hongerrr

2D pocket milling doesn’t recognize nose radius of endmill for step over

Recommended Posts

Hello all, 

when I do a facing pocket pattern that leaves islands I’m noticing that the tool path doesn’t change when I change my tool nose radius for an endmill. It’s leaving unwanted materials due to it not calculating the nose radius of the endmill. Is there way around this? Or another cycle? I’m currently using MC 2017. Any help would be greatly appreciated. 

Share this post


Link to post
Share on other sites
6 minutes ago, hongerrr said:

Hello all, 

when I do a facing pocket pattern that leaves islands I’m noticing that the tool path doesn’t change when I change my tool nose radius for an endmill. It’s leaving unwanted materials due to it not calculating the nose radius of the endmill. Is there way around this? Or another cycle? I’m currently using MC 2017. Any help would be greatly appreciated. 

Sorry no the step over is the step over and it is the job of the programmer to think about the effective size of tool doing the cutting. You had the same step over with a ball endmill the cusp would be extremely bad. You have a 1" bull endmill with a .12 R then the effective cutting size is .760. I would make sure my step over is around .456 to maybe  go up .600 but I never like go more than 60% of the effective step over for finishing pockets. For roughing I go high as 95% depending on the tool and other factors. 

  • Like 1

Share this post


Link to post
Share on other sites

seems to me, long ago there used to be a chook for this exact thing

Share this post


Link to post
Share on other sites

Thanks for the quick response guys! I’m a long time Esprit User, have also been programming in Hypermill for like 2 years now. It just seems so antiquated to have to play with the step over settings to see if it cleans up or not. 1” E.M. with .120 rad with a .750 step should clean up. I think it’s pretty straight forward. Once again thanks for the quick response and let me play with my stepovers while cursing at the screen. Haha 

Share this post


Link to post
Share on other sites
3 hours ago, hongerrr said:

Hello all, 

when I do a facing pocket pattern that leaves islands I’m noticing that the tool path doesn’t change when I change my tool nose radius for an endmill. It’s leaving unwanted materials due to it not calculating the nose radius of the endmill. Is there way around this? Or another cycle? I’m currently using MC 2017. Any help would be greatly appreciated. 

That's what 2d dynamic mill is all about, let Mastercan deal with the toolpath,area mill also I believe wont leave islands.

Share this post


Link to post
Share on other sites
3 hours ago, hongerrr said:

Thanks for the quick response guys! I’m a long time Esprit User, have also been programming in Hypermill for like 2 years now. It just seems so antiquated to have to play with the step over settings to see if it cleans up or not. 1” E.M. with .120 rad with a .750 step should clean up. I think it’s pretty straight forward. Once again thanks for the quick response and let me play with my stepovers while cursing at the screen. Haha 

Try creating your own end mill with the radius you want .dxf style.

Share this post


Link to post
Share on other sites
On 10/15/2020 at 12:25 PM, hongerrr said:

It just seems so antiquated to have to play with the step over settings to see if it cleans up or not.

That's because it is antiquated. ;)

Share this post


Link to post
Share on other sites

The "Pocket" algorithm dates from the 80's I believe.  There are the "Parallel Spiral, Clean Corners" and "Constant Overlap Spiral" methods which may help.  As said above, "2D Dynamic" is the modern way of doing it.

 

Share this post


Link to post
Share on other sites
On 10/15/2020 at 8:44 AM, hongerrr said:

Is there way around this? 

The old legacy pocket routines are primitive to say the least, but they do work

Calculate the stepover yourself 

(Tool dia - ( radius x 2)) x .6

Use that value for stepover

Share this post


Link to post
Share on other sites

I am going to play around with this 2D dynamic stuff and see what it’s all about. I originally asked if there was maybe another cycle, and it seems like 2D dynamic tool path is where it’s at. Like every other software that I’ve been on, I am sure Master cam has its pros and cons. I will enjoy finding things out. One things for sure, the Mastercam community seems to be one of the biggest and most helpful so far. Thanks guys! 

  • Like 1

Share this post


Link to post
Share on other sites

Some info here on Dynamic motion in Mastercam.

 

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!

Register a new account

Sign in

Already have an account? Sign in here.

Sign In Now

  • 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