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:

dynamic contour, be careful!


Seedy steve
 Share

Recommended Posts

12 hours ago, Seedy steve said:

dynamic contour... the finish pass ignores the set minimum toolpath radius!)

It is incredible that a simple aspect of a basic path can be completely ignored !

I don't get it.

If you are running a finish pass, you want the toolpath to follow the part profile.

If you have a minimum toolpath radius set that is bigger than a finish radius, you'll be leaving stock

and it won't be a finish pass.

Am I missing something

 

  • Thanks 1
Link to comment
Share on other sites

That minimum toolpath radius is controlling the roughing motion of the path, not the finishing. In what situation is this causing a problem? Have a picture or file? My guess would be that you had it set to a large value, the roughing left a lot in the corners because it was respecting that value, and then the finishing path came in and overengaged and perhaps broke a tool?

  • Thanks 1
Link to comment
Share on other sites
6 hours ago, gcode said:

Am I missing something

All the broken tooling that happened because the tool dives in to a corner taking all the material that it just carefully left behind!

I tore the flutes off  endmills over and over before I figured out this fault! it took three years to figure out why.

I rarely used the path, and on tool steel less than that. hence the three years of smashed endmills.

What is the min. radius for if not to save the tool from a right angle corner?

a right angle corner won't be finished either way.

the response from cnc software was... basically Yes that is a bug that will be fixed. 

p.s. good to hear from u Gcode .. RESPECT.

Link to comment
Share on other sites
5 hours ago, Chally72 said:

finishing path came in and overengaged and perhaps broke a tool?

oh ya! every time ! the last time was a brand new 3/4 long series end mill. I was taking about .002" when it hit the corner and was destroyed!

I  was not expecting to have to look at this path with such scrutiny! 

  if I wanted to ignore that setting I would just use a simple contour path to finish.

it is ridiculous to have a setting that, anonymously, only applies to part of a tool path!

it is not that way in 2d contour . if I set a min. radius it listens!

Link to comment
Share on other sites
6 hours ago, Chally72 said:

In what situation is this causing a problem?

I program and machine about 40 to 60 parts per month hurray for 5 axis if only temporary .

so it comes up every so often. when there is a smaller tool following a larger one to pick out corners better.

(it should be called left over by how it works.)

thanks Chally72 for replying.

Link to comment
Share on other sites
7 hours ago, gcode said:

I don't get it.

 I don't get it... how is it EVER helpful to encounter a sudden gob of material at the apex of an internal corner when finishing?

Or for that matter, to find any extra material any where when on a finish path ?

That makes no sense! at best it causes chatter.

sometimes the engineers need the sharp corners, so I pick it out in a different setup, other times the radius is irrelevant so I can leave it.

 

Link to comment
Share on other sites
  • 9 months later...
On 3/30/2021 at 11:51 AM, Chally72 said:

That minimum toolpath radius is controlling the roughing motion of the path, not the finishing. In what situation is this causing a problem? Have a picture or file? My guess would be that you had it set to a large value, the roughing left a lot in the corners because it was respecting that value, and then the finishing path came in and overengaged and perhaps broke a tool?

Hey Chally, any I idea if they fixed this flaw yet? 

It is NEVER  good to leave stock in a corner for the finish path.

If it is fixed, I might update from mc2019

S.

Link to comment
Share on other sites

Hey Steve, this isn't my area and honestly I'm confused by the request. The minimum toolpath radius you rough with determines what's left to clean when you take your finish pass. The path is doing exactly what you ask it to do and I just don't see it as an issue when I use this path.

The functionality is identical to if you say, used an Optirough to cut a pocket and then used a Contour to finish the walls. Your corner stock to clean is dependent on what you told the Optirough to use for a minimum radius. To ask for different behavior is to ask that the path ignore the values you're entering in Minimum Toolpath radius. It's also completely valid to have a roughing with a large minimum toolpath radius and then do a finishing pass with a feedrate/rpm override that takes a slower pass with a bigger chunk all at once.

 I'd recommend emailing your reseller to get an official request number for this so that the Mill product owner can look at it with the team- my opinion on this functionality is just that- an opinion and not the final word- and they might have a different view. If you already have a request number, you can post it or message it to me and I can take a look and see the current status and let you know what's going on with it.

  • Thanks 1
Link to comment
Share on other sites

"Yes, this is a legit problem. The finish pass of a Dynamic Contour toolpath is simply driven directly to the chain, with no regard of the minimum radius setting. We have request #R-14452 logged to add support for a separate min radius for the finish pass."

1 hour ago, Chally72 said:

If you already have a request number

found  the reply.

Link to comment
Share on other sites
2 hours ago, Seedy steve said:

"Yes, this is a legit problem. The finish pass of a Dynamic Contour toolpath is simply driven directly to the chain, with no regard of the minimum radius setting. We have request #R-14452 logged to add support for a separate min radius for the finish pass."

found  the reply.

Awesome. Can confirm that R-14452 is still an active item.

  • 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...