Circle Mill Helical Entry Not Working

[Bill H]

I can't get a helical entry to work in Circle Mill.  Can someone look at the attached file and tell me what's wrong?

circle mill test.mcam

[Leon82]

Check the minimum radius and XY clearance in the entry motion section.

 

I usually set mine to 1% and 45%. XY to .005 or less depending on what I'm doing.

Also check your clearance planes and feed planes

[Bill H]

Leon82:  I've checked all these parameters and I still can't get a helical entry.

 

[Leon82]

Is the linearize helix button checked? I can't see the file at home.

 

[#Rekd™]

I tried to get it to helix but it wouldn't go. 

[So not a Guru]

You have to have "Finish" check for the helical entry to activate. i dunno why.

Also the 0.00001 total tolerance was blocking it. I changed it to 0.001 & it worked

3 minutes ago, So not a Guru said:

You have to have "Finish" check for the helical entry to activate. i dunno why.

I was wrong, it is the 0.00001 total tolerance that is blocking it. I changed it to 0.001 & it works fine,

[So not a Guru]

0.0001 works too.

[neurosis]

In the arc filter I clicked 'output 3d arc entry motion' and it added the helix without doing anything else. 

I don't remember having to do that in the past (pre 2023).  I'm on 2024 now but 2023 seems to do the same.

[Aaron Eberhard]

I believe that Neurosis & So Not A Guru together have the correct answer.

You have a toolpath tolerance that's below the default system tolerance:

You over-rode the default behavior of Circle Mill (Output 3d arcs) which means that the helical entry needs linearized at your toolpath tolerance, which it won't be able to do, so I'm guessing it's dumping it into the "If Helix Fails" loop.  

You'd need a programmer to validate this, of course, but that's my theory.

And just to confirm you're not crazy, Neurosis - Pre 2020 there was no "toolpath tolerance" page for Circle Mill, and it was always outputting 3d arcs.    When we consolidated 3 axis & 5 axis circle mill, the tolerance page was needed.  The default behavior was to have it on, as that matched what had happened since circle mill was invented in V3 or whenever it was.  It's greyed out if you set Tool Axis Control to 4 or 5 axis, since that toolpath cannot generate 3d arcs at all.

[Bill H]

Thanks for the help everyone!!!