Cutter Speed in shallow vs steep contouring

[Diedesigner]

Hi all,

To get the best possible finish when machining complex surfaces with a ball em, it seems to me that the rpm of the em should be adjusted depending on how shallow or steep the surface is.

 

For instance, a 5/16 ball em at .023 depth of cut on a flat surface has an effective cutter dia of .163".

The same cutter cutting .023 deep into a 45 deg surface has an effective cutter dia of .304".

 

At 250 SFM, the first example should run a speed of 5858 RPM, and in the second example 3141 RPM -- a significant difference. In addition, to maintain a constant chipload, the feed would have to be adjusted to the rpm.

 

I bring this up because I am new to 3D machining, and I wonder if I am over-thinking this, or do some of you take the time to make these type of calculations? I just want to get the best surface finish possible, to keep polishing to a minimum.

 

I know the highfeed function will automatically calculate optimum feedrates according to the amount of stock being removed, but it doesn't adjust cutter speed at all, even though the conditions are changing quite a bit.

 

I appreciate any comments/input you might have for me.

 

As always, thanks for your time with my questions.

Chris

[MACHINEMASTERG]

to get the best possible finishes i maintain the smallest scallop hight .0002.. etc this keeps your polishing to a minimum - the rpm isnt as big a factor as the scallop hight and remember a ball end mill tecknicaly dosnt really cut in the center!!so you will have some finishing to do

[Scott Bond]

Hi

quote:

---

For instance, a 5/16 ball em at .023 depth of cut on a flat surface has an effective cutter dia of .163".

---

If we leave .023 machine stock while roughing,,

and we call the .023 depth of cut---the .023 of machine stock to be machined away ,,,then the amount of material to be removed is a constant

.023---then just experiment with the best choices of cutting types.

[steve f]

Diedesigner,

 

This is one of the many reasons some tool and mold shops are beginning to invest in 5 axis mills. The cutter can be maintained at a specific angle to the surface normals during finish machining to prevent material "dragging" that occurs when cutting on center of a ballnose. To get away from this in 3 axis machining I use flat endmills whenever possible on horizontal or near horizontal surfaces. Up milling on a 10 or 20 degree sloped surface using finish, parrallel, one way with a flat endmill and small stepover can give really nice surface finishes.

 

Steve

[cadcam]

Some of my logiic come from the scallop hight .

 

an example a 1" ball EM at .05 step over leaves a .0005 scallop now as the tool gets samller and the tip to you need to go smaller.

 

I find with a .250 ball end mill bettween a .008 & .01 you get about te same result.

 

So to get even better results of course lets bring the step over to about .004 & .006 this has given me good results on many tool projects.

 

Now this thought for steep angle walls can work to but only on surface paths that are constant,

Were in say parallel if the angle becomes real steep the tool will not stay constant.

 

Hope this helps some along with the rest of the thoughts from the other TEAM MEMBERS .