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:

Control cutting diameter with ballnose


BBprecise
 Share

Recommended Posts

Been doing a lot of work lately using 5x parallel toolpaths. As everybody knows near the tip of any ballnose a 4flt becomes 2 effective (approx. Ø.2 on a Ø1/2" ballnose).

What I'd like to know is if there is a way to get Mastercam to automatically tip the tool so the effective cutting dia of the tool on the part is larger then Ø.2?

I know I could break down every section and change the tilt angle of the tool to whatever angle I need, but on the part I'm doing currently I'm looking at having to make 50+ sections to control this. Would be pretty sweet if Mastercam could do this. I would think it would be a fairly simple function, but that's in my head.

Thanks.

Link to comment
Share on other sites

I'm using a tilt angle of 30º right now John. Which for the majority of the area I'm machining is fine. But there is a spot in that section where the 30º makes the ballnose cut on the tip or at a dia smaller then Ø.2. 

When I've used lead/lag angle before Mastercam still ends up cutting on the center of the tool a little bit.

Now maybe I'm being to demanding on not wanting to cut on the center at all and that there's no way I can completely eliminate it. I was just hoping there was a way to get Mastercam to recognize what the effective cutting dia of the tool is (in relation to drive surfaces and not the stock) and tilt the tool so it can maintain the minimum effective dia.

 

Link to comment
Share on other sites

There are options in Tool Axis Control for Unified/Parallel to tilt by contact point rather than angle. There are also more enhanced contact point controls in Pocketing- Wall Finishing and Pocketing- Floor Finishing. It's hard to offer more suggestions without a part file to use as an example.

  • Thanks 1
Link to comment
Share on other sites

I am thinking it would be a kin to how Mastercam calculates toolpaths for "Accelerated Finishing" tools. Knowing the shape of the tool and specifying the contact angle Mastercam will orientate the part so the drive surfaces stay at the proper orientation.

Link to comment
Share on other sites
19 minutes ago, Chally72 said:

There are options in Tool Axis Control for Unified/Parallel to tilt by contact point rather than angle. There are also more enhanced contact point controls in Pocketing- Wall Finishing and Pocketing- Floor Finishing. It's hard to offer more suggestions without a part file to use as an example.

This is the zone I'm looking at. As you can see near the end of op#2 the tool is cutting on the tip.JUNK1.ZIP

Link to comment
Share on other sites

Attached is an example. Here's what I changed- I swapped tool axis control to Surface with Tilt, and then set the Side tilt definition to ortho at each contour, which gets you an averaged positioning across each slice that roughly mimics what you were doing with the original Fixed to axis strategy, but allows the toolpath to properly react to the changing surface vector near the top of that geometry. The 30 degree tilt angle is then respected per pass as you travel along the part. No need to even get into contact point controls instead.

 

2053412883_Anglechanges.thumb.jpg.7cc884042338a53ceb2058295b7c837d.jpg

DGG Example.mcam

  • Thanks 1
  • Like 2
Link to comment
Share on other sites
33 minutes ago, Chally72 said:

Attached is an example. Here's what I changed- I swapped tool axis control to Surface with Tilt, and then set the Side tilt definition to ortho at each contour, which gets you an averaged positioning across each slice that roughly mimics what you were doing with the original Fixed to axis strategy, but allows the toolpath to properly react to the changing surface vector near the top of that geometry. The 30 degree tilt angle is then respected per pass as you travel along the part. No need to even get into contact point controls instead.

 

2053412883_Anglechanges.thumb.jpg.7cc884042338a53ceb2058295b7c837d.jpg

DGG Example.mcam 2.72 MB · 0 downloads

I see what you did and it looked good except right at the very end it drove the tool thru the surfaces. I'll have to go back and and finished model to the file and see if I can fix that with collision or something.

Also looks like it might be tipping the part to far and slam holder in to part, but you wouldn't know that because you don't have a completed model. I'll adjust the tilt angles in collision control to restrict how far Mastercam can rotate the trunion.

Appreciate the help on this.

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

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

 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

×