[toyranosaur]

So Gents, I have a question I hope you can help with. I'm a newer machine guy, and have a prob with tool marks: When I cut a pocket in Aluminum (99% of what I cut is 6061-T6,) using a flat endmill, it leaves very shallow- About 1-1.5 thou- swirl marks where the tool enters & exits on the flat bottom (The rest of the area comes out acceptably.) It's like the tool has one low corner: I usually use fairly inexpensive tools, but tried some Accupro's & got the same result. I would like a finish that can be hand-polished without having to sand out the swirls first, if this is doable. Average pocket is .750 deep, 1/2" 2 or 4 flute cutter, carbide or HSS, on a brand-new Haas VF-3 running 10K RPM & around 22 IPM.

A related question, I see a round, flat Crystolon Machine Knife Stone in an MSC flyer, stating "....for sharpening and honing." Is it possible to lower an endmill by tenths/ a thou until it just hits the stone, thereby giving me a perfectly flat cutter? Forgive me if this is a bone head question, but I guess I'm a bonehead as far as this goes! Many thanks for any advice, Chris

[txcncman]

Z axis must be PERFECTLY perpendicular to X and Y axis movement.

[toyranosaur]

The machine is only 2 lightly-used years old, so I had to assume (I know....) that the Z axis is dead-on: Bein's it'll cost me a few hundy to get it checked/rectified, I'm hoping there may be some other factors at play. Largest tool I use is .5", & biggest piece I've made is only a few inches long, no crashes, so.....Of course, no one's machines are perfect, and this may need a touchup if no one has any any other thoughts. Thank you for your assistance Mate, I just hope you're not right 'cause it'll be pricey! Chris

[Lomach]

Have you tried dramatically reducing your spindle speed on the finishing pass say down to 1000 or 500rpm and feed rate to suit. It could be vibration from the spindle at high speed that is causing the finish. Any pictures would be a great help

Lomach

[kelef]

hei'ya toyranosaur, might help to check with DTI/clock, for spindle/Z, to table to check 90 degrees and from the table to spindle/tool rotation, if all comes out good then your slowest and lightest finishing cut to eliminate tool deflection, keep the tooling minimum length - my 2 cents- good luck :rainfro::rainfro::rainfro: kelef

[txcncman]

Maybe I should repeat, the Z axis must be PERFECTLY perpendicular to X and Y axis movement. If there is any misalignment of the Z axis being perpendicular to the X and Y axis during machining, you will get tool marks on horizontal surfaces. You can check "at rest" alignment with a dial indicator attached to the spindle and "sweeping" across the table surface. There are plenty of YouTube videos showing how to do this. Checking for tool deflection and other misalignment while cutting is almost impossible and has to be determined more by the results of the first test and what is witnessed on finished parts.

[RICHARD ZASTROW]

A typical end mill is not ground flat, it has a slight relief angle ground into the end. This leaves a very slight cone shape standing unless the end mill is run over the cone area.

I'll repeat what txcncman said. The spindle MUST be perpendicular to the table/workpiece surface. Otherwise the cutting tool will leave marks.

Dick Z

[neilw20]

1. Needs to be PERFECTLY square.
2. Try to do the finish path with NO Z movements as even repeating to microns will still leave visible marks.

Using feed patterns for constant surface speed will help,
If the cutter rubs in one place longer than another, it will end up slight lower and very visible.

Reflected light will show up even microns of irregularity.

Lots of flood coolant so the chips are not recycled, or a strong airblast.
As the cutter wears, the vertical load on the spindle will change also.

If the spindle is not up to temperature, you might see an extra 10-20 microns or more from cold to hot.

And there is no mention hear of vibration and many other factors.
Use super sharp tools for the finish pass.

[toyranosaur]

Tremendous, thanks Chaps! I'll get a picture up soon, but it seems you've given me some things to ponder as is. Great stuff! I truly appreciate your taking the time to punch the keyboard. Chris

[fizzissist]

Try endmills with radius'd corners. A .03 radius will work wonders.

A simple test to see if the spindle is out of tram (even for a fixed CNC) is to simply take a test cut in one direction, shift the tool over by more than the diameter of the cutter, and take a cut in the opposite direction..then compare the two cuts for surface finish. Do this in X, then in Y.

You could find that for your machine you'll get better finish cuts going in a particular direction. PITA, but that's life. I know it shouldn't make a difference, but ... that's life.

...And don't waste you money on cheap tools.

[txcncman]

Try endmills with radius'd corners. A .03 radius will work wonders.

A simple test to see if the spindle is out of tram (even for a fixed CNC) is to simply take a test cut in one direction, shift the tool over by more than the diameter of the cutter, and take a cut in the opposite direction..then compare the two cuts for surface finish. Do this in X, then in Y.

You could find that for your machine you'll get better finish cuts going in a particular direction. PITA, but that's life. I know it shouldn't make a difference, but ... that's life.

...And don't waste you money on cheap tools.

I was waiting to make the bull nose mill suggestion until some other issues were clarified. In addition, sometimes you can "fake" a truly flat bottom by taking very small step over cuts (i.e. less that 40% cutter diameter).

[fizzissist]

I was waiting to make the bull nose mill suggestion until some other issues were clarified. In addition, sometimes you can "fake" a truly flat bottom by taking very small step over cuts (i.e. less that 40% cutter diameter).

There are occasions where I need square corners at the bottom, so I go back in with a regular endmill about .0001-.0002" off the bottom, and clean up the radius corners. You have to look real close to see it.

I usually use a small step-over for finish cuts anyway, and I've always been complimented on my bottom.

[gateman]

There are occasions where I need square corners at the bottom, so I go back in with a regular endmill about .0001-.0002" off the bottom, and clean up the radius corners. You have to look real close to see it.

I usually use a small step-over for finish cuts anyway, and I've always been complimented on my bottom.

lol

[toyranosaur]

Excellent thoughts Gents, I'll be able to get out to the shop today & in the next 2 try a couple things suggested, starting with checking for spindle squareness. I shall let you know the result, but I have a good feeling that, bar a spinndle issue, some of these may work since the marks are ALMOST passable. What a great site, it's helped me before, and I'll hopefully pass on some of this to another guy one day. Mucho appreciado! Chris REC