I'am trying to mill some simple form by using volume machining of large material - cavity mill.
There are 4 holes on side internal walls which I need to ignore. In Z-level operation there is an useful option in Cutting Parameters: continue cutting below tool contact + extend - Iam looking for same combination in Cavity mill. I know that I can cap this holes in synchronous modeling but i want use standard operation with proper set up.
I attach my file in prt. (nx 10) together with cavity and z-level milling for comparison.
If You have some idea to make bypass of this cutout will be very great
I'm afraid you cannot handle this with cavitymill without creating additional part geometry but maybe you can consider using, for this particular case, floor and wall.
check the attached example.
hope it helps
Follow periphery cut pattern will bridge the gaps better, but not directly like you want.
I think you will find that there are many different ways of controlling the tool path in Cavity Mill.
Go to Cutting Parameters and check out the Strategy Menu. There you will find an attribute input called Extend Path. In extend at edges integer box you can input the distance this will connect the gaps.
Also using largest tool helps to connect gaps as well.
Cavity Mill works as though draining water out of a lake level by level. When you have a leak you need to plug this leak or the tool will escape the water line.
In Cutting Parameters _ Strategy Cut Order depth first will keep the tool engaged in material.
Also Non Cutting Moves _ Transfer / Rapid _ Between Regions - Within Regions _ Transfer Type you can control clearance moves by using direct moves.
I would highly recommend you use Check Geometry to look for gouges. You set the tolerance in Cutting Parameters too under stock, check stock integer.
Ibonomi - yes, floor and wall is the best example there, so thanks for advice. There are better options to ignoring holes while rough machining. But here is one importand condition - cut area floor must have flat surface.
59holloman - I will remember about to use Check Geometry (gouges), this was good suggestion !
About Extend At Edges in cavity mill, yes - th the functionality of this option is known to me, but sometimes I have some strange results.. I mean in Z-Level there is better becouse I can bridge the gaps in logical way, but in cavity I recieves something different. I attach two pictures with cavity and zlevel extend for comparison.
I told you the example was for that particular case, if you have a non planar floor, cannot use floor and walls.
I do not like using the word wrong. It is a matter of getting the right combination of switches turn on and the ones not needed turned off. I have used Cavity Milling for years. It is one of my favorite tools in the box.
Check out Cutting Parameters _ Containment _ Blank and Small Area Avoidance.
The Reference Tool is new and is very beneficial in this case were you can use a bigger tool and then comeback with smaller tool and clean out corners.
Another is a suggestion by Mark Rief to set Cut Pattern to Follow Periphery.
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.)