.050 ball endmill .025 deep for miles

[left coast lefty]

This is in 304 SS, and I have 10K RPM. I'm using a Harvey Tool stubby 4 flute. I went .005 deep per pass at 12 IPM and got a fair amount of success, but very slow. Should I go deeper on the 1st pass? Faster feed?

 

Thanks in advance

[YoDoug®]

I have had good results taking a roughing pass first with a 60 or 90 deg offset tip engraving tool. then go back for a single finish pass with the ball endmill. The roughing pass go almost full depth, .002-.003 shy. This will get most of the material out towards the tip of the ball mill which is where your SFM is the worst on a ball mill. The offset tip engraving tools can take a little higher chip load than a ball mill from my experience.

[Sticky]

I am using a regular LOC 2 flute .0625" ball em in 304ss at 15k rpm, and .01" depth, 15ipm. Turned down to 10k is 10ipm. So I would think your could start by doubling your DOC. I would think you could up your chip load quite a bit because I am running almost double, with a regular LOC flute, which is less ideal. Also run out is critical on small tools like this I have found. I like to be under .0001" when running tools this small.

[Sticky]

Good idea YoDoug, I'm gonna have to try that if I ever need to go deeper. I am mostly just doing engraving with these small ball mills.

[EX-wccprogrammer]

Good idea YoDoug, I'm gonna have to try that if I ever need to go deeper. I am mostly just doing engraving with these small ball mills.

 

For engraving I use this:

 

http://www.youtube.com/watch?v=lpWkqvhDlVQ

[Sticky]

How does it do on small text? A lot of the engraving I do is .120" tall and smaller. For the small text I only go .003" deep with a ball mill to get nice crisp lines.

[left coast lefty]

I am using a regular LOC 2 flute .0625" ball em in 304ss at 15k rpm, and .01" depth, 15ipm. Turned down to 10k is 10ipm. So I would think your could start by doubling your DOC. I would think you could up your chip load quite a bit because I am running almost double, with a regular LOC flute, which is less ideal. Also run out is critical on small tools like this I have found. I like to be under .0001" when running tools this small.

 

Good point about the runout. I am using an ER16 collet and it's tough to get it within .0005. Maybe I'll try 15IPM? As far as the depth, I think I should try deeper on the first pass, then smaller as it gets to the bottom where the tool is almost fully engaged.

 

Thanks!

[Sticky]

Yikes .0005" is a bit much for a small tool like that. Fwiw you can get .0001" with an er16. I use mostly Techniks holders now, and with an er16 holder with their regular collets I am almost always under .0002" Sometimes I am lucky and am less then .0001". We always torque to spec, which I have found makes a difference.

[EX-wccprogrammer]

You can get cutting info on the indexable here:

 

http://www.advancedcarbidetooling.co.uk/assets/166/168/nine9_engraving_tools.pdf

 

It does a very nice job in 316 forgings.

 

HTH

[left coast lefty]

Yikes .0005" is a bit much for a small tool like that. Fwiw you can get .0001" with an er16. I use mostly Techniks holders now, and with an er16 holder with their regular collets I am almost always under .0002" Sometimes I am lucky and am less then .0001". We always torque to spec, which I have found makes a difference.

 

We have Briney holders. I guess I'll try to tap it in. Thanks for the help!

[Matthew Hajicek - Singularity]

Lefty, are you engraving or surfacing? If the latter you might try roughing to near net with a solid carbide high feed first. I use them down to 2mm in 47RC H-13 with good results, then come back and finish off the last .003".