Facing and getting a FLAT surface

[SRT Mike]

We have a block of 6061 AL that is about 3.5" long and about 2.5" wide, about 1" thick.... mounted in soft jaws on a vise. Using a 4-flute 3/4" DIA endmill, making 5 passes or so on the top, you can feel a prominent ridge between passes. I want to finish these parts in a vibratory bowl so the flatter I can get the top, the better. The final pass is only about 1/8" depth of cut.

I figured using the 3/4 mill would reduce deflection but we still get pretty big ridges between passes. The max tool diameter on the holder is 3.5" I believe, so I can't go using some huge flycutter, and while 3.5" would help on this part, it wouldn't help as much on other parts in the future.

I'm thinking the problem is maybe due to the head not being 100% square to the table, or possibly deflection within the part (we do pocket it so it loses a lot of it's mass before the final finish pass on the back). But I'm not sure those problems are entirely fix-able.

Any other suggestions to getting a better finish? If a flycutter, anyone suggest a brand/model for 6061? What about doing finish passes front-to-back in Y instead of side-to-size in X? That would perhaps make a smooth transition if the head is not 100% square rather than the more ridged X-axis passes, no?

Any other suggestions are appreciated. We're not talking big deep gouges here or anything, just you can easily feel it with your finger if your rub it back and forth over the part.

[Mcgyver]

the head needs tramming, but don’t take my guess as gospel, put an indicator in and check. Most mills get knocked about enough to come slightly out of square over time – using a tenth’s indicator is my preference…not that anyone mills to tenths, it’s just that the error is magnified and easy to see.

you say you're not sure adjusting the head is possible??? there is no way to adjust it? if not you've got to find way to shim to square. fly cutting might avoid the ridges, but if the head is out of sq so will the cut be, the has to be a way to fix that

while .125 isn't much of a cut, it could be enough to cause some deflection (what type of machine), try like 10 thou - what happens. like i say, my bet is the head is out of tram but if you are worried that it might be deflection, try a lighter cut.

ps if really can't square the mill and you're not making millions, why not just cleaning it up with a file?

[Geof]

What Mcgyver says is most likely the case, the head is not perfectly true. And sometimes depending on the machine it is very difficult to get it true enough that you do not get detectable ridges as you describe.

As a side comment it can be surprising how sensitive fingetips are, you can probably feel a 0.0005" ridge maybe even less.

So try to go around the problem. Buy or make yourself a flycutter large enough to take a finishing cut spanning the full 2.5" width. You can hand sharpen a high speed tool with a good rake, Mcgyver may remember a picture he posted a while back and give you the link. Take off only a few thou and you should be able to get a very nice finish.

[SRT Mike]

Thanks for the feedback. I agree that the fingers can detect very slight variations - I don't think it's THAT far off square, but it is a little off. I am sure it's technically possible to fix, I just don't know how off I am from truly square, and I am not sure it's something I'd be able to do myself (and if I couldn't, I'm not sure it's enough of an issue to justify calling in a repair guy). The machine is a V-40 (40"x20" mill) so it's a pretty big and beefy machine.

The main issue is that I was hoping to automate the finishing of the parts in a vibratory bowl, and if I leave them in the bowl long enough to remove the ridges, it will also break the nice crisp corners we've machined and soften the lines up more than I'd like. If I could reduce the ridges, I could probably just toss them in the vibratory bowl for a shorter time and the flat portion would be smooth without breaking all my corners too much.

I will be doing these in batches of about 50 at a time (50 fronts, 50 backs, so say 100). Thats about once every couple of weeks. Its not a ton of effort to manually remove the ridges but better if I could avoid it

I use a palm sander now with 220 grit paper to remove the larger machining marks, then sometimes go to 320 grit for a smoother (brushed-look) finish. Any other/better tools to quickly remove the ridges than a palm sander? I have a random orbital sander too thats a big bigger than the palm, and I have a pretty industrial strength belt sander.

[davereagan]

I would never expect a perfectly flat surface when taking .125" depth on the final pass. I would try .005" like suggested earlier. I think that is your only problem. Higher helix endmills work better in aluminum and other materials as well. If you are currently using a 30 degree general purpose endmill, you'll love a 3 flute 45 degree helix endmill.

Dave

[DonutSlayer]

I doubt you will ever get a perfectly smooth surface using a endmill and multiple passes, at least I've never seen it done, like said above make very small finish passes, I saw some parts once that were finished that way but they used a S shaped finish pass to break up the straight lines and give a cool look to the part.

[RdHawg]

Another alternative - although a lengthy process - use a ball mill and spiral out from the center. Control your finish with your step over. I do it sometimes if I have another job I'm working on another machine. If I'm not there the machine sits idle anyway, so I reclaim the time in a nice finish.

[daking]

Why not use a flycutter? Use a good sharp tool with positive lift and good clearance. Leave .005 t0 .010 for a finish pass with the flycutter. We make our own flycutters. 3/4 or 1" shank with a 3/4 or 1" body-dia. to suit. Cut a slot for 1/2 tool like an AR8 or a D (V shape). Tap for a couple of set screws and you're in business. We finish similar parts this way time. If your head is not square it may not be flat or parallel but you wont have cutter mismatch and the finish should look real nice.

Dave


Edit: I guess Geof pretty much said this already. In that case "What Geof said"

[Caprirs]

No fancy repair guy needed to square up the machine. It can be done with a wrench, a good .0001" indicator, and an understanding of what is happening. A lot of folks don't realize VMCs have to be installed correctly to achieve the advertised accuracies. Having the riggers set it in place and bubble level is okay for some work but if you need precision, you need to spend another hour doing the detail work.

The quick check is put the indicator in the spindle and hold it such that you can sweep a fairly large circle like 6". Bring the head down and sweep the indicator on the table (not a vise, not a fixture). On a decent VMC, you should see less than .0005" variation across the 6" sweep. If you get more than .0005", the head/column is not square to the table/saddle/base.

Use the screw jacks in the base of the machine to control the flex. Start will the machine sitting on only the corner screws and perform a bubble leveling of the machine. Once it's square to Mother Earth, then you have to adjust for the flatness of the floor it's sitting on. Based on where the indicator sweeps high or low, use the middle screws to control the deflection of the base of the machine. You'd be amazed how little changes in the screws will affect the squareness of the machine.

See attached illustration which I've greatly exaggerated for visualization. The bigger the machine, the more pronounced the effects of an uneven or settling floor. On big HMCs like Niigata and Makino, there are like 20 screw jacks that have an effect on the column's perpindicularity to the workpiece.

[mark c]

I've had good luck on a machine thats slightly out of square, doing a spiral cut from outside in, taking .010" or so finish pass, with 50 or 60% stepover.
HTH

[joecnc1234]

What kind of feeds and speeds and tool are you using? We do what your talking about everyday the only diffference is we leave .010" for finish pass.
You can hog off as much material as your machine will allow then leave .010"
for finish. If this still doesn't work go with a flycutter or shell mill.
Joe

oh we also use a DA with 240 grit paper for a real nice blend.

[SRT Mike]

Thanks for the suggestions! I have the machine perfectly level (used a machinists level) - the thought of adjusting the screws to try to control the flex makes me cringe after how long we took to get it perfectly level The floor in the shop is pretty damn flat and it's poured in squares - we made sure to keep it all within one square.

I will try the S-shaped finish pass - sounds like a neat idea. Sure I can use a flycutter, but the only issue is that this particular part is juuuust small enough to cut with one pass from the largest flycutter my machine can hold, but there could be cases in the future where I need a larger part. I will try dropping the finish pass to .005 or .010 and see how I do. I will also try some different bits to see how I do. I am thinking of those Dataflutes mentioned in other threads and see if they are as good as claimed

I've seen folks get practically a mirror finish on a DMG with a 30k spindle. Maybe I am expecting too much (I have a 6k spindle).