I am really needing to get a better finish. The vertical strides on the embossed ring on the part shown are my issue. Seems to show up in nearly all parts, some worse than others. I am highly suspecting the machine but of all 3 Haas VMCs, they all do it, just one is worse than the others.

Cut was from a 3/8 Imco streaker, 50ipm, 7500 rpm, .005 rad DOC, .300 axial DOC. What is strange is I get a much better finish in steel but Al just sucks. The helix on my cutters is 45*.

Attached Thumbnails

 

If it shows up in every machine my first guess would be you have some crap material.

Is it a problem exclusive to this run of material? Or does it show up everytime you machine Al?

Is your G-code actual G2/G3 commands or is it a bunch of segments? Just curious. I have seen surfaces like this because the code was segmented rather than actual arcs.

just a thought, it looks like the space of the high points are equal, if you change the rotation rate does the gap in the vertical strides get bigger? may be acting like a gear hob.

What happens if you do it at 20ipm?

Are you climb or conventional cutting it? Looks like climb and the machine isn't very rigid and the cutter is climbing the material. Try to reverse it and conventional cut it and see if it gets better.

Viper, I've run a few haas machines, and never had much luck with fine finishes at high feed rates & circ. interp. Are they even capable of it?

We have a Haas VF-1 and I can circular interpolate parts at 50-75 IPM with a good sidewall finish

Have you checked to see if the cutter is running out?

I would drop the rpms first if it was me.

I am going to go out and say your roughing passes aren't cleaning up fully. You can see the axial depth of cut on the finish. My guess is you are using an insert cutter say in the realm of 3/4" to 1" to rough out your part. If your inserts are not in the pockets right, or have a chip behind the insert they can easily cut larger than your .005" stock allowance. Your part is short enough that finding a decent cutter to finish in one axial doc won't be hard.

If this isn't the case... As was said earlier, check your code for actual arc moves and also verify the amount of stock removal you have. .005" of radial doc isn't much even for finishing.


Husker

I'm with husker on this one...looks like you used an insert tool for roughing and it's not cleaning up.

Check actual cutting diameter of your roughing tool and make sure you have G41/G42 applied properly, including your offset tables.

Check your roughing feedrate and check against how your "accuracy mode" or "high speed" mode is set up. If it isn't right...at high feeds the machine will interpolate a smaller radius than actually programmed.

Looks like faciting to me.

Looks quite similar to a lot of finishes I saw when inspecting parts that were made on Haas vmc's, I mentioned that before. A few other members here have also posted similar pictures before or talked about it, usually it was the machine, those SS series being even worse.

You should be able to kinda fight with it until it gets a bit better, assuming the cutter/holder runs concentric. The fact that it seems better in steel kinda tells you right there that there's a rigidity issue, conventional(just realized I wrote "climb" earlier) milling will usually keep the machine more loaded, higher cutting force. Also increasing that finish cut depth to keep it loaded can help. .005 ain't much.

Being as it is across multiple Haas machines. I would go with what Husker said, as well as make sure your finish pass is using arcs.

Also there is a setting in the control for how close it stays to the programed path (kind like a cut tolerance or something), I believe it can be set to fine, medium, and course. perhaps yours is on course and you don't know it. Mine is set to medium and does fairly nice. I can't recall which setting # it is at the moment though, will check later and post it up if no one else has.

Edit; Setting number 191 Default smoothness.

N1770 X-1.7514 Y.1764
N1780 Z1.1
N1790 G1 Z.68 F100.
N1800 X-1.7468 Y-.1985 F50.
N1810 G3 X-1.6709 Y-.2726 I.075 J.0009
N1820 G2 I.0209 J-1.7274
N1830 G3 X-1.5968 Y-.1967 I-.0009 J.075
N1840 G1 X-1.6014 Y.1782
N1850 G0 Z1.25
N1860 M9
N1870 G0 G28 G91 Z0
N1880 G90

Here is the bit of code that milled that OD. Yes, I used a 3" face mill to do most of the profile and had to clean up with an endmill just to get to a zero corner rad. The cut was climb and that is what I use 95% of the time. I am just at a loss to know where to take the machine for better finish. faster, slower, more or less material to load it, etc. Just always seems to do this regardless. I could not verify how much I removed on the OD but I measured the part after the face mill and it was .005 big and had a better finish. My feeling is that the 3/8 mill caused this.

My face mill leaves small circles like something is no perfect but the actual mismatch in the X is measuring about .0002. Probably cannot get too much better than that. I would like to see a better finish from the face mill.

This tool is done but I might just throw some crap material in there and see if I can find a feed/speed that works better. I have a part to do that must have a good finish or we will burn 10s of hours sanding them...

After the roughing operation paint the surface with dykem or even just a black marker. Then you can verify 100% that the end mill is finishing the surface.

I never finish at faster than 47ipm, the magic number that Haas setup the machine for the threshold of accuracy vs speed. My 1993 VF-0 would do a much nicer job than that, so it's gotta be the tool, the feed, the speed, or the radial DOC.

Well damn Perry, 50 is not far from 47....

I do seem to remember working with Haas on a surfacing issue where the machine was overshooting with a 1/8 mill so we tuning the 191 (?) setting for a better position check. They said it might slow the machine down. I said I was rather run slower than scrap parts even though it is embarrassingly slow....


Perry, are climbing, what rpm and such? radial DOC? I am using ER32 holders but kind wondering if there is an issue there. I seem to always find excessive runout when I test for it even though we can find no issue with the spindle.

I can pretty much promise you that it isn't a problem with the material.

1-verify your finish pass is cleaning up.
2-make sure your work holding is solid.
3-check tool runout
4-replace with NEW tool
5-change tool holder, collet, and nut.

...then worry about the machine.