Machining Gasket Surface (32-64 Ra)

Hello. I’m looking for some help on a new job.

Having an issue getting a consistent finish across the whole face of the part.

Customer is calling out a 32-64 Ra surface. I’m curgently running a fly cutter with a 1/32 rad tool (brazed carbide tool from McMaster), and I’m getting a very inconsistent finish.

Parts are round, front and back (y axis) is around 20 Ra lower (around 42 Ra measured 0 and 6 o’clock, around 60 at 3 and 9) then left to right (x axis). Taking a .005” cut, 1000 sfm and 21.5 Feed. Tool is around 4” in dia.

I’m open to suggestions to other tooling as well, keep in mind this is a very high volume job so the right tooling for the job would help.

Thanks in advance.

What is your material and what kind of machine are you doing this on?

I would think 1000sfm is too fast in anything but aluminum, and if you're getting weird surface finishes, the first thing I would try would be to slow down the rpm.

I suspect your flycutter combination, whether at the round shank or brazed shank, is flexing and "bouncing" as it goes around.


If it is a high volume job, I would lose the brazed carbide and get something inserted. I would suggest a 4" facemill with all but one insert removed. Although to be honest, I think I could get a 64 micro with all the inserts in a facemill.

You don't want to be doing lots and lots of parts having to change a brazed bit and re-measuring every time. Inserts are quick to flip.

A fly cutter makes one scalp per each revolution. You can calculate how much travel there will be per revolution and pretty much know what the surface finish will be. Yes, then add chatter and the like...the larger radius makes the surface finish better.
Considering the balance of a fly cutter is another factor for surface finish.

A mill face cutter with a few opposing teeth indicated to near zero will reduce the distance between scalps, and only vary to how close you indicated.
The old Valenite value mills were good for matching/plate checking a mill cutter face to set individual inserts matching to near zero.

For dead pocket mill cutters, one might use a set of shims .008 .009 .010 ..and if having a surface grinder grind a few at .0075 .0085 .0095.. because thicker shims are easier to handle.

I've done similar jobs with a 4" Kennametal face mill with every other insert being a wiper insert. - This was in Cast Iron. Contact your tooling supplier for recommendations.

Which cutter? I've seen a lot of junk brazed carbide.

Consider that a mill cutter might have 6 cuts in one rpm, whereas a fly cutter has only one, .but yes it may have a few mill cutter passes on a wide part/head.
The best engine head machine I have seen has a diamond bit with a fly cutter action that makes a wider cut, perhaps a small section of a 1/2" radius cutting the surface. You might try that with having a very smooth edge carbide or HSS cutting edge, perhaps ..003 negative land on a cast iron part ..and a positive rake edge on an aluminum part...and have the fly cutter very well balanced.

A face mill cutter can be more balanced than most fly cutters, having the mill cutter full of inserts for insured balance, and one insert .003 higher than the rest gives the fly cutter finish. Having the high insert (inserts) specially ground to a small section of a 1/2" or 1" radius facing the part may give the best surface finish..but yes it may not be good for high stock removal.
Grind such a blade/insert with a 220 or finer grit wheel, best wet grinding.

This kind of insert grind can be done on a surface grinder using the OD of a diamond wheel buy locking the long travel and setting a block on the mag chuck to act as a table and set at the height that gives 7* clearance to the cutting edge..done by hand turning the insert to the wheel and using a radius gauge.
Yes, you may have two or more opposite inserts in the face mill but then they should be height set with a surface plate check/set.

Yes, the face mill does not have to be fully loaded with inserts, pockets can be empty as long as opposite pockets have an insert so to insure balance. *and set and lock height design.

I think the surface finish will vary across the width of the part due to chip thinning. The closer the flycutter diameter is to the width of the part the more roughness variation you will see from part center to edge. Can you post a pic of the part?

1000 SFM is really pushing it for a flimsy HSS shank flycutter. Also 21.5ipm at 1000sfm on a 4 inch tool is .022ipt which is WAY too much. I'd back off to 650sfm (620rpm) and set the feed to about .003-.005ipt (2-2.5ipm) and see what happens.

Or even better get an inserted bar for your flycutter and use the appropriate insert for the material you're cutting, easy peasy, they give you the speed and feed to run.