Molding toolpath clearance issue

[Old_Rustic]

Folks,
I often use the Molding toolpath with a custom profile to make round or oval frames. During the Clear Waste stage, the emitted toolpath cuts an "X" in the waste part preventing it from being used for other jobs.

Does anyone know why this is done?
Can this behavior be turned off as it doesn't seem to be of any value?

What I do now is cut a profile around the inside of the shape, stopping the router, manually removing the inner waste by cutting tabs with a chisel, then running the Clear Waste process. I will often make 3 or more oval frames from the same starting blank.

Mike

[dealguy11]

I have never seen it do that, and I use the moulding toolpath every day. Could you post a file where is shows that behavior?

[adze_cnc]

Steve: The only thing I can think of that would do this is if you are doing a Profile Toolpath and using straight Leads.

[SteveNelson46]

Maybe not enough Z1 clearance?

[Old_Rustic]

Here is a simulation display & the corresponding model file.

Sorry I had to use DropBox links as page would not accept "bmp" extension and the "crv" file was "too large"

https://www.dropbox.com/s/2mtbvte0fg1y7 ... 0.bmp?dl=0
https://www.dropbox.com/s/812x9dy2bsgwf ... 0.crv?dl=0

Mike

[Adrian]

I don't use that toolpath enough to offer an explanation of why it's doing that but if you check the "Machine Flat Regions" box in the Larger Area Clearance tool section and recalculate it removes the crossing toolpaths.

[dealguy11]

I see the behavior and it appears to be a program error. You can make the problem go away by selecting "Ramp Plunge Moves" in the clearance tool setup for the moulding toolpath. Ramping is a good idea for this file anyway, and the extra cuts totally disappear. However, the original toolpath is an issue and should be reported to support@vectric.com. Make sure you send a copy of the file.

[Adrian]

Bit of a red herring on my part. Simply recalculating the toolpath removes that cross. I thought it might be something to do with being a later version that the file was created in (8.517) so I tried it in other versions.

Lo and behold versions later than 10 don't have the cross when the toolpath is recalculated but 9 and earlier do so I'd say it's a bug that was fixed in 9.5 or 10.

[Old_Rustic]

Yes, I'm still on 9.513. Haven't found the change to upgrade yet.

I will try the Ramp Plunge moves to see if this fixes the issue. I use ramps on most of the other profile cuts.

[dealguy11]

Hopefully that helps. Based on Adrian's info, it may be that the reason it went away for me was just because I recalculated, using v11.5

[adze_cnc]

For the flat clearance tool use a "Machining Allowance" other than zero and the "crossing" goes away in v9.513. Much like a 3D Roughing toolpath you really shouldn't set this at zero. It's better to leave some material for the ball-end cutter to clean up.

From the help file:

Machining Allowance

The machining allowance is a virtual thickness which is added to the moulding profile when the Use Large Area Clearance Tool is calculated. This ensures that the toolpath leaves some extra material on the part cut with a larger tool.

This is beneficial for two reasons, the first, is that when the larger area clearance tool is used, it tends to be done with a relatively large tool with aggressive cuts and so is more prone (depending on the material) to chip, the skin left by the Machining Allowance helps to prevent chipping the finished surface. The second reason is that most tools cut well when they are constantly removing material. Therefore leaving an allowance of material on ensures that there is always some material left for the finish toolpath to remove with the smaller tool.