G0704 High Helix end mill pocket problems

[DJEkim33]

Been working on some parts that require a deep pocket. The basics of the pocket are 1.25" deep, 2.5" long and .690" wide with the corners radiused .220". For the most part the pocket is symetrical except for a small contour and shelf at one end but for the purpose of diuscussion I will focus on the main dimensions of the pocket.The material is 7075 (guessing T6). My probelm is that when I try and perform a finishing operation with high helix end mills they seem to be deflecting out of the cut.

I have been using a 3 flute carbide end mill to rough it out with no issues there, I am ramping down a slot at .1" per revolution 60 ipm, 6000 rpm with .020" stock to leave. I then have followed up with a Niagara Carbide 3fl A345 45 degree helix .375 diameter x .375 shank x 1.5 LOC sticking out 2" needed to clear other features from a TTS set screw holder, link here N61647. The problem cut comes on the last pass which is .005" WOC and 1.25" DOC, 60ipm and 6000rpm climb milling. I use one spring pass to clean up anything leftover. The end result is awesome finish no chatter but instead of a pocket .690" wide I get a pocket .678" give or take, some parts are better than others. I have the same issue with the length and the other dimesions and features. It usually takes another 4-6 passes with negative compensation on either the cutter or negative stock to leave to get it to final dimension. Chips are coming off thin and wispy.

I have tried:
Slowing down the cut
Speeding up the cut to 120ipm
Roughing step downs of .1" with .002" stock to leave for the finish pass
Ramping to a narrow finish pass
Measured the cutter to make sure its to spec with <.001" runout


All with similar results, the pocket is not even close to spec. I suspect the cutter is deflecting I would just like to know why. What leads me to believe this is that I do the same exact cut with a Niagara HSS 4fl SC406 30 degree helix .375 diameter x .375 shank x 1.5 LOC sticking out 1.75" and it does the cut to spec just at 25 ipm and with a lot of chatter and leaves chatter marks in the corners. My hope of going to the high helix was to get ride of the chatter marks with a more stable cutter. I also used a similar Niagara HSS A337 7/16" 37 degree helix which had less chatter but was giving the same issue of not finishing to spec but was closer than the carbide.

Ultimately I know the answer is probably the machine is not rigid enough to do this but I was hoping to see if anyone else has run into this issue or if I am missing something obvious. I have seen people have good luck with the YG1 42 degree end mills but most of the time folks just reort feeds and speeds achieved and don't meantion if the cut is within the accuracy they were trying for.

Thanks for any advice and help in advance.
Mike

Similar Threads:

• Need Help!- helix to close to edge of pocket
• *NEW Dura-Mill 5/8" 3 Flute - 60° High-Helix Carbide End Mill
• *NEW Dura-Mill "Mixed Bag" 60° High Helix 3 Flute Solid Carbide End Mills - TiCN
• High Helix Endmills
• High helix end mills keep gouging

[Jim Dawson]

Did you measure the end mill? Carbides tend to run a bit small. The carbides I normally use measure 0.005 to 0.010 small, I just plug in the cutter comp. I normally run a finish pass at 0.1 step down and 0.020 WOC. Yes, that takes longer, but it leaves a nice finish and an on-size part.

[atomarc]

Jim,

Wow...those endmills are .005 to .010 under their advertised size? Never heard of such a thing. I think I would find another source for my tooling.

Stuart

[DJEkim33]

Jim,

Wow...those endmills are .005 to .010 under their advertised size? Never heard of such a thing. I think I would find another source for my tooling.

Stuart

No the end mill is dead on to size. It is less than .0005" undersized which is well within it's tolerance stated.

When I was using it in a ramping operation I noticed it was cutting correctly for the first little bit of the operation and then would deflect out. I have not tried a similar operation in 6061 to see if it's the combo of hard material and lack of rigidity in the g0704.

[Jim Dawson]

Jim,

Wow...those endmills are .005 to .010 under their advertised size? Never heard of such a thing. I think I would find another source for my tooling.

Stuart

I should have put ''end mill'' in quotes. I use a lot of carbide router bits for end mills. The ones from from the local big box store tend to run a bit undersize. The shanks are on size, but the cutting ends tend to run under. The web is a bit thinner than a conventional endmill so they won't hog material, I normally run DOC at 0.5D when cutting full width and a chip load around 0.002. On the other hand, they are razor sharp and seem to last very well in all materials. The helix angle is perfect for aluminum, and works well in other materials.

I would try reducing the DOC on the finish pass, that should take the load off of the machine and eliminate spring. Maybe try dramatically slowing the feed and speed down, maybe 2500 rpm and 10 IPM or so.

[bhurts]

I have used a lot of endmills from many different suppliers. Always good quality if I'm not in a bind and have to take what I can get locally. In my experience high speed steel is dead on size both shank and cutter pretty much always. Carbide the shank is always is dead on size and the flutes run .001-.0015 undersized. That doesn't explain the issue here but it's my experience. I have also found as Jim said that router bits even of good quality the flutes are usually undersized .003-.01. The shanks are dead on.

Ben

Sent from my HTC6525LVW using Tapatalk

[photomankc]

Machine should be fine to do that. That looks like about 0.006" on each side off. Is the 2.5" dimension also off by the same amount? I've not seen my carbide endmills off dimension by anywhere near enough to account for that or deflection of more than 0.002 or so even with heavy passes. What about backlash? Are exterior dimensions all as expected in the same axis?

[DJEkim33]

Machine should be fine to do that. That looks like about 0.006" on each side off. Is the 2.5" dimension also off by the same amount? I've not seen my carbide endmills off dimension by anywhere near enough to account for that or deflection of more than 0.002 or so even with heavy passes. What about backlash? Are exterior dimensions all as expected in the same axis?

I have not measured the interior 2.5" entirely as it is a bit difficult since there are a number of features in the way. I have measured portions of it and they all are not to spec also. Backlash on the machine is .001". Its a precast part so I am not finishing the outside. It is 7075 so technically it should be twice as strong as 6061 and a bit harder. The part that gets me is that the HSS end mill does just fine in a single pass, just some chatter marks in the corner when climb milling, I will try and do one conventional.


As for other things I have tried:
Did cuts at .005" WOC and .250" DOC, no luck
Did a ramping operation, this had limited succes as the cutter stayed on track for the first .5" of cut and then deflected out. How do I know this you may ask? Had a good line on the wall until that point. The line disappeared when I finished the pocket to spec with HSS.
I tried everything at different feed rates from 12IPM to 120IPM, although the same RPM.

I know carbide is a bit duller and according to Niagara these cutters have a different geometry to them but I would believe they should have no issue doing a light cut like this but they are not even developing good chips. I am also looking at some YG-1 carbide or any other aluminum specific tool suggestions anyone has to give it a try.

[Jim Dawson]

.
I tried everything at different feed rates from 12IPM to 120IPM, although the same RPM.

You might try lowering the feed rate and the RPM, and keep the chip load up around 0.001 to 0.002. I have found that this works well with a 1/4 inch carbide endmill (router bit) going an inch deep, but using a 0.020 WOC and a 0.065 step down. Works in both 7075 or 6061. Sounds like at the lower feed speeds you are just rubbing rather than cutting.

[CL_MotoTech]

Just for experiment sake, do higher tool loads create a closer to modeled dimension?

[DJEkim33]

Made another small part with both interior pockets and exterior features the other day. This time using 6061. The interior dimensions were almost dead on to spec but the exterior was not. It was off .003" per side. I had a bunch if different feeds and speeds programmed in to check things out and the exterior cuts we're a lighter WOC than the interiors.

What I came up with is that this cutter likes to take wider WOC cuts to stay happy, over .020" on the finishing, anything less did not come out to spec. DOC was not nearly as important as the WOC.

I ended up cleaning up the part with a 1/4" carbide end mill that had no issues getting it to spec.

My thinking is that the high helix Niagara needs to be run faster on a more rigid machine and me having it sticking out 2" from the holder is not helping. Probably just order a regular carbide in the length I need to do the parts I started.

[lcvette]

What's your backlash for each axis? I found that the machine will move under cutting regardless of backlash compensation. The other thing to consider is slowing your RPM down. Use the tool by ramping down the finish pass, reduce the cutting forces on it to stop it from rubbing/bouncing. If it deflects at all at full depth it will rub which will skew part dimensions. 2" of stick on a 3/8" tool is alot in hard material like 7075. I sometimes use a roughing ramp down pass and dimensions are some on and finish is super nice!

Sent from my QTAIR7 using Tapatalk

[DJEkim33]

Backlash is .001" and compensated for. I ordered a YG-1 Aluminum Power and gave that a try with similar results. I have tried all the ramping options and changed in feed and speed you mentioned except slowing the RPM down. I will say the YG-1 did perform a bit better overall.

I am writing this all off as a rigidity issue between the machine and stick out. Long term plans are to scrape the ways and do a column reinforcement that integrates the z into the base of the machine. In the short term I plan to divide this into two operations. Since I have a collection of 3/8 end mills now I will choke up on one for the bulk of the work and use the long one only for the spot that needs that reach.

[lcvette]

How about your steps per inch setting? I have seen where people do this setting measurement in a way that doesn't accurately reflect actual machine movement. This can lead to all sorts of tolerance problems. I myself did this incorrectly many moons ago and it baffled me for sometime before I was instructed to try a different method which resolved many of my finished part tolerance issues.

Steps per should be set over at least a 6" span using a precision ground block. I also like to set backlash with the same block over 6" to remove any section from the equation. Because when cutting the machine is usually in a state of constant motion, suction rarely would be influencing actual cutting tolerances. So eliminating it during setup will get your machine closer to true movement than small single step moves would. If you have not done your setup this way I would recommend giving it a try.. also be sure the ways are lined will during deep as if you were preparing for cutting a job. Vactra#2 is pretty amazing for slide ways and I found I had to reset my settings for backlash comp after seeing from regular oil.

I have the same machine and can tell you it isn't a rigidity issue with the machine as I can hold .0005-.001" if I have to by playing with feeds and speeds and finishing passes. It's definitely some thing amiss mechanically or in the steps per I would guess to p be off that much. How is your spindle runout and vibration? Removing vibration and running with good bearing (Nachi tapered roller, not crappy AC bearings, will help tremendously if you aren't running them. Also what belt drive? Timing pulley setups are bad for vibration..

Maybe some is your setup?

Sent from my QTAIR7 using Tapatalk