X4 REFINE TOOLPATH, SMOOTHING

[DavidB]

What sort of figure are you guys using in the "Smoothing Settings" of the new filter?

 

When "Best" surface finish is selected "Smoothing" activates.

 

[peon]

We manufacture molds for the plastic and die cast industry. These settings seem to work very well.

 

 

[DavidB]

Why dont you use "Best" surface quality for your finishing?

You also have arcs turned on but in NO planes?

 

I ran my A66 last night with "BEST" surface quality and "LONG" NC program length and it ate it like ice cream,YUM, YUM

 

Cheers Dave

[peon]

The filter also filters lines, not just arcs. I do not wish to filter using arcs. It is defective and WILL violate surfaces. I have sent files to QC who have seen the surface violations themselves. Their answer is that it is fixed in the next MU. I question whether it will really be fixed since I've seen this problem since vs.9. My finishes have been excellent using these settings and not sacrificing crunch times or extra code.

 

 

I'm kinda shocked we don't have more users chiming in this topic. Is anyone besides Dave and I experimenting with the toolpath smoothing? This option does work very well!

[Tony35]

works good

[Guest CNC Apps Guy 1]

Has worked great with the parts I've tested with it.

[strabe]

I've only used a couple times with excellent results.

[Thee Rickster ™]

When using tool refinement does the total tolerance

become ignored?

 

I use the same setting as Davis pic and my total

tol is set at .0003 (does it matter?)

[Chris Rizzo]

It will always maintain the total tolerance. (from what I've figured out, and I've played with smoothing quite a bit now).

 

Cut tolerance, arc filter, and smoothing tolerance added together equal your total tolerance. What is goofy is that you set the total tolerance on the page outside all the filter smoothing settings. It carries that value into this filter smoothing page, but greys it out.

hth

[Newbieguy]

Peon: I'm kinda shocked we don't have more users chiming in this topic. Is anyone besides Dave and I experimenting with the toolpath smoothing? This option does work very well!

 

http://www.emastercam.com/cgi-bin/ultimate...ic;f=1;t=034970

 

We're experimenting too - patterns and mold building. And after peon's help, are getting very nice surface finishes!

[peon]

I have been loosening the tolerance a bit with improved finishes and faster crunch times. I changed my total tolerance to .001" and the cut tolerance to .0005" with excellent results and the tools fit fine when they are ready for assembly with minimal blitzing. I was originally crunching toolpaths with a .0004" total tolerance and a .0002" cut tolerance. I'm finding that it may have been unnecessary crunching with such a low tolerance.

[Thee Rickster ™]

Newbie guy, there are a bunch more ppl trying it

do you not see the other post in this thread like mine, strabes, chris, cnc and tony....

 

Alright so if I am using .0005 and then use the

same setting as in Davis 1st pic will I get a better than or just smoother .005 tolerance path created ?

[peon]

Rick, you confused me with your question. Total tolerance determines how close you wanna stay to your model.

[Jack Sierra Cad/Cam]

peon

Member

Member # 10077

 

posted 07-23-2009 09:25 AM

The filter also filters lines, not just arcs. I do not wish to filter using arcs. It is defective and WILL violate surfaces. I have sent files to QC who have seen the surface violations themselves. Their answer is that it is fixed in the next MU. I question whether it will really be fixed since I've seen this problem since vs.9. My finishes have been excellent using these settings and not sacrificing crunch times or extra code.

 

Try adjusting your arc tolerance in your control. X4 is supposed to automatically set this for you but if you do a migrated install it doesn't set its self. This problem has to do with your machine freaking out when it sees an irregular arc size in the toolpath.

[peon]

The violations are shown in Mastercam's verify. Please take a look at the tolerances below. Do you have any recommendations?

 

 

 

 

[Chris Rizzo]

random thought, do you have the tool tolerance tightened up in verify?

[peon]

Yep, I usually verify at .002" You can also see the tool violate the backside of the surface when backplotting.

[Jimmy Wakeford from Barefoot CNC]

peon do you have multi threading turned off? When using multi thread and toolpath refinement I was getting surface violations when processing two toolpaths at one time. This has been fixed for mu1.

[Jimmy Wakeford from Barefoot CNC]

I have been doing testing on machines that utilize aicc or highspeed smoothing of their own and notice that the cycle times are shorter when turning that off in the machine.

 

Anyone else testing the different machine/mastercam options against each other?

[peon]

Jimmy, yes, I always have multithreading turned on. I'll check that out. Thanks!!!

[Mark Baker CNC Software]

Peon, I have two questions with your filter problem.

 

what is your arc output? IJK's or R's?

 

What is your "break arc" setting in your post set to?

[peon]

I always use IJK's and I break my arcs at 180 degrees. Chris Bell actually has the file dated July 9th and he mentioned in an email that the problem is fixed in MU1. The file is named "MCX4_BUGS_BY_MATT_G.Z2G"

[Mark Baker CNC Software]

Having the "break arc" set to 180 degrees can cause you problems with the toolpath filter. Change the break arc to break on quadrants.

 

With the setting on 180 degrees the filter can "float" and cause trouble.

[peon]

Ok, I changed the "break arcs" to "quadrant", but it still violates the surface. Although, I do agree quadrants would be safer and I'm gonna make that change to my other control defs and posts.

[Slick]

2 cents:

 

This is a great thread. Keep up the input/comments, I'm learning a lot!

 

Thanks