Surface rough flowline

[jeff]

Hi all,

I am having a very stressful time trying to find the problem to my program.

I am trying to machine a .5315 radius in the top of a part with a 5/8 carbide insert ballnose.

My first depth of cut goes about .227 deep and then it starts the depth of cut that I had told it to do which is about .03.

I am about ready to "fix" something with my hammer if I cannot figure this out.

settings are:

max stepdown .03

stepover control .1

total tolerance .02

the cut depth is the default setting "incremental and .01 are the values in the boxes.

How can I get this first cut to be reasonable about .05 or so???

[Guest CNC Apps Guy 1]

Without seeing the topology of the surface(s) it's kind of hard to tell.

[MGIRLING]

James is correct it is hard to tell without seeing the surfaces, but could you try setting your cut depths to absolute and make minimum depth 0 and maximum -.844

[McRae]

The software is going to drive the intersection of the ball nose and the surface radius. You will need to set your containment boundry to the center of the tool and then look at the surface settings. Post a file and we will help.

[mold100]

try using a scallop hieght instead of stepdown,maybe that will help a little.

[Jean-Simon]

Hi Jeff, I don't know how familiar you are with MC and I did'nt see the drawing but make sure your surface normal is up otherwise your tool is going to machine under and that's something that can look with what you explained. Hope it helps!

 

Simon

[jeff]

the file is named 1.063 dia groove and I put it in the mc9 folder on the ftp site.

thanks.

[MGIRLING]

set your cut depths to absolute and minimum depth to -.030 and maximum depth to -.400

[jeff]

Thanks MGIRLING!!!

That did the trick.

I had the cut depths set to absolute before BUT I had zero for minimum cut depth and a -.03 for max.

I knew it was something simple but just wasn't looking in the right place.

Thanks again.