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 with Surface Finish Flowline Toolpath - How to Eliminate?


Bill H
 Share

Recommended Posts

I have a part with an odd-size round-over edge and would like to cut it with Surface Finish Flowline Toolpath and a bullnose endmill.  My problem is that there are very obvious facets.  How can I eliminate these?  I've tried reducing the total tolerance from 0.001" to 0.0005", but the facets are still apparent.  Instead of using the solid geometry, I also tried creating a surface by sweeping a 90-degree arc along a path of lines and arcs.  This had no bearing on the facets.  What else can I try?

Link to comment
Share on other sites

Change the direction to follow the longer edge. If you start from the bottom, you don't have to do as much roughing or none at all depending on the size of the cut, tool, part etc.etc. Arc filtering is on the 3rd page under the "total tolerance" button That, and stepover are your only facet controls.

  • Like 1
Link to comment
Share on other sites
20 minutes ago, Bill H said:

JParis: My contract prevents me from posting the actual part file, but I've attached a sample piece that shows the problem.  I'd sure appreciate any suggestions on eliminating the faceting!  Also, what's with the crazy motion when the tool gets to the +Z extreme?

surface test.mcam 1.09 MB · 0 downloads

You using spiral and will need to tighten your tolerance and use a smaller step over. You have no arc filtering on.

Link to comment
Share on other sites
54 minutes ago, Bill H said:

crazy millman: Is spiral not a good idea?  What strategy and settings would you suggest?

I would do a zigzag to get true arcs. Spiral on that shape if you want a mirror finish is going to require 100,000 points and kick the tolerance down to .0001. With Arc you put the machine in my humble opinion in the best places to run like it should. Many discussions over the years about what is better on a machine. More code to let them machine do what it needs to less code to let the machine do what it should. There is so many factors that go into machining to say one way is the end all again in my humble opinion is ignorance. I am fluid in my programming style not rigid, but will do certain things in a certain ways. You have presented a simple fillet and when you run this on the machine what tests have been done to determine the sweet spot to make the best looking finish? What is the material you are cutting? What is the tool? What is the holder? The spindle Taper? the work holding? The coolant? Does the machine has TSC(Thru Spindle Coolant? If it does what pressure? What is the amount of stock left? Was the stock left in a stair-step roughing or was there a semi finish operation done? You are staring at the bottom and working your way up. What made you determine that was the best approach? I normally go top down to limit the tool pressure on the side of tool I would expect spiraling or zig-zag upwards would create. I have cut parts with .001 step over using a 1/16 ball endmill that ran for 40 hours. When that part was finished we vapor polished it and it look like glass. I have run mold inserts that looked like they were polished. I have a project running right now that is 16 hours of run time, but I was asked to hold a 32 finish with a .008 profile tolerance. I have rough, semi finish and then finish operation on the Swiss cheese part it turned out to be. 

Spiral is a good choice, but you have to feed it code and might think about using smoothing setting on the filter and give it .005 segment length. You program will grow by a factor of two, but more points the better. The other thing is that surface is bad to use. Make a solid fillet and then use that solid surface to drive the toolpath. Always try to use solid when doing any surfacing. Using surfaces by their very nature will be problematic since they can have gaps and not be water tight. The links to the screen shots are backplotted with what you posted and the other is with the smooth settings one with .005 and the other with .0015. Notice the difference in the gaps? I want to hold something really tight then I might go as small as .0015 gap. Now the file just went bigger by a factor of 40, but run that code and see the difference in your part. This is the last link.

https://www.dropbox.com/s/6b9kups5aqui1dv/Surface_no_filtering.png?dl=0

https://www.dropbox.com/s/zqaq2s1eap6qvdv/Surface_Smooth_Settings_005.png?dl=0

https://www.dropbox.com/s/0b6on817lanta2t/Surface_Smooth_Settings_0015.png?dl=0

 

  • Thanks 1
Link to comment
Share on other sites

crazy millman:  Wow!  Thanks so much for this explanation!  Looking at the linked images, am I right in thinking that endpoints are white and line segments are green?  I'm confused about filtering settings.  Does moving the slider to the right produce more arcs in your code or am I not understanding this?

Link to comment
Share on other sites

Here's another question:  I tried changing the cutting strategy to One Way, reasoning that the surface then becomes just a series of circles at different Z depths.  When I post this, however, there's not a single arc to be found; just linear X-Y moves.  Why?  Is there a way to get arcs?

Link to comment
Share on other sites
On 7/16/2022 at 3:51 PM, Bill H said:

I'm only looking for arcs in the XY plane. A slightly different radius at each Z depth.  Will it not do this?

If that has been turned on in Machine Control Definition. If not then the filter settings are ignored in the operation and the Machine definition take over.

On 7/16/2022 at 12:31 PM, Bill H said:

crazy millman:  Wow!  Thanks so much for this explanation!  Looking at the linked images, am I right in thinking that endpoints are white and line segments are green?  I'm confused about filtering settings.  Does moving the slider to the right produce more arcs in your code or am I not understanding this?

Yes the points are white and the moves between them are green.

You cannot use 50/50 you need to use 40/60 to get it to output code correctly. It is related to D-47584 that I am not sure has been addressed in 2023.

Link to comment
Share on other sites

Spiral method is cool, however it has it's ummmmmmm, tradeoffs too. With spiral, you tend to have leftovers on the 1st and last passes unless you have/can extend the surfaces... at least on the majority of  surfaces I have tried the strategy on. I'm sure theere are many feature topologies that it looks awesome on, just not many I have used it on. 

Like Ron and the other guys said, check your Control Def to make sure that you have the appropriate settings for arc creation "on" or enabled.  

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...