stepover, speed, and feed

[Travis2282]

I am milling a 3d part using surface finish parallel. using a 1in. carbide ball nose emill 4 flute cutting aluminum. My tool is cutting from 0 to -.875,I started off of the part and stepping over my way through the part. not much experience on cutting 3d any suggestions on what my max stepover, speeds,and feed should be. Thanks

[Justin Beebe at Folsom Tool]

Bowhunter,

 

I prefer 2 or 3 flutes in aluminum because they evacuate the chips better than 4 flute. The stepover depends on your surface finish requirement. If you use a stepover 1% the diameter of the endmill ( in your case .010) you will get a nice finish but it may be too nice and waste time. It's hard to say for sure not knowing the surface finish requirement and not seeing exactly what you are machining. Are you roughing and finishing? Can you post a pic or share a file of the part?

[Travis2282]

It does not require the best finish because it will be polished after machining. I am just doing one cut on the part since there are no real tolerances. I just need fast cycle time with a decent finish.

[PaceToolmaker]

A lot of time i start with 1000 sfm,20% stepdown and stepover depends on my finish requirements.Most times i ruff with .100 to .200 stepover just to get the meat off then finish with .010 stepover if using a parallel toolpath.Depends on the part and the toolpath being used.3 flutes is the way to go also,4 flutes tend to plug up.

[PaceToolmaker]

crank it up til the cutter breaks then back off half a notch.

[Travis2282]

Thanks for the advise, i will try it tomorrow.

[neurosis]

Bow,

 

Your question is a little hard to answer with the information you gave.

 

You say from 0 to -.875 but are you descending in to the material? Are you climbing from the -.875 up? What is the shape of the part that you are cutting? are there valleys? or are you just climbing up a cone shape?

 

If you are going up then the four flute will probably be fine. How much rpm and feed do you have available to you?

 

If you are descending then things will change a little.

[Chris Rizzo]

what he said ^. Not to mention how much your leaving for this finish tool. .020 ought to be good. Your filter settings are very, very important. Off will prob. give you the most accurate finishing. 2:1 at .001 will probably be fine for your application. Study the verify closely. What you see is what you will get in regards to surface finish and toolpath. You see little gouges (which is just the filter working) in verify, they will be there on the part. Part shape depends alot on this too.

 

Full speed on the spindle. Start at maybe 100ipm and use feed override till she looks bad or the machine starts to choke on code. Oh, turn your gap settings to "smooth" and you'll get smoother edge motion too. Don't be afraid to try the HST Raster, that does some wicked stuff too..but tha's a whole nother thing to learn.

 

you ask 10 different programmers and you'll get 10 different answers. this is just mine.

[LaszloK]

My general rule of thumb is to use .002 per 1/8 of cutter diameter when using ball nose in parallel machining, so .016 for a 1.00 ball endmill. You can also use .0002 scallop height and get similar results.

[Cad-Camr]

We use a 1/2 4 flute carbide EM for Surface Finishing,somewhere around .005 step over to get a good finish. Spindle at max and 180. to 200. Feed Rate.