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:

Cutter Comp Beginning on Arc Move - How to Avoid?


Bill H
 Share

Recommended Posts

On 6/19/2019 at 4:08 PM, Bill H said:

Sorry, I should have been more specific in my original post.  In the circle mill toolpath, you cannot use just a roughing pass, unless the diametral wear value in the control is zero because MC is invoking the comp on an arc move.  This is also true with thread milling ID threads, but fortunately in this case MC provides some lead-in/lead-out options to eliminate the problem.  I suppose the heart of my question is whether there's some setting that would prevent the invoking of comp on arc moves.

Sounds like a settings issue. I run a 3 Haas machines. A 1994 VF0, 2005 VF2 and A 2019 VF2. Use wear all the time and not an issue if your settings are correct.

For circle mill be sure you have it set for perpendicular and 90 degree. 

 

Capture.PNG.79b09c00faa7d2cc4d9a3e240e444332.PNG

 

Edit: If you want to contour an ID use the formula of ( dia. of hole - dia. of tool/2 * .4142 ) with a sweep of 135 and you will drop into the center of the hole and sweep on and off with no problems.

Example 1/2 inch hole with 1/4 inch endmill.

.500-.250 = .250/2 = .125*.4142 = .051775

Lead in and out line and arc .051775 with 135 degrees of sweep.

Works great for slots also.

  • Thanks 1
  • Like 1
Link to comment
Share on other sites
  • 1 year later...
  • 3 weeks later...
On 4/19/2021 at 4:59 AM, takefour said:

I am trying to preform a simple helix bore toolpath to expand a 1.250" Drilled hole to 1.408".

Under parameters when I select computer compensation everything works fine! However, it leaves no way to adjust at the machine for tool wear. When I select "Control" all I get is an alarm stating that "tool dia/nose R compensation start/cancellation is errenous" I can get the alarm to go away by setting the geometry and wear value in my machine to zero. However, again this defeats the purpose as it will not run with any other value other than zero!

Use "wear".

Link to comment
Share on other sites
  • 10 months later...

In that version you could use Contour Ramp and get G2/G3 on the moves. I would switch to that and call it a day using WEAR. You also have the ability to apply comp at the end and start of the Hole so you need to use Control it will apply the lead in above the hole giving you enough room to apply comp and the come out of the hole and turn off the comp.

Link to comment
Share on other sites

I have found that i get that sometimes when turning on multipass while roughing out a hole. 

To get around it i select "use entry point" on the lead in and out and ad the point.

doesn't work for ramping with point entry, which I still don't understand why mastercam won't let you use point entry while ramping. 

I rarely use helix bore and just choose ramp. 

Old school hahaha

Link to comment
Share on other sites
On 6/21/2019 at 2:07 PM, gcode said:

proper programming techniques will prevent most of these errors

 

for example

helix mill/wear comp/start at center/lead in set to 180°   will produce an error every time

switch lead in to 90° and you are good to go

 

There are a few things we're looking to do to alleviate these issues in the future:

-Change helix mill entry/exit sweep default to 90°. Because of the math being used to automatically create the lead arcs, 180 degree arc sweep and control/wear comp immediately put you into the scenario of turning on comp on an arc- and invalidate the use of Start/End at Center to get you that linear move. 

-Notify a user at toolpath generation that cutter comp is being activated/deactivated on an arc move, and suggest adding a linear entry/exit. This would replace the need to add this logic to the post just to see the issue that is being created at the toolpath level.

-Make it easier to add perpendicular entry/exit in a relevant way.

 

 

 

 

  • Like 4
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...