Flowline Chamfer

[JeremyV]

Currently working on a 10" thru hole with a 45deg chamfer that is .850dp.... Tried a chamfer cutter going 3+ passes and that left lines between cuts;

 

Now trying flowline on a spiral path, except my program is miles long....   Is there a way to switch from linear to arc in the flowline section or am I using the wrong type of cutting parameters/tool path?

 

-JD

[cncworker]

Use 2D contour, parameters, go into cut depths and select tapered walls, set taper angle to 45.  Also use more depth cuts, on that same page.

[MIL-TFP-41]

48 minutes ago, JeremyV said:

Now trying flowline on a spiral path, except my program is miles long....   Is there a way to switch from linear to arc in the flowline section or am I using the wrong type of cutting parameters/tool path?

 

-JD

When you are doing a spiral path, there really are not any arcs to filter. Well maybe the first pass at the top & the last pass at the bottom....but as long as you are doing a spiral on a cone, there isn't an arc on any one plane.

[JeremyV]

58 minutes ago, cncworker said:

Use 2D contour, parameters, go into cut depths and select tapered walls, set taper angle to 45.  Also use more depth cuts, on that same page.

This can work with a ballnose?  I've never tried it before, except with a chamfermill and the chamfermill leaves lines we don't want between cuts...

 

But I can try it anyhow...

[Leon82]

use one way instead of spiral and turn on the filtering 

[nickbe10]

If you want to stitch it with a ballnose you will need a surfacing path. Flowline and Waterline (my preference, more control of ramping between z levels) will work.

[JeremyV]

We went with the ballnose option as management did not like seeing the lines in between cuts...

 

So I programmed it automatic with .02 per pass going 140-160ipm @ 5800RPM - I didn't account for spacing and left it automatic... it was funny looking - kinda like a disco ball.  So i tweaked that to .01" and jeez... the program ballooned to 11,000KB+ in size, which is way to big as the machine  can only hold 500-600KB of code...

So after a lot of adjusting, managed to fit the program in the machine at .128" i took about 15 mins to do.

Hopefully this'll be the only time we need to make a chamfer that big, however if we get it again or something else, I think we should consider getting an ISCAR 45deg cutter that can do large chamfers...

[Brian Pallas]

Swept 2d works perfect for this if you can get the first chain aligned with x or y. Then you create multiple tool paths if you need to rough  and finish it.

[jeff]

On 12/8/2017 at 3:59 PM, Leon82 said:

use one way instead of spiral and turn on the filtering 

This is how I do it with those large pesky chamfers

[Colin Gilchrist]

Surface Finish Contour is the proper path for this, since you will get multiple circular cuts. Use the Toolpath Filter, and you'll get a nice, short program, with Arcs.