Multiaxis Arc filtering & Smoothing

[Shiva.aero]

Is there any equivalent to '3D Line/Arc filtering & smoothing' option for Multiaxis toolpaths, to get good surface finish without tightening the cut tolerance?

[Chally72]

Hey Shiva,

There are a few levers we can pull in multiaxis paths to enact surface finish changes without just adding zeroes to the cut tolerance. Take a look at controls like Damp on the Cut pattern page, and especially all the controls like Points Distribution and Smoothing on the Cut Pattern Subpage, "Advanced Options for Surface Quality". That's where you'll find most of the like for like options.

In short, ignoring the arc settings which aren't applicable to linearized multiaxis code, most of the controls you see on the 3 axis paths do exist in one form or another across different areas of (most of) the multiaxis toolpaths, just not organized the same. You've also got tool posture to think about at all stages of the calculation, which is the single biggest contributor to scrubbing, slowdown, micro-gouging/stippling/etc that can affect the end result.

 

Check out this video which walks through methods of improving a multiaxis toolpath for surface finish. Hopefully it gives you some ideas on thinking about how to tweak your specific application for the best motion:

 

 

[Shiva.aero]

21 hours ago, Chally72 said:

Hey Shiva,

There are a few levers we can pull in multiaxis paths to enact surface finish changes without just adding zeroes to the cut tolerance. Take a look at controls like Damp on the Cut pattern page, and especially all the controls like Points Distribution and Smoothing on the Cut Pattern Subpage, "Advanced Options for Surface Quality". That's where you'll find most of the like for like options.

In short, ignoring the arc settings which aren't applicable to linearized multiaxis code, most of the controls you see on the 3 axis paths do exist in one form or another across different areas of (most of) the multiaxis toolpaths, just not organized the same. You've also got tool posture to think about at all stages of the calculation, which is the single biggest contributor to scrubbing, slowdown, micro-gouging/stippling/etc that can affect the end result.

 

Check out this video which walks through methods of improving a multiaxis toolpath for surface finish. Hopefully it gives you some ideas on thinking about how to tweak your specific application for the best motion:

 

 

Thank you!!!

[Joey5axis]

Hello guys,

I have tried fiddling with these settings.

Tried machining a 190mm "Bowl" with unified multiaxis, strategy is great, single toolpath and cutting off center with a sphere mill.

However I still get the "flat spots" on the surface finish.

These parts need to be polished to high gloss so its important to me to get the best results possible.

Mind you my settings are METRIC.

Cut Tolerance 0.02 

Maximum distance 0.5

Maximum angle step 0.5

 

Unfortunately I am not allowed to share 3D files with anyone.

Machine is a DMG DMU75 Monoblock with Heidenhain TNC640

Feeding it 10,40 or even 100MB of code is no problem for it.

 

I create surfaces from solid to machine the part.

Am I right thinking there is some kind of tolerance on creating the surfaces?

 

Thanks for the video, that was of great help especially the vector lines, that will help in the future for sure.

 

 

[#Rekd™]

Without a file it is a guessing game. 
 

Could you create similar geometry/ toolpaths and share the file?

[MrFish]

On 12/17/2022 at 10:05 PM, Joey5axis said:

Hello guys,

I have tried fiddling with these settings.

Tried machining a 190mm "Bowl" with unified multiaxis, strategy is great, single toolpath and cutting off center with a sphere mill.

However I still get the "flat spots" on the surface finish.

These parts need to be polished to high gloss so its important to me to get the best results possible.

Mind you my settings are METRIC.

Cut Tolerance 0.02 

Maximum distance 0.5

Maximum angle step 0.5

 

Unfortunately I am not allowed to share 3D files with anyone.

Machine is a DMG DMU75 Monoblock with Heidenhain TNC640

Feeding it 10,40 or even 100MB of code is no problem for it.

 

I create surfaces from solid to machine the part.

Am I right thinking there is some kind of tolerance on creating the surfaces?

 

Thanks for the video, that was of great help especially the vector lines, that will help in the future for sure.

 

 

you could try this, Lisa from CNC software sent me it a while back

You can improve the surface (and sheet solid as well) by adjusting the Chord Height Parameter in the Shading Settings.  This change will immediately render in the sheet solid, but you will need to use Regenerate display list to update the surface.  Regenerate display list is not currently in the ribbon or context menu, so I customized my context menu and added it from the Commands not in the Ribbon list.  Then I navigated to the view tab, and launched shading settings from the Appearance group and tightened the Chord Height tolerance to .001.  Next I right clicked in the graphics view and selected Regenerate display list.  Those steps removed the facets from both my surfaces and sheet solids.  Let me know if this does not work for you!

 

 

[cncappsjames]

In multi-axis cutting there's usually a minimum of 3 things in play BEFORE you even get to running a part on the machine;

1)Surface/Solid/Wireframe creation tolerance

2)Cut Tolerance

3)Point Spacing

In my experience (mostly FANUC), both 1 and 3 individually have a bigger influence on finished part quality than 2 does. Tightening 2 and doing nothing with 1 does nothing but hold you closer to what is already bad.

 

HTH

 

 

[#Rekd™]

One option often overlooked is using 3D toolpaths then using the convert to 5 axis operation. Possibly a Scallop toolpath will give you a better finish. 
 

 

[gcode]

Depending on the Unified toolpath you are using, this setting may or may not be available

 

Cut Pattern/Advanced Options/Method

by default it is set to approximate

try changing it to "Exact"

The Min/Max point distribution settings on the same page can help to, but the posted NC files can get pretty big

 

[Chally72]

On 12/17/2022 at 4:05 AM, Joey5axis said:

Hello guys,

I have tried fiddling with these settings.

Tried machining a 190mm "Bowl" with unified multiaxis, strategy is great, single toolpath and cutting off center with a sphere mill.

However I still get the "flat spots" on the surface finish.

These parts need to be polished to high gloss so its important to me to get the best results possible.

Mind you my settings are METRIC.

Cut Tolerance 0.02 

Maximum distance 0.5

Maximum angle step 0.5

 

Unfortunately I am not allowed to share 3D files with anyone.

Machine is a DMG DMU75 Monoblock with Heidenhain TNC640

Feeding it 10,40 or even 100MB of code is no problem for it.

 

I create surfaces from solid to machine the part.

Am I right thinking there is some kind of tolerance on creating the surfaces?

 

Thanks for the video, that was of great help especially the vector lines, that will help in the future for sure.

 

 

 

That cut tolerance is large, especially if you're using an accurate machine that can hold position well. You'll see more accurate machines leave more definitive "lines" or visual marks at point spreads. Are you using Cycle 32 smoothing? If so (which you should be) what settings?