on initial test
take one pass on the test/demo piece at 0.160" radial doc, then...

2) FINISHING:

use S=6078 and F=641 at only 0.027" radial doc
take a pass and inspect
if its acceptable then machine to correct size
if its not then machine to correct size using existing method

3 SUBSEQUENT PARTS:

roughing ; with multiple 0.160 deep passes leaving 0.027 on for...

The finishing data shown is a calculated theoretical 100Ra max finish

he's using DOC parameters for speed/feed calculations. i kind of understand what he's getting at with the whole thing, using a 3/4" cutter to remove .027" of material is going to be a super low load on the tool, going to slow will cause cutter to "rub" instead of cutting. i'd love to get this cutter to work as going from F10.-F15. to 100-300+ipm would be a huge time saver.

Red James · Jan 25, 2014

"he's using DOC parameters for speed/feed calculations. i kind of understand what he's getting at with the whole thing, using a 3/4" cutter to remove .027" of material is going to be a super low load on the tool, going to slow will cause cutter to "rub" instead of cutting. i'd love to get this cutter to work as going from F10.-F15. to 100-300+ipm would be a huge time saver."

Then you need to hold your cutter concentric. A couple of 'tenths' runout, then you can feed that fast. Finish would look good, though accuracy may suffer.

shimmwagen · Feb 6, 2014

ran it again. rough at 3500rpm with 150" feed, finish at 4500rpm and 125" feed. estimate 150Ra surface finish. two .160" rough passes and one .027" finish pass. i dialed in tool and found around .002 runout with er holder. switched to solid holder and runout is now approx .001.

shaky cell phone video here...

3/4 Walter 8 flute endmill - YouTube

Limy Sami · Feb 6, 2014

I watched the Vid and IMO the part is vibrating - you can hear it singing, stop where there's more support then start again, look to better clamping, if that isn't an option try running a smaller dia cutter - it can help.

shimmwagen · Feb 6, 2014

we're limited with clamping. milling the back as well with back face tool so no where to support underneath the part. it is just a cradle that a winch housing sits in so finish isn't super critical. we make our own product so all that needs to be done is convince engineering/inspection that a little roughness does not affect the final product. would like the tool to last as well though, we were told that too slow feed will cause the tool to "rub" which lessens tool life...

Limy Sami · Feb 6, 2014

Change to a smaller tool with a low helix, high helix tools cause more ''pull''

allloutmx · Feb 6, 2014

You couldnt use some small jack screws off the back?

Milland · Feb 6, 2014

Hi Glen,
I think the lack of support of the part is an issue, the video was pretty clear on the change in cutting sound. Since you can't change the fixturing, and it sounds like you're happy with the roughing performance of the cutter, why not use a finishing tool? I agree with Limy Sami that a smaller diameter cutter will put less "energy" into the part, but the other thing that might help is to change the helix of the cutter so you don't pick up the existing vibration pattern and replicate it in the final pass. If you had lots of these parts to do I'd think about a custom compression cutter (like for composites: Compression End Mill supports composite machining., Sandvik Coromant Co.) but made for cast iron. The alternating helix angle could be tuned via RPM and feed to a sweet spot that stopped the singing.

An easier thing to try would be a low-helix tool for the final cut, it would have less axial load on the part, reducing the singing. Again, I'd try a 1/2" tool and around .015-.020" DOC. Try to lower the runout, I'd want no more than .0004" with a 1/2" tool, less is better. An SGS Z-Carb with its variable flute spacing could work too.

shimmwagen · Feb 7, 2014

full length video here, youtube only let me do 45 seconds for some reason. when i do the final pass the cutter/part wasn't as noisy.

https://www.dropbox.com/s/fk4tuocfc4bt4a4/2014-02-06 22.13.31.mp4

we have a couple screw jacks/bolts at tip of the cradle where the outer clamps are. i realize it's not the most rigid setup but it's the best we can do if we want to machine the part in one setup. the part gets machined on the bottom as well which is why we have no other way to put support on the longer section that's in the air. like i mentioned the finish has been accepted so that's all good, i'm just hoping cutter life will be sufficient to warrant the price of the tool. excess vibration will affect cutter life i assume? i haven't done a lot of high speed machining on anything but aluminum so not sure what to expect with our cast iron. i was told we average 40 pcs a month, i'm saving 6 minutes per part so that's 4 hours a month, shop rate is around $100 per hour so if i can get a couple months use out of it the price will be worth it. plus i can use it on other jobs.

shimmwagen · Feb 7, 2014

and i have thought about the finishing tool option as well. i'm not a huge fan of roughing and finishing with the same tool. i find it much easier to keep tolerances in check when using a finishing tool. i'll look into the compression cutter...

Limy Sami · Feb 7, 2014

One trick that might help ;-

Cut yourself some pine wedges and just lightly seat (tap) them in between the job and fixture plate, they will help stop the job ringing and rattling.

cutter leaving feed lines at high feed rates-walter prototyp end mill

Plastic

Stainless

Diamond

Stainless

Hot Rolled

Stainless

Plastic

Titanium

Diamond

Plastic

Stainless

Plastic

Diamond

Plastic

Diamond

Titanium

Diamond

Plastic

Plastic

Diamond