3D Chamfer in 2022

[[email protected]]

Hi all my 3d chamfer is looking really weird on the radius. Have any of you experienced this or know what's causing it?

[SN_MCam_User]

I'm curious on this also - using 2022 latest update - but saw similar solid edge jittery-ness on one solid feature edge the other day...yet smooth as glass on the opposite side of the part w a copied toolpath/identical feature. I was using 3D hybrid but decided to use a unified tp instead...and the strangeness "went away".  Merged solidworks model in my case.  

I just assumed I was doing something wrong...

[Chally72]

On 2/11/2022 at 9:14 AM, [email protected] said:

Hi all my 3d chamfer is looking really weird on the radius. Have any of you experienced this or know what's causing it?

If you can, please send me the part file so I can take a look. 

[[email protected]]

Do I need to check the toolpath files box when making the Zip2Go? I usually do, but not sure if it's needed. Also what are the ATP files? I imagine some kind of report about posting maybe? Anyway the 3D chamfer was fixed by adjusting arc filter tolerances but that is not something I ever had to do before. Also the Zip2Go ended up being 12MB with the toolpath files box checked. Where would you like me to send it? Or did you actually just want the whole Mastercam file?

[crazy^millman]

1 hour ago, [email protected] said:

Do I need to check the toolpath files box when making the Zip2Go? I usually do, but not sure if it's needed. Also what are the ATP files? I imagine some kind of report about posting maybe? Anyway the 3D chamfer was fixed by adjusting arc filter tolerances but that is not something I ever had to do before. Also the Zip2Go ended up being 12MB with the toolpath files box checked. Where would you like me to send it? Or did you actually just want the whole Mastercam file?

the Z2G does send the complete Mastercam file. ATP is Automatic toolpath processing and normally associated with Router.

[Chally72]

I took a look at the file. Having Roll cutter around corners set to ALL on the cut pattern page and having it enact changes upon the 3D splined edge at the corners of the part was inserting small arc segments that were causing this up and down noise. Setting it to Sharp or None drops it away without having to modify the tolerance!

[[email protected]]

So I looked at programs from my older versions of Mastercam and sure enough They are all set to Sharp. What is the purpose of setting it to All anyway? If I set it to sharp and put values in "internal corner rounding radius" and "external corner break radius" it will still "roll" the cutter around those edges and make the radius i put in their boxes right? Maybe I am misunderstanding the term roll. Anyway thank you for that hopefully it helps SN_Mcam_User too

[Chally72]

It changes what is considered a corner to apply this roll to. By setting it to All and then considering the 3D spline and trying to find/apply rolling to parts of the profile that might be considered corners, it was incorrectly applying arc motion to segments of those part corners. I'd expect it to have some trouble in scenarios like this, especially depending on where the model came from/what the shape of the spline was.