speed/feed sugestion

[Surface]

I think this outside-radius is costing me too much money. I am hoping someone can offer a suggestion to get more parts per tool or a less expensive method to do this.

I am machining a .203R along the length of a part using a 5/8OD (.218 tip) uncoated, solid-carbide, 3-flute, corner-rounding-tool. Plenty of rigidity and coolant. Cutting HRS.

I'm running this tool at 2300rpm([email protected]) and 9ipm (.0015 fpt).

I'm currently getting about 100 linear feet before the cutter is dull.

Each part requires 19 inches or radius and at $150 bucks for a double ended cutter, it is costing me $1 each to machine the radius.

Any sugestions?

[masterp]

if surface finish allows i would double you feed rate. your current .0015 fpt is not alot. Have you looked for TiN coated cutters?. This will increase your tool life and cost. I would expect at least

2 to 3 time the tool life with a coated cutter.

[Guest]

I also might look for something insertable as well.

 

[Storkman]

We use a line called Superbee. It is and indexable cornerround. They seem to run forever in 400ss.

[HevyMetl]

Uncoated carbide should not exceed 200SFM in HRS. This material sucks by the way due to inclusions and hardspots which are exceptable in the process. You should also increase you chipload and only use air for coolant. If you use water in will cause thermal stress cracks in your sharp cutting edge which results in premature failure. One of the problems with that cutter is where you do figure your SFM. You have many different diameters and based off of where you figure you will be running too fast or too slow.

 

I would look at HSM milling with a ball mill and adjust your stepover to get you where you need to be surface finish wise. Do not exceed a .02 x Ø (.0075) doc with a .05 x Ø (.01875)stepover. I would run a 3/8" ball mill TIALN coated at 10K at 120ipm. This is a pretty good High speed machining application and the cutters are easily obtainable through OSG, SGS, DATAFLUTE, ect. Look to your supplier for recommended speeds and feeds. We have stopped buying all specialty cutters (except on rare ocassions) and try to do with a ball or bull nose endmills off of the shelf.

 

 

Inserted is also way to go if you have the application and volume to support it.

[Surface]

Thank you all for time and your input. Your expertise and experience makes the MC-forum such a valuable resource. They are all good suggestions.

To see the exact application, I put a file on the FTP. (Multi pole coil.MCX)in the MCX-directory.

 

HRS is crap, but I was afraid CRS would curl when facing. (BTW; my facing-problem was answered yesterday. Thx Kannon) Therefore I am looking at #3000 lbs of HRS and if I can make money on this job, there are plenty of these parts to make. I don't mind investing in tooling.

The reason I chose a specialty cutter, over a ball-endmill or even an indexable, is the radius terminates in a sharp corner. I couldn't find an indexable cutter which wouldn't cause a different specialty-cutter-issue, and a ball-endmill required moving up-and-down the radius rather than along.

I'm going to try a TiCN coating on this tool, with identical speeds and feeds. I will report any increase in tool life.