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:

Rest Machining


JB7280
 Share

Recommended Posts

I machined the outside of my part with a .5 endmill.  I want to do some rest machining with an .125 endmill for some inside radii.  I got the toolpath almost how I want it, but there's a few questions I have.

 

1)I'd like to do the corner machining, without the it milling the whole profile.  The straight segments, and outside corners have already been milled.

2) The toolpath lines on the screen show a feed line throughout.  I would want it do move at my transition feedrate in between cuts.  I can make it retract, and rapid, but I'd like to keep the tool down, and reposition.  

 

**edit-after posting the code, i looked, and it seems that it IS doing a micro-lift, then repositioning at 800ipm like i wanted, but usually my transition/repositioning moves show as brown lines.**

 

Thanks!

rest.jpg

Link to comment
Share on other sites
6 minutes ago, Seedy steve said:

in cut parameters click the drop down for contour type and select remachine...

He's using a Dynamic toolpath, that's the move around the part......it's set to keep tool down always

 

Any feed move will show a a feed color 

Link to comment
Share on other sites

Instead of a dynamic path, you could go with a 2D contour-remachine. That's more of a straight to the point toolpath that will only machine where it finds stock based on the parameters that you give it.

In the 2D contour parameters, there's an option for 2D, ramp, or remachine.

Link to comment
Share on other sites
1 hour ago, JB7280 said:

still trying to do the whole, or most of the outside profile.  I'm attaching a Z2G, in case anyone wants to take a look at it.

13704402.ZIP

If you're just trying to get it to clean the corners, rather than using "all previous operations", set it to "roughing tool diameter" and set the diameter of the roughing tool a little over .5 to compensate for your "min toolpath radius"  used in your dynamic path.

 

plVXM9B.png

Link to comment
Share on other sites
11 minutes ago, Neurosis said:

If you're just trying to get it to clean the corners, rather than using "all previous operations", set it to "roughing tool diameter" and set the diameter of the roughing tool a little over .5 to compensate for your "min toolpath radius"  used in your dynamic path.

 

Got it!  That did exactly what I wanted.  Thanks!  I like your dark background, and model transparency, btw.  I'm gonna give that a shot.  Thanks again.

Link to comment
Share on other sites
21 hours ago, Neurosis said:

If you're just trying to get it to clean the corners, rather than using "all previous operations", set it to "roughing tool diameter" and set the diameter of the roughing tool a little over .5 to compensate for your "min toolpath radius"  used in your dynamic path.

Basically, the same thing is accomplished, but to use the parameters properly, enter .5 for your roughing tool diameter and then enter a value in the Clearance field to extend the toolpath enough to accommodate any other stock, such as the min toolpath radius, allow a little bit of overlap, etc. Nitpicking, I know, but I just wanted to point it out since JB is a new MC user.

Another helpful hint is to click the ? on any parameter page and then click the Field Definitions tab. It tells you what each parameter on the page does.

  • Like 1
Link to comment
Share on other sites
1 hour ago, Thad said:

Basically, the same thing is accomplished, but to use the parameters properly, enter .5 for your roughing tool diameter and then enter a value in the Clearance field to extend the toolpath enough to accommodate any other stock, such as the min toolpath radius, allow a little bit of overlap, etc. Nitpicking, I know, but I just wanted to point it out since JB is a new MC user.

Another helpful hint is to click the ? on any parameter page and then click the Field Definitions tab. It tells you what each parameter on the page does.

Thanks again Thad!  Nitpicking maybe, but it's actually more important to me than it probably should be to use the software correctly.  "Tricking" the software, or lying to the machine is a huge frustration to me, even though sometimes it may be the only solution.  And yes, when I remember, I try to use the "?" button.  Unfortunately sometimes I just get in a hurry and forget it's there.

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...