Speeds and feeds for a 16 pitch gear cutter

I will need to make some gears using a HSS 16 pitch gear cutter. Can I
do ths with a water based soluble oil cutting fluid and what speed and
feed would you recommend.
thanks
i
Reply to
Ignoramus7187
Loading thread data ...
What diameter cutter?
Wes
Reply to
Wes
Assuming the general ~3" diameter gear cutter, and assuming you are making gears of relatively mild stuff, then about 150 RPM and about 5 IPM feed. But, just calculate it very much like an end mill.
Water-base cutting fluid should be fine.
Jon
Reply to
Jon Elson
I would say 3 inches.
i
Reply to
Ignoramus7187
OK, thanks. I may go lower on IPM, but it is a good start.
i
Reply to
Ignoramus7187
Well ... first I would need to know what metal you will be cutting. The cutter alone does not define the speeds. (And if you want RPM, we'll need the diameter of the cutter.)
As for the feed -- we would also need to know the number of teeth on the cutter -- feed is usually specified as feed per tooth, so the more teeth the faster the total feed you can get away with.
You can look these up in _Machinery's Handbook_ -- which is where I would go to calculate these once I knew the specifics of the workpiece material and the number of teeth.
Or -- if "some gears" does not translate to enough to make time consumed particularly important, I would aim for perhaps 50 to 70% of the maximum speed, and perhaps as low as 50% of the calculated feed. Those speeds and feeds are for a company turning out the maximum number of pieces in a day, considering the tradeoffs between the number of minutes per piece and the time lost to changing tooling. With the recommended speeds and feeds, it is *assumed* that you are willing to sacrifice some tool life for more parts in a day.
Perhaps the ideal (for such a factory) would be speeds and feeds which would call for replacing the cutter once a day -- at the change of shifts. For your own tools this is probably not optimum, unless someone is paying you to make a lot of these.
Good Luck, DoN.
Reply to
DoN. Nichols
Can you resharpen the cutter?
When I've cut gears flex and chatter limited the feed.
jsw
Reply to
Jim Wilkins
DoN's admonition above is well put; form cutters and slitting saws are run much slower than run-of-the-mill cutters. I would start with 1/4 to 1/2 of the speed as determined by classic means. Let's see: 4xCS/ dia=3D4x80/3=3D106rpm. (assuming low carbon steel work piece) I would start off with 30 rpm for a 3" dia. cutter.
As these cutters are quite robust one can use a fairly aggressive chip- per-tooth feed. How much depends on the surface finish required, horse power of the spindle, and rigidity of the set-up. I'd try .004" to .006" chip per tooth. Assuming a 12 tooth cutter the feed in inches per minute becomes 12x.004x30=3D1.44" say 1.5 inches per minute. Too low a feed increases cutter wear.
For cutting steel a sulphurized cutting oil is best when using form cutters. For a one-off any good cutting oil would suffice.
Let us know what you decide and how it worked out for you.
Wolfgang
Reply to
wolfgang
I would run about 60 surface feet per minute (sfm) and use either water based coolant or a mister with coolant in it. You could run faster but it will save the tool to run at 60 sfm. You could also use sulfur oil and either mist or paint it on the cutter. The final decision of speed comes from looking at the color of the chips and how much heat you are generating, all revelent on the sharpness of the tool, the type of coolant and the sfm of the cutter. To get the most life out of the tool you want the chips to come off shiny with no discoloration and the coolant not steaming from the heat.
formatting link
formatting link

John
Reply to
john
John, thanks. I will try to hook up the rotary indexer to my CNC mill tonight, so that I can do the entire job automatically without needing to press the button on the indexer. The mill itself would electronically "press the button".
If I do that, I do not particularly care of the job takes 10 minutes or 30 minutes due to too conservative setting of the feed. I can just start the job and go home to do something else. Plus, I have to worry less about rigidity.
I would say, I will start at 80 RPM or so. at 3 inches diameter, it gives me 62 FPM.
i
Reply to
Ignoramus8184
forgot to tell you how to compute the feed rate.
RPM x the number of teeth on the cutter x load per tooth (.002 to .004)= feed in inch per min.
John
Reply to
John

PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.