Haas VF2 surface finishing issue

I’ve got a 2009 Haas VF2 7500 rpm coolant induced spindle. I have some weird issues with surfacing material. I machine a lot of aluminum but have noticed it on bronze and various steels.

I recently had a Sumitomo rep come by and I tried a 45 deg angle insert 3” tool for facing material. We ran a wiper and got a pretty good finish. But they suggested I try their 90 insert 3” tool cause it is known to produce a better finish. Tried and never could get it to face clean. Always had a fish scale look. The faster feed rate it improved but was still there. Inserts that were PCD sharp or Diamond.

I originally inquired about their HF cutters that are designed specific for aluminum, they leave no burrs and have basically a mirror finish. They are extremely expensive compared to traditional model cutters by any brand. They decided to send over one since that’s what I originally wanted to try. It wasn’t producing results like it should. So that’s the point I decided to have a Haas tech come inspect the machine.

We checked the draw bar pressure, it was 1700 (spec range is 1600-2300) they said no way they would change that out. Checked the spindle bearing preload. Checked backlash in all axis. Spindle taper looked great. My new Maritool holders have no bad wear showing. Only about two years of use on them. Machine is solid and level.

We’ve tried facing coolant induced, normal coolant nozzle, and air. No real change. Coolant induced seemed the best. I’m scratching my head. Haas tech can’t find anything wrong with the machine.

Has anyone had anything like this happen before? Tried various DOC and Feeds all starting with the recommended parameters for each tool.

some cutter types give better or worse finish at certain sfpm

DMF_TomB said:

some cutter types give better or worse finish at certain sfpm

Click to expand...

I was working directly with the tool rep in my shop and we started with their recommended speeds and feeds and then tweaked things from there. And also were emailing images to their head application engineers at the headquarters. They were confused by the results too.

I’m getting better finishes from my $40 Chinese facemill on an old fadal.

If there’s nothing wrong with the spindle do you maybe have an issue with the table rocking or not being quite as stiff as it should be?

This would be a great time to try out a small accelerometer and recording oscilloscope. Place the accelerometer on the spindle housing nose as close to the cutter as possible (to the right, to avoid tool changer conflict), then record various RPM and feed rates, comparing the vibration outputs to the resultant surface finish of the parts.

Do the same with the accelerometer on the table or vise, this gives you another set of data as to whether you have resonance through the machine base or have potential tuning issues with the servos.

Or just say the heck with it and bead blast all the parts.

Sounds crazy but is your tram in ? Check that. If the machine took a hit something could be off. Check your ways if the guide ways have rust spots you can have trouble like this, Don't ask me how I know but it costs almost $9K for new X axis guide rails. Are you roughing then taking a light finish pass ? Looks like it relaxes after the stock is off and drags on the far side as the cutter passes over.

Make Chips Boys !

Ron

We just went from my old faithful 2007 VF-2ss to a brand new Brother R650. One thing that has us scratching our heads all the time is how much better our finishes are in the Brother. You know, in that weak ass 30 taper machine [/sarcasm]. It's almost comical how much better this 30 taper does than the Haas ever did.

Face it, you own a Haas. The finishes you show are very typical in my experience. There are things you can do to help: Smaller tool. A 3" facemill is too large for your machine in my experience. Or maybe a free-er cutting insert would help. Larger chip load and / or larger DOC can help too. Also make sure you indicate the bottom of all the inserts so they match as close as possible. I've got extremely nice finishes on our Haas, but you have to do your job perfectly and the moon has to be in the correct phase for it to happen.

Dupa3872 said:

Sounds crazy but is your tram in ? Check that. If the machine took a hit something could be off. Check your ways if the guide ways have rust spots you can have trouble like this, Don't ask me how I know but it costs almost $9K for new X axis guide rails. Are you roughing then taking a light finish pass ? Looks like it relaxes after the stock is off and drags on the far side as the cutter passes over.

Make Chips Boys !

Ron

Click to expand...

I haven’t checked Z tram to the point where I use an indicator. But the problem doesn’t improve in direction of pass. So it’s not kicked up significant one side or the other.

But even the best photo of the ones I have attached, the very edges are flaky looking. Instead of a perfect pass with clean feed lines. I have it programmed to extend pass the part completely.

Yes it does seem to relax and drag on the far side. I take roughing passes when necessary. But mainly just doing testing of a specific depth of cut one pass the problem is there. The three tools I have tested with them can go over .200 DOC. But we test anywhere from
.005 to .03+ with varying feed rates and the induced coolant.

Matt@RFR said:

We just went from my old faithful 2007 VF-2ss to a brand new Brother R650. One thing that has us scratching our heads all the time is how much better our finishes are in the Brother. You know, in that weak ass 30 taper machine [/sarcasm]. It's almost comical how much better this 30 taper does than the Haas ever did.

Face it, you own a Haas. The finishes you show are very typical in my experience. There are things you can do to help: Smaller tool. A 3" facemill is too large for your machine in my experience. Or maybe a free-er cutting insert would help. Larger chip load and / or larger DOC can help too. Also make sure you indicate the bottom of all the inserts so they match as close as possible. I've got extremely nice finishes on our Haas, but you have to do your job perfectly and the moon has to be in the correct phase for it to happen.

Click to expand...

Man I was concerned about a 3” tool being to much for it. But I see a lot of my machining friends with the same machine have amazing results with these tools or Mitsubishi is a popular favorite for mirror like finishes. I have indicated the inserts on the tools that is possible to do that on. And I use the sharpest positive cutting inserts possible. Larger chip load and doc it does improve. It’s worse when you only have .005-.01 DOC and high sfm and low ipm. It feels unacceptable of a finish honesty. But I want to try to figure out what it could be if anything with the machine that could contribute.

clayton said:

I was working directly with the tool rep in my shop and we started with their recommended speeds and feeds and then tweaked things from there. And also were emailing images to their head application engineers at the headquarters. They were confused by the results too.

Click to expand...

.
.
listening 100% to your tooling rep is your 1st problem
.
we had recommendations from tooling rep and we got near mirror finish for about 2 minutes which obviously good for tool rep selling inserts
.
we did some testing at various settings with and without coolant which probably is 10,000% more testing than tooling rep ever did. after 100 tons of limited testing said
above critical threshold sfpm (550-600 for steel, cast iron)which varies depending on material and coolant use we get shiny surface for short period often less than 5 feet, then we get instability and after wear in period done we get a dull more stable finish. also at higher sfpm it takes 0.2 to 1.0 in from edges for cutter to warm up so sometimes not shiny near edges. so shiny mirror finish is more unstable. and yes we tried changing inserts after less than 5 to 10 minutes use. gets to point refuse to change inserts that often
.
if below 500 sfpm its normally dull but more stable finish. sometimes some minor bands or variations in dullness which if go below 450 sfpm generally gives a more even dullness. slower is more stable
.
so are data has recorded "maytag" settings. if we want dependable works every time we use them. if we want mirror finish and deal with instability problems which often consumes hugh amounts of time and inserts we can always go fast.
.
smart operators read sfpm and ipt and often just run 60% rpm 70% feed and are done 1st time and new guys try running 100% of tool rep settings and recut a few times and change inserts 300% more often. smart operators often dont say anything as not worth effort. had tooling rep recommend 943 sfpm on carbide inserts for cast iron. sure it works a few minutes then looks like crap unless you change inserts. good way to sell more inserts

See the micro vibrations. That can be cause by many things. Taper, spindle, worn linear way casettes, loose part, loose vise or vise jaw.

Speedie said:

See the micro vibrations. That can be cause by many things. Taper, spindle, worn linear way casettes, loose part, loose vise or vise jaw.

Click to expand...

.
thats basic apprentice stuff if part vibrating try going slower. my point is i would try various sfpm and see if it goes away. usually with finish cuts you maintain a .0030 ipt or whatever is minimum recommended for inserts as less ipt have little effect at certain minimum levels
.
other anti vibration trick is if 6 insert cutter take 3 inserts out and run 1/2 feed. that is common when part or machine or long tool holder is vibrating

Look at what he is running and look at the surface finish. He should be able to run .001-.030 ipt from 1000-10000 rpm in that aluminum. The vibration is a dead ringer. He even has a bad finish on his soft jaws.

Take and indicator on the spindle and see if you can pry a few thou left and right.

Speedie said:

Look at what he is running and look at the surface finish. He should be able to run .001-.030 ipt from 1000-10000 rpm in that aluminum. The vibration is a dead ringer. He even has a bad finish on his soft jaws.

Take and indicator on the spindle and see if you can pry a few thou left and right.

Click to expand...

I tried pushing on the spindle with a tool in and with orient spindle on it would shake if I barely twisted the tool and was difficult to get any real reading. Didn’t look like it had any measurable slack. But I also checked the bearings with the Haas tech and he pryed up with a 2x4 on the spindle dogs and it came back to zero on the indicator no problem.

How would you pry exactly to test?

You can take a regular toolholder, and put the indicator needle on the OD of the flange or other concentric part of the body. Then arrange the vise in a position that you can use it as a fulcrum when placing the 2 x 4 either against the side of the holder opposite the indicator, or at the bottom of the holder when testing Z play (needle now locating off the underside of the flange).

Milland said:

You can take a regular toolholder, and put the indicator needle on the OD of the flange or other concentric part of the body. Then arrange the vise in a position that you can use it as a fulcrum when placing the 2 x 4 either against the side of the holder opposite the indicator, or at the bottom of the holder when testing Z play (needle now locating off the underside of the flange).

Click to expand...

I’ve checked Z play. But I’ll try side to side like you suggested.

clayton said:

I’ve checked Z play. But I’ll try side to side like you suggested.

Click to expand...

Check Z again while you're in there, and try to estimate how much force you're putting on the lever, along with the ratio. Then record the displacement readings and talk with a good tech at Haas to see if they're reasonable.

There's some flex you'll get at the head due to the Z trucks giving a bit, you can get an idea of how much it's moving by using a second indicator on a solid portion of the head, and seeing how much it moves relative to the toolholder indicator. Maybe using the spindle housing is the best contact point, keeps it close to the same as the main indicator.

Milland said:

Check Z again while you're in there, and try to estimate how much force you're putting on the lever, along with the ratio. Then record the displacement readings and talk with a good tech at Haas to see if they're reasonable.

There's some flex you'll get at the head due to the Z trucks giving a bit, you can get an idea of how much it's moving by using a second indicator on a solid portion of the head, and seeing how much it moves relative to the toolholder indicator. Maybe using the spindle housing is the best contact point, keeps it close to the same as the main indicator.

Click to expand...

Haas tech placed it on the dogs with the indicator right next to the spindle taper surface area perpendicular to the table.

Would that slack cause issues profile finishing stainless vs aluminum and bronze? Cause I have a part I do for a customer in bronze. They wanted to try stainless so I changed tooling and speeds and feeds roughing all goes well. Then using a 3/4 5 flute imco endmill to finish the stainless it chatters and has so much harmonic sounding vibration no matter what sfm or feed or doc on the finish pass. I’ve used that same endmill though this one is brand new on A36. Its designed for stainless and titanium.

What’s odd is I finish with no problems on the 954 bronze same parts different speeds and feeds etc... but a 1/2” endmill. I have been scratching my head.

Have you by any chance tried facing the exact same part either with square (unchamfered) edges, and compared the results to the exact same part (and face mill DOC and path) where the edges have been chamfered first?

PM

clayton said:

What’s odd is I finish with no problems on the 954 bronze same parts different speeds and feeds etc... but a 1/2” endmill. I have been scratching my head.

Click to expand...

Try using a 1/2" endmill on the stainless too. For lack of a better way of putting it, the smaller endmill imparts less sideward stress into the cut (smaller "arc of engagement"), and given that Haas's are just not as stiff as more robust machines this makes it trickier to cut harder materials.

I've successfully cut 17-4 SS and 6Al-4V Ti on my VF-5, but I try to use 1/2" or smaller cutters when I do so. With Al (shiny butter) I can get away with much larger tooling options.