HST Area Mill with feed mill. Custom tool?

[Joe788]

Usually my high speed stuff is in aluminum with regular endmills, but now I'm about to run a .750 Mitsubishi AJX cutter in 17-4PH on a complex hogout. I've got a bunch of rest milling operations afterwards to get all the way down to a .125 ball mill in a lot of places.

 

Is there anything special I should be doing? Should I draw the feedmill as a custom tool so the rest-mill stock is accurate? Or is the flat bottom accurate enough?

[peon]

Joe, you are correct by creating a custom tool. I cut some scrap carbon with my AJX cutters and analyzed them in a comparator. Using the cutters theoretical radius as defined by the cutter manufacturers will be inaccurate on the shallow surfaces of your workpiece and will overload your restmilling tool.

[Superman]

I have had better success using the feedmill described as a bullnill on surfacing operations, ie using a Ø1.5" feedmill, base Ø=.5", tangental rad=1".......putting these together equates to a Ø2.5" bullnose with 1" corners

 

The custom tool profile is not used to calculate a surface path, the custom profile is only used to remove material in verify to give a reasonable STL to look at. Calculations are only based on the OD and the Corner Radius

[cobra95kev]

Superman,

Does what you are saying apply even if you are driving your restmill from an STL stock?

[peon]

Even defining the cutter as a bullnose and saving as an .stl IS NOT good enough in rest milling applications while comparing against the saved .stl as stock. The shallow surfaces will be stock heavy and you may overload your tool.

[Superman]

quote:

---

The custom tool profile is not used to calculate a surface path, the custom profile is only used to remove material in verify to give a reasonable STL to look at. Calculations are only based on the OD and the Corner Radius

---

I'll try ot explain further.

A custom tool will only use the defined OD and defined corner radius to calculate a path against an angled surface, the actual tool profile that is drawn IS NOT USED in the actual calculation.

The tool profile is only used in the backplot or verify screen graphics. The remaining stock can be compared to an accurate STL of the model to highlight uncut or gouged material.

 

There is a more involved method of using a bullnose cutter with a scaled version of the custom tool to get the graphics working your way ---you are effectivly just tricking the system

 

Try this:-

2 custom tools, drawn identical except for corner radius ( make it a big difference ),

but have the defined radius common to both, generate a surface toolpath for each tool, and compare the NC output. the NC code is identical

 

now.....alter the defined corner radius on 1 tool and re-post.

 

notice the code is now different, you didn't alter the drawing...this indicates that the tool profile on a custom tool is NOT AT ANY TIME used to calculate toolpaths.

[Colin Gilchrist]

Superman is correct. Mastercam will not use the actual profile of a custom tool to drive against surfaces. The only tools in Mastercam that will actually drive surfaces accurately are Flat, Ball, and Bull Endmills.

[peon]

This is how I define the high feed cutters. It will cut as close to the model as possible using the theoretical radius and verify accurately so you can save the verified stock as an .stl and use it in your next rest rough operation.

 

[YoDoug®]

+1 to peon. The cutter manufacturer should give you a theoretical corner radius to program to.