Toolpath suggestions for roughing 3D with Feed Mills

[lowcountrycamo]

I am about to test several solid and insert Feed Mills for roughing 3D pockets in TI 6AL-4V and 13-8 PH Stainless 42-48RC.  Any suggestion for toolpaths? These are running on 3x and 4x Okuma osp200 and osp300.  I have thru coolant.  I have never programed for a Feed Mill.

Much appreciated as always,

Steve Austin

[Leon82]

Depending how deep you may need one with a draft option.

Dynamic and optirough with no up cut if you have pockets with steps.

 

It's usually.03 to .09 depth cuts at 50 to 70% radial from what I remember. Depends on the insert and cutter. Still chip thinning but with the tool radius not the diameter

[JoshC]

19 hours ago, Leon82 said:

Depending how deep you may need one with a draft option.

Dynamic and optirough with no up cut if you have pockets with steps.

 

It's usually.03 to .09 depth cuts at 50 to 70% radial from what I remember. Depends on the insert and cutter. Still chip thinning but with the tool radius not the diameter

Yea i agree with Leon, Dynamic Optirough, No Stepups (just set step down to the Depth your tool vendor says their tools can handle, like .04" or something similar probably and if its small DOC you dont really need stepups). Make sure your min toolpath radii is like 10%, smaller you go the more you could hear chatter in the corners but the bigger you on min toolpath radii the more stock you will leave in corners. 

Both 3d Area Mill and 3d Optirough will work but optirough gives the nice entry/exit moves and also doesn't bury the high feed mill into corners due to min toolpath radii. 

Also use a Micro lift, just couple thousandths of an inch is all that is needed. 

[crazy^millman]

Old School Surface Rough Pocket does a good job with this if you willing to put in the effort. I have used the OPTI-Rough and it does okay with these tools, but you cannot define the tool with custom geometry or life will become unbearable very soon if the file is more than a block with 4 holes in it. Defining them as Mastercam Bull endmills using the OEM defined Tool Radius is the only way to use OPTI-Rough with high feed cutters in Mastercam with any file that going to be complex. Problem with old school surface rough pocket is stock awareness as far as I know is still not part of the toolpath, but if the shape is a standard shape then surface rough pocket is a good choice for these types of tools. Odd Shape, Forging or Casting then OPTI-Rough is my go to toolpath with these tools and then adjust my parameters like I want.