Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Faceting


So not a Guru
 Share

Recommended Posts

I've used filters for ever.  Generally I don't have the faceting problem, the main reason I use it is to make the programs smaller and because it gives smoother tool motion.   I see here that everyone seems to have One Way Filtering off, I've always had it on, without really know what it changes, or why it should be on/off.  Anybody know what that setting does different?

  • Like 2
Link to comment
Share on other sites
3 hours ago, AMCNitro said:

I've used filters for ever.  Generally I don't have the faceting problem, the main reason I use it is to make the programs smaller and because it gives smoother tool motion.   I see here that everyone seems to have One Way Filtering off, I've always had it on, without really know what it changes, or why it should be on/off.  Anybody know what that setting does different?

I would like to know as well. Good question.

Link to comment
Share on other sites

One-way Filtering is used with a Zig-zag Cut Pattern, to be sure the path is only filtered in "one-direction", of the tool motion. This means that if you are outputting Arcs in the G19 or G18 plane, that the segments of the path will have better alignment. Without this on, during Zig-zag motion, the path can be filtered in both path directions, but with output that doesn't necessarily "line up" with the last/next pass.

To be clear: it has no effect on One-way or Spiral Cut Patterns. 

  • Like 2
Link to comment
Share on other sites
On 9/17/2021 at 9:29 AM, SlaveCam said:

Don't forget to set control to "free cutting mode" instead of "accurate cutting mode". It could make a huge difference. Unless, of course, there is surface tolerance.

Where are these parameters located? Also, why choose free cutting mode over accurate cutting mode?

Thanks

Link to comment
Share on other sites
1 hour ago, Metallic said:

Where are these parameters located? Also, why choose free cutting mode over accurate cutting mode?

Thanks

G61 is exact cutting mode; G64 cancels exact cutting mode, essentially allowing the control to make use of the various parameters that are set for smoothing.

G61 forces the machine to come to a complete stop, at every point programmed, before beginning the next move. This often creates chatter & finish problems and is why a lot of shops run in G64.

Link to comment
Share on other sites
On 9/22/2021 at 8:04 PM, So not a Guru said:

G61 is exact cutting mode; G64 cancels exact cutting mode

On Mazatrol there is G61.1 (contour control) which is on by default, at least on our machines. You have to use incredibly tight values for filtering and smoothing to avoid faceting. With G64 the contour is not followed so strictly, allowing for smoother and less precise movement.

I have exprimented with the K parameter and even with that, it is hard to match G64 in terms of smoothness.

  • Like 1
Link to comment
Share on other sites
5 hours ago, SlaveCam said:

On Mazatrol there is G61.1 (contour control) which is on by default, at least on our machines. You have to use incredibly tight values for filtering and smoothing to avoid faceting. With G64 the contour is not followed so strictly, allowing for smoother and less precise movement.

I have exprimented with the K parameter and even with that, it is hard to match G64 in terms of smoothness.

Yes, we have 3 Mazaks, I have changed the parameters to have them all default to G64. My posts all have misc value functions that allow us to set the G61.1 settings.

Do any of your Mazaks have the Smooth X controller?

Link to comment
Share on other sites

G61.1 is used here...mostly in 2 uses....it is required for feed rates over 315 IPM and with tight corners.....a .065"R with a .125" Ø endmill...either G61.1K10. or G61.1R.001

If I am surfacing, those paths that need it will get G05 P2 on the newer smooth it's G05P2 P0 - P20 depending on the tuning necessary for the desired result.

Link to comment
Share on other sites
1 hour ago, JParis said:

G61.1 is used here...mostly in 2 uses....it is required for feed rates over 315 IPM and with tight corners.....a .065"R with a .125" Ø endmill...either G61.1K10. or G61.1R.001

If I am surfacing, those paths that need it will get G05 P2 on the newer smooth it's G05P2 P0 - P20 depending on the tuning necessary for the desired result.

Is this on Mazaks?

On ours we use both G5 P2 & G61.1 P# (P1 - P20). often simultaneously.

  • Like 1
Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...