Is this facing finish normal?

[michiganbuck]

If all the inserts were cutting then the feed rate might be divided by the number of inserts. If one insert was high the lines would be one feed rate apart, as from that one insert..
Good to plate-check a set-up cutter and add lifting shims to make all..or at least two opposite inserts the same height.

Good for this thread if the Op would fill a cutter with inserts, and then indicate the height of all the inserts... Then reset inserts to .001 or less and run another part.

Still, at the big shop, we had lines that could not be eliminated with the best height setting/grinding to tenths and indicating the cutter circle. We called them rotation lines and blamed them on the balance of the cutter or spindle assembly. the lines would not show on a tenth indicator but were there for visual observation.

 

[Ox]

He did.


------------------

Think Snow Eh!
Ox

 

[MiniMillMachinist]

IMO, it could be some subtle imperfection in the lead screw. Again, nothing is perfect. The error needed to cause a visual effect can be really small and below any numbers the manufacturer would be willing to guarantee.

Makes sense - thanks for the input! I guess I'll leave as is as it's a 9 month old machine and hasn't been crashed (yet...) so should be in spec.

It does make it sound a little like ballscrew error, but whether it's worth pursuing I doubt. In theory the linear bearings should be stiff enough on their own to mask minor perturbations of the ballscrew, but as the saying goes, everything is rubber...

Agreed, I think I'll leave this one alone. Appreciate your input into the thread!

people strive to GET that finish !!!
nice work

Thanks for the input - appreciate that!

Are you getting the same pattern in steel with steel inserts, or is it just non-ferrous with non-ferrous inserts? (I assume that you are using the correct insert for the material ) It would be interesting to see if you get the same with a fly cutter on brass using hss and zero rake. That would tell you if it is tool pressure related. Some non-ferrous inserts tend to be a bit grabby in brass.

I've not actually faced steel with this machine as it works exclusively with brass and aluminium at the moment. One of the face mills I have is positive rake and one is negative - personally I think the positive rake gives a cleaner looking cut for the same feed per tooth. I am curious to try with a single insert though so I'll give that a go.

I used to put a small flat on an end mill end outward place near the corner ( the distance of one feed per rev) to blend in that effect, a small radius can also help eliminate it, and a dulling tool that has suffered a small wear land helps eliminate it...
Not much way to get away from with not having a slight scalp cut in one pass travel to the next by deliberately setting a tad out of tram.
less end dish on an end mill end allows faster Beak-in making the slight wear land flat.

Very accurate end mill end sharpening (or setting inserts on a mill cutter) so one tooth is not high is another important thing to consider.

Thanks for the suggestion - essentially you added a wiper by creating the flat? I can always try a larger radius, I think the inserts I have are 0.4MM and 1.6MM. BTW, all the inserts were tweaked to be within 3-4 microns, I rotated the spindle and probed the tool setter until it looked good. I find that having one or two inserts 10-20 microns extended versus the others actually masks the effect seen in the original photo, but reduces the overall shine of the part, so a tradeoff for sure.

 

[MiniMillMachinist]

If all the inserts were cutting then the feed rate might be divided by the number of inserts. If one insert was high the lines would be one feed rate apart, as from that one insert..
Good to plate-check a set-up cutter and add lifting shims to make all..or at least two opposite inserts the same height.

Good for this thread if the Op would fill a cutter with inserts, and then indicate the height of all the inserts... Then reset inserts to .001 or less and run another part.

Still, at the big shop, we had lines that could not be eliminated with the best height setting/grinding to tenths and indicating the cutter circle. We called them rotation lines and blamed them on the balance of the cutter or spindle assembly. the lines would not show on a tenth indicator but were there for visual observation.

That sounds similar to what I'm observing here. Did you ever try a wiper insert?

 

[Digital Factory]

The nicest finish I've ever gotten with a facemill was on a very heavy box way machine... 8" diameter Mitsubishi AHX-640S facemill cutting steel, zero cross hatching and zero movement when sweeping with a tenths indicator.

The machine was not nearly as capable in other areas as the DMG Mori 50-taper horizontal right next to it, but the finish could not be matched.

The finish you're achieving is quite decent. You'll just need to temper your expectations with what can be achieved with a Haas Minimill.

 

[BT Fabrication]

Side note, but does anyone have experience with the Sandvik R590 face mills? Tempted to try one out with a wiper but they are a small fortune.

yep got a few of them, but to cut you can't baby them. needs min 8 thou fpt and cuts like butter.
your lines are all from tool deflection or machine deflection. 90 degree cutters push everything sideways. if running this thing in a mini mill, 2" is like a Bridgeport does, just too much side loading causes vibration resonance and does the weird finishes, or you aren't feeding fast enough to make a chip and its welding to the tooth and dragging the cut.

 

[MiniMillMachinist]

yep got a few of them, but to cut you can't baby them. needs min 8 thou fpt and cuts like butter.
your lines are all from tool deflection or machine deflection. 90 degree cutters push everything sideways. if running this thing in a mini mill, 2" is like a Bridgeport does, just too much side loading causes vibration resonance and does the weird finishes, or you aren't feeding fast enough to make a chip and its welding to the tooth and dragging the cut.

That sounds ideal. What I find with the 90 degree cutters that I have is that the cutting edge will break if I try and run 0.2MM/T - 8 thou per tooth. Typically I run it at 0.125MM/T or 5 thou. The 45 degree face mill I have can take a more aggressive cut without the tips going. On an R590 it'd be £20-30 per insert so I'd definitely want to get it right! BTW, these lines are most prominent in light cuts, i.e a 0.2MM stepdown

 

[BT Fabrication]

a mini mill doesn't have the weight to push 90 degree cutters to full depth on a 2" face mill. only does id bet 3/4" holder about 50-100 thou wide and 100 thou depth. all 90 degree will only rub if not cutting deep enough, then wear the edge off, then start rubbing and leaving streaks like that.
why, the edge radius is larger then the depth or fpt you are taking.

 

[MiniMillMachinist]

a mini mill doesn't have the weight to push 90 degree cutters to full depth on a 2" face mill. only does id bet 3/4" holder about 50-100 thou wide and 100 thou depth. all 90 degree will only rub if not cutting deep enough, then wear the edge off, then start rubbing and leaving streaks like that.
why, the edge radius is larger then the depth or fpt you are taking.

That's interesting, I run the 2" 4 flute face mill at 0.7MM depth, 30MM width of cut in brass at 3000RPM and 1500MM/M and the spindle load is only around 50% and the cut sounds fine - it's only on clean-up that I get these marks, when I take a very light cut. I'd actually go heavier but because my parts vary in size and I don't want to kick the parts out of the vice and I'd like to keep the same template I limit the depth to 0.7MM. I actually think the heavier cut looks better because the head moves enough that the trailing edge of the cutter isn't making contact with the workpiece and so I don't get the pattern every 6MM.

 

[Milland]

Why not program a heavier final pass? That's after all the stock removal bar finish is done, so no worry about kicking the part from the vise.

 

[MiniMillMachinist]

Why not program a heavier final pass? That's after all the stock removal bar finish is done, so no worry about kicking the part from the vise.

Cheers Milland, that's what I've started doing now! I prefer the look overall I think

 

[michiganbuck]

Tool geometry can reduce cutting forces. Some materials can well up (mush) so the cut is not the only or last action, some cutters run out of balance at 3000RPM, some insets are not very sharp when you look at the edge at high magnification, some holding devices hold a part poorey, some surfaces actually look worse when you get to the best surface finish because light reflection is amplified so small imperfections are seen better.
*What does a profilometer tell you about the finish quality?
We tried a much higher precision cutter on a part at the big shop and with it the part showed waves at about every half inch that made it look poor. The waves were not even measurable, so we went back to the old method
Some part specifications/prints ask for a ground finish just to rid such markings.

 

[BT Fabrication]

That's interesting, I run the 2" 4 flute face mill at 0.7MM depth, 30MM width of cut in brass at 3000RPM and 1500MM/M and the spindle load is only around 50% and the cut sounds fine - it's only on clean-up that I get these marks, when I take a very light cut. I'd actually go heavier but because my parts vary in size and I don't want to kick the parts out of the vice and I'd like to keep the same template I limit the depth to 0.7MM. I actually think the heavier cut looks better because the head moves enough that the trailing edge of the cutter isn't making contact with the workpiece and so I don't get the pattern every 6MM.

0.7mm depth is only just over 20 thou, that is really light depth of cut for it.
3000 rpm is only 282 sfm, which is slow in brass.
1.5M per min is 4,921 RPM, so which is it?
at 4921 its 0.82mm per tooth on 4 flute. which isnt much.

 

[MiniMillMachinist]

0.7mm depth is only just over 20 thou, that is really light depth of cut for it.
3000 rpm is only 282 sfm, which is slow in brass.
1.5M per min is 4,921 RPM, so which is it?
at 4921 its 0.82mm per tooth on 4 flute. which isnt much.

3000RPM with a 50MM face mill is over 1500 SFM, or 471M/M, my feedrate is 1500MM/M - see attached

 

[BT Fabrication]

P
fpt 0.28 mm(0.2-0.35)
sf 260 m/min(265-250)

sandvik recommended values on a face mill, like i said, feed per tooth is low and rpm is higher than recommended. need 2-3x feed
others are in the same ball park for a general face mill on non ferrous