cancel
Showing results for 
Search instead for 
Did you mean: 

Eliminating retracts between milling passes

Pioneer
Pioneer

In the part below, I'm drilling a clearance hole then sinking an endmill to finish out the pocket. The tool is retracting and reinserting several times when it doesn't have to. How can I eliminate these wasted moves? I know I can change my non-cutting moves within regions but I'm not sure how to verify if the tool will avoid uncut material with these settings, though. NX9.0

 

On a related note, some of the default settings are pretty frustrating. The first part I ran left this little uncut nub, which the 3D preview did not show. After some digging I found the overlap option and changed it from 0 to 0.2in. Hopefully this takes care of it. With so many options it would be nice to have some defaults that make it easier to get things right the first time.

 

4 REPLIES

Re: Eliminating retracts between milling passes

Valued Contributor
Valued Contributor

AICLE > I'm not sure how to verify if the tool will avoid uncut material with these settings,

 

Use Check Geometry to look for gouges.

You set the tolerance in Cutting Parameters too under stock, check stock integer.

Re: Eliminating retracts between milling passes


AlCLE wrote:

In the part below, I'm drilling a clearance hole then sinking an endmill to finish out the pocket. The tool is retracting and reinserting several times when it doesn't have to. How can I eliminate these wasted moves? I know I can change my non-cutting moves within regions but I'm not sure how to verify if the tool will avoid uncut material with these settings, though. NX9.0

 

On a related note, some of the default settings are pretty frustrating. The first part I ran left this little uncut nub, which the 3D preview did not show. After some digging I found the overlap option and changed it from 0 to 0.2in. Hopefully this takes care of it. With so many options it would be nice to have some defaults that make it easier to get things right the first time.

 


It sounds like you know this, but to be sure in Non Cutting Moves, there are 7 options for Transfer Type within a region. It sounds like you are looking for "Direct/Previous Plane Backup" or something similar. If another option is better for you, then you should adjust your templates, so that you don't need to change this every time.

 

If everyone used the system the same way to cut the same parts, then we could provide defaults you would always like. But in reality, everyone wants or needs something different, so we provide customization tools such as templates. And when in doubt, we will set defaults on the safe side, which is why the default transfer is to retract along the tool axis to the clearance plane.

Mark Rief
Retired Siemens

Re: Eliminating retracts between milling passes

Legend
Legend
Be careful finishing any areas with trichodial paths. It uses smoothing and will not cut your corners correctly if your tool is too close in size to the fillet.
NX11.0.1

Re: Eliminating retracts between milling passes

Valued Contributor
Valued Contributor

Make sure the CNC Rapid Traverse Mode Parameter is set to handle Linear Interpolation or the result at the machine will be unfavorable. This is a Machine Parameter that sets the Executive Software Variable to handle Rapid moves G00. Without this synchronization between the CNC Machine CPU and the NX Software, (Non Cutting Moves, there are 7 options for Transfer Type within a region) there will be gouges, scrap parts and broken tools.

 

Use Check Geometry to look for gouges. You set the tolerance in Cutting Parameters under stock, check stock integer. Make sure to have the Non Cutting Moves, More, Collision Check, Collision Check is activated and in the Customer Defaults, Manufacturing, set the Collision Check to handle Clearance Plane Moves, (when gouge occurs, Clearance Plane, Minimum safe clearance, are some choices you can select.) Use direct in non-cutting moves, transform/rapid, within regions, transfer using- engage/retract, transfer type- direct this will keep the tool down into the cut.

 

Use Check Geometry to look for gouges. You set the tolerance in Cutting Parameters under stock, check stock integer. Make sure to have the Non Cutting Moves, More, Collision Check, Collision Check is activated and in the Customer Defaults, Manufacturing, set the Collision Check to handle Clearance Plane Moves, (when gouge occurs, Clearance Plane, Minimum safe clearance, are some choices you can select.)

Learn online





Solution Information