Island left with dynamic toolpath

[JB7280]

I'm using a feedmill for a dynamic facing toolpath.  I've tried playing with the stepover, and can't seem to eliminate the little island in the middle.  Other CAM packages I've used had features like "extra moves" that would get rid of it.  Any trick to eliminating this in MC?

 

[AHarrison1]

This was brought up on the Mastercam forum.

https://forum.mastercam.com/Topic39965.aspx

Apparently they are looking into it.

[JB7280]

1 hour ago, AHarrison1 said:

This was brought up on the Mastercam forum.

https://forum.mastercam.com/Topic39965.aspx

Apparently they are looking into it.

Cool, thanks.  I added my $.02 there as well.

[gcode]

That screen shot looks like you are using a high feed cutter

When using these, you must be aware of the bottom diameter of the cutter and adjust your radial step over accordingly

IMO, the software should know this and do it automatically, but it doesn't at this time.

(see D5 is this screen shot)

 

[Newbeeee™]

/Hijack on

2020 2D pocket...i see it can still leave upstands depending upon stepover % and part shape (using square bottom endmills not hi feeds)....

 

[gcode]

3 hours ago, Newbeeee™ said:

2020 2D pocket...

I don't think the legacy pocketing toolpaths have seen any TLC since the DOS days.

I'm almost always muttering nasty words when using these toolpaths.

They usually produce terrible results, mostly lots of unnecessary recutting at the end of the toolpath

I'll use them if I'm doing a one off part, but anything involving production, I'll use as pocketing toolpath,

save the C/L wire frame then edit to get rid of the overcutting.

[JB7280]

55 minutes ago, gcode said:

That screen shot looks like you are using a high feed cutter

When using these, you must be aware of the bottom diameter of the cutter and adjust your radial step over accordingly

IMO, the software should know this and do it automatically, but it doesn't at this time.

(see D5 is this screen shot)

 

Yes, you're correct, it is a 2.5" feed mill with a "cutting diameter" of 2.040.  I started my toolpath with an 80% (2.0) stepover, and tried as low as 50%.  It was like Mastercam just NEEDED that island to be there, lol.  I ended up abandoning the dynamic toolpath, and cutting one-way passes down toward the floor as I'm having other rigidity issues with the machine anyways.  Just a point of frustration that I thought I would ask about, as I run into it often.

[crazy^millman]

28 minutes ago, gcode said:

I don't think the legacy pocketing toolpaths have seen any TLC since the DOS days.

I'm almost always muttering nasty words when using these toolpaths.

They usually produce terrible results, mostly lots of unnecessary precutting at the end of the toolpath

I'll use them if I'm doing a one off part, but anything involving production, I'll use as pocketing toolpath,

save the C/L wire frame then edit to get rid of the overcutting.

Turn off Finish pass and works like a champ. How I did it for years before switching to Horizontal after Murlin showed me a good way to use it.

[gcode]

Just now, crazy^millman said:

Turn off Finish pass and works like a champ.

I almost never use finish pass

[huskermcdoogle]

Define your cutter as a bull nose with the same end diameter and it should get rid of the overlap.  Do not use this definition for anything other than dynamic milling or facing/pocketing operations.  3d toolpath should not use this definition.  For 3D you can still and likely should use a bull nose as the definition, but you will want to program with a smaller corner radius value (usually provided in the tooling manufacturer catalog) to prevent profile overcutting.

[Guest]

42 minutes ago, gcode said:

save the C/L wire frame then edit to get rid of the overcutting.

That was a neat trick i got from u, I made a chook that appends pocket operation toolpath points into a contour, I saved over 1000 pocket toolpaths into one contour

[gcode]

29 minutes ago, huskermcdoogle said:

Define your cutter as a bull nose with the same end diameter and it should get rid of the overlap. 

+1  .. you can define the high feed cutter as a bull endmill using the manufacturer's  recommended corner radius.

Then use the step file has eye candy. Mastercam will use the bull endmill definition to calculated the tool paths

and the step file for backplot and verify..and yield accurate stl files for stock models

 

[JB7280]

24 minutes ago, gcode said:

+1  .. you can define the high feed cutter as a bull endmill using the manufacturer's  recommended corner radius.

Then use the step file has eye candy. Mastercam will use the bull endmill definition to calculated the tool paths

and the step file for backplot and verify..and yield accurate stl files for stock models

 

Interesting.  Good to know.  So it would use the white outline geometry for actually generating the toolpath, but then use the 3d portion in your screenshot to actually generate the cuts in verify?  I'll try it shortly.  Wouldn't that give me the opposite effect though, as it thinks the bullnose is covering more ground than it really is?  Just thinking out loud.  I will try it in a bit and see for myself.

[gcode]

7 minutes ago, JB7280 said:

Interesting.  Good to know.  So it would use the white outline geometry for actually generating the toolpath, but then use the 3d portion in your screenshot to actually generate the cuts in verify?  I'll try it shortly.  Wouldn't that give me the opposite effect though, as it thinks the bullnose is covering more ground than it really is?  Just thinking out loud.  I will try it in a bit and see for myself.

you still adjust your step over per the D5 diameter, not the major diameter

In your case 2.04 x.5 = 1 

[Matthew Hajicek - Singularity]

Or you can just use the graphical toolpath editor to add a move or two at the end.

[#Rekd™]

On 4/14/2021 at 11:00 AM, crazy^millman said:

How I did it for years before switching to Horizontal after Murlin showed me a good way to use it.

Ron can you share an example?