Exact Stop G61

[ujmujm]

Where is the parameter in Mastercam to do a exact stop (G61) I'm milling a deep pocket with .125 corner radii with a .250 end mill and I would like dwell in the corners so I won't get chatter any help would be appreciated.

Thanks

[Leon82]

I feel that's a way to get extra chatter.

 

I would drill it indersize when it's whole then peck the end mill slow to clean the radius out

 

Or rough, peck, finish with a internal corner radius like .005 or so

[Leon82]

I'm not sure if it's available in canned text but you could use a manual entry before the finish paths

[crazy^millman]

56 minutes ago, ujmujm said:

Where is the parameter in Mastercam to do a exact stop (G61) I'm milling a deep pocket with .125 corner radii with a .250 end mill and I would like dwell in the corners so I won't get chatter any help would be appreciated.

Thanks

That would be a post modification not a Parameter in Mastercam. Like what was mentioned could use Cantext to turn it on where needed. The use of G61 will be for the whole toolpath unless you turn it on and off in specific areas then you must use the toolpath editor and Cantext to do that.

[Guest]

That's gonna squeal like a mofo.....

You might try conventional milling the walls.....but if there's some tolerance on those rads I would use every thousandth available of it so I could to get some motion through that corner

Edited August 2, 2018 by Guest

[jlw™]

You can use can text to output things like G09, G61, and G64 and other words.  Very easy post mod.  Do you have a purchased or generic post?

[jeff]

2 hours ago, ujmujm said:

Where is the parameter in Mastercam to do a exact stop (G61) I'm milling a deep pocket with .125 corner radii with a .250 end mill and I would like dwell in the corners so I won't get chatter any help would be appreciated.

Thanks

What is the tolerance on those corner radii?

If it were me, I would set the internal radius to .01 so that the end mill actually contours those rads.

 

[navsENG]

Try it, but if I had to mill that I would likely bore the corners out if I couldn't use a smaller tool. That rarely works , and usually your radii will always show big. 

[Mark VIII]

Use can enter the G61 manually by using the manual entry box in the "change at point" dialog. Right click on tool path and select "change at point". However, you would probably want to use G09 instead of G61 so the exact stop only activates on single lines of code instead of affecting the entire path.

[motor-vater]

I'm no expert but I do usally alot of deep pockets like you mention. For me Depending on the size of the pocket I would use a really nice (helical solutions maybe) 3/8 endmill dynamic rough it, then run a finish contour, and run it through high feed mode to slow it in the corners. Probably not what you are looking for but works for me. If deflection is a problem use a reduced shank endmil and step downs.

EDIT.. Sorry missed it in the OP thought we were talking 1/2 inch here. Same principles apply though, 3/16 for the finishing tool reduced neck with step downsand high feed.

[Newbeeee™]

If it is deep, look at the tolerance on you corner rad. If it's +/-.005, then tweak your geometry to .130Rad.

Frill the corner out .125R (1/4 drill) and profile it to finish to the top of the drill angle.

Add another op with a smaller stepdown to then profile from the top of the drill angle to the final depth, otherwise the extra mtl in the bottom may overload the tool.

If it's a production part, I've drilled corners first, then G73 the corners to size but with the centre point of the G73 op "inwards" of the sidewall. This then has taken out most of the mtl and the bottom of the hole, but still left a small radial amount of mtl, so it can be finish profiled (and clean up).

I'd never used exact stop in my life, and would never even try it in this application.