Showing results for 
Search instead for 
Did you mean: 

Finish problem


Whenever i used ball cutter for finishing a small corner radius by flow cut reference tool, the finishing is not proper and it not matched with previously run ball cutter operation its like gouges but its not detect and slightly impression is shown in my cavity plate

Please see this photos


Re: Finish problem

Siemens Phenom Siemens Phenom
Siemens Phenom

Hey @Vora,


would you mind filing an IR through GTAC with the part which you are describing here?


We are currently modernizing our Flowcut Algorithm, so I guess this issue will be solved by then.


Thank you in advance for your help.




Lead Product Manager - Mold & Die

Re: Finish problem

Solution Partner Creator Solution Partner Creator
Solution Partner Creator

Hi @Vora,


I think if this happen because of geometry problem, before you create program, its better to make sure the solid body, edge or surface is with no errors. Try this:


1.Export your single body part to healed geometry, make sure the geometry's errors are healed.

2.Once you get your_part_hg.prt, then import this into your existing part.

3.Try to make smiliar operation, then compare.


Base on my experiences, bad tool paths caused by bad geometry.


Hope this help,



PT.Mitra Makmur Teknologi

Re: Finish problem

Siemens Phenom Siemens Phenom
Siemens Phenom

When you say that the operation "like gouges but its not detect," do you mean that the surface finish on the actual part is bad, but NX does not detect any collisions or gouges with the Gouge Checker?


There can be multiple factors why this can happen. Spindle speeds and machine feed rates are important. Some of the cusps on the other surfaces look rather choppy in the provided picture, so you may be running things a bit too fast overall. For a smaller cutting tool such as the ball end mill you are using with the Flowcut path, going too fast can cause a lot of tool deflection when cutting. Try adjusting the speeds and feeds of the machine and see if you can get better results.


Also, make sure the cutting tool is running true by checking for runout with a dial indicator.

Re: Finish problem


I find I like to turn down the look ahead in the cutting parameters.

By default it is 30% of the cutter.


For fine finishing I'll take it as low as double my intol outtol

You get more code, but a finer finish also...


Paul S.

{Paul Schneider}, {CNC Programmer}, {DRT-Rochester}

Production: {NX11.0.2,MP5, NX12.0.2, MP4}

Re: Finish problem


I would use Reference tool diameter = tool dia used in previuos operation + 2 mm : as reference tool diamenter for this to overlap the flow cut toolpath.

Re: Finish problem

Solution Partner Legend Solution Partner Legend
Solution Partner Legend

How did you set up the Intol and Outol of the Flow-Cut operations?

Sometimes it is a combination of the finishing path and the cutting with the smaller tool. Also cutting forces could be relevant, perhaps there is much more material left in the edges than expected and because of that the cutter gets dragged into the surface.


Sometimes it is not the algorism, perhaps :-D 

Learn online

Solution Information