Is it possible to finish flats with end mill and all others with ball mill?

[CanSir]

I'm testing out MeshCam 4 and it's kind of frustrating me. The part I'm cutting has a lot of flat areas and they come out looking great after roughing with a 1/4" end mill, then the "finishing" path comes along with a 1/8" ball mill and ruins the surface finish. I already have the ball mill stepover set to 0.02" (!) and you can still see the cut lines left by the ball mill.

I realize this crappy surface finish may be a result of a few thousandths variance in cutter length after performing a manual tool change, but if MeshCAM had the end mill cut the surface to the final depth already, then why is it wasting time running the ball mill over it? Come to think of it, CutViewer shows the crappy surface finish I'm experiencing in real-life so it can't have anything to do with my machine.

Is this a beta version bug or am I missing something?

Thanks!

[ger21]

No bug, that's the way MeshCAM and similar programs work. Typically, for a really good finish, people use 5-8% stepover, which would be .006-.01" with your 1/8" endmill.

A new beta version of MeshCAM 4 was just released, and let's you select regions to machine. This should allow you to machine flat areas with an endmill, and other areas with the ball mill. However, it may not be as simple as you'd like. I only played with it for a minute.
http://www.grzsoftware.com/v2dl.php

[CanSir]

No bug, that's the way MeshCAM and similar programs work.

Thanks Ger21. I guess watching the VCarve tutorials had me thinking it was typical for cam software to optimize the tooling paths with consideration given to the shapes of cutters being used.

For $175, I want MeshCAM to have all the features of the much more expensive CAM's !

[robgrz]

You can leave the end mill in and tell MeshCAM to only finish areas that are less than some shallow angle- maybe 20 degrees. You could then do another toolpath with only waterline finishing using the ball mill and tell MeshCAM to only machine areas steeper than 15 degrees. (The overlap makes sue that all areas are machined without gaps).

This method would give you a pretty good finish with the right cutter for each region.

-Robert

[ger21]

Thanks Ger21. I guess watching the VCarve tutorials had me thinking it was typical for cam software to optimize the tooling paths with consideration given to the shapes of cutters being used.

For $175, I want MeshCAM to have all the features of the much more expensive CAM's !

You do realize that V-Carve Pro can not do 3D carving, which is what MeshCAM does, right? Competely different types of operations.

[CanSir]

You can leave the end mill in and tell MeshCAM to only finish areas that are less than some shallow angle- maybe 20 degrees. You could then do another toolpath with only waterline finishing using the ball mill and tell MeshCAM to only machine areas steeper than 15 degrees. (The overlap makes sue that all areas are machined without gaps).

This method would give you a pretty good finish with the right cutter for each region.

-Robert

Big improvements! Your suggestion significantly cut down my machining time as well. Thanks.

I still can't make sense out of your two-sided machining though. I align my material to an L-shaped fixture mounted in the SW corner of my cutting table. I also zero my machine there. After physically flipping the material to cut the bottom side however, I have to manually re-zero my machine to the top left corner of the material or else all the cutting is trying to occur past my machines limit in the -Y direction. The Z-zero also gets inverted (was top of material, but after flip it is now bottom of material).

[robgrz]

When I do a two-side job I usually center from the center of the left side of the stock since that allows helps offset any error (if any) in the stock measurements you entered into MeshCAM.

The zero should not be moving when you flip. If you zero on the SW corner then you should zero on the SW corner after flipping as well. Is this not what you're seeing?

-Robert

[ViperTX]

You can leave the end mill in and tell MeshCAM to only finish areas that are less than some shallow angle- maybe 20 degrees. You could then do another toolpath with only waterline finishing using the ball mill and tell MeshCAM to only machine areas steeper than 15 degrees. (The overlap makes sue that all areas are machined without gaps).

This method would give you a pretty good finish with the right cutter for each region.

-Robert

Robert, How exactly is the above quote performed?

Also regarding 2-sided machining, when you flip the part over..why do you have to re-zero?

Also how are you centering on the part? What exactly are you using?

Is there any documentation on the angle stuff you mention?

I'm not a machinist and am struggling with the 2-sided machining.

Thanks,

Paul

[robgrz]

For parallel finishing there is a parameter labeled "Limit Surface Angle". Just select that and enter "20". For waterline it's labeled "Min Surface Angle". Just enter "15" for that. Because parallel and waterline share a single tool you'd have to run two separate toolpaths if you want to use a flat mill for one and a ball mill for the other like the original poster requested.

The angle settings should be covered in the help file although I will probably document it better in the V4 documentation.

If you had a very good fixture to align the stock then you would not need to rezero. Personally, I have gotten better results by finding the center of the pat by using a wiggler to find the top edge and bottom edge and then going to the midpoint between them. From a theoretical point of view this shouldn't matter but I have never spent the time setting up a good fixture and accurately squaring my stock. The method outlined above is more tolerant of my sloppiness.

-Robert