Deburr / Edgebreaks

[Andris Skulte]

I inherited a part from the last regime that has been getting deburred by hand, and I'd like to program a 1/4" spot drill to put a small chamfer on the sharp corners. There are quite a few compound curves on the part, so I figured I would solid model it, and have the tool follow the profile. What is the best way to have it get the edgebreak on a single pass? I put a .032 radius fillet on the corners to see what Mcam would do, but the various roughing/finish toolpaths all seem to generate way too much geometry, since I'm just looking to get rid of the sharp corners. Any ideas?

[Guest CNC Apps Guy 1]

Just do a chamfer(contour) toolpath, You can even use a ball end mill.

 

HTH

[richardtraver]

if your part is 3D the contour 3d chamfer may not be what you want. if it's a 2d chamfer you can use the 2d chamfer but not with a spotdrill you have to call it a chamfer mill. to do an edgebreake with a spotdrill select contour select your spotdrill and on the toolpath parameters page put a negitive stock to leave in XY and a negitive in Z. the combined stock to leave and -Z must equal the tool radius+however big you want the edgebreak

[cadist]

Create the curves on edges. and select them in contour. If it is a 3d profile mcam will automatically genrate a 3d contour. Define the depth (the size of chamfer)

[Andris Skulte]

Thanks guys. I'll give it a shot!

 

Andris

[Chris Rizzo]

I run into this situation alot... I'd try 3d contour with the chamfer option turned on...

 

HOWEVER depending on your part and the steepness of your 3d contour, a 45 degree chamfermill/spotdrill may gouge into the part too much in the steeper inclined areas. What I've done on some of our parts is create a smallish fillet (.020 in my case), and run a flowline toolpath on said fillet with a .250 ball em at about 150 IPM. Adjust the step over to make just a couple of passes, and she breaks the edge a heck of alot nicer than hand de-burring and in only an xtra minute or two....

[Bryan Johnson]

Mastercam does allow the "Chamfer" option with tools defined as Chamfer Mill or Spot Drill.

 

I use the same tool a lot for spot and chamfering, and find the Spot Drill tool definition to work best.

 

For a 3D chamfer, try a Ball Nose EM, and Surface Finish Project toolpath. Use neg. amount of stock for chamfer size. This gives an even result.

[crazy^millman]

Bryan have you tried this using wear as the cutter comp becuase I do it the oppsite way and it works. I use a chamfer mill for my spotting now and my chamfering and this has suprised me how well and seamless this works. I however have not been lucky getting the spot drill to work for chamfer operations.

[Chris Rizzo]

I'm a big fan of Surface finish project, however I've found it to take alot of trial and error to create two chains that work properly to "contain" the toolpath for and edgebreak. I have tried offset contouring chains then squashing many times, but I never seemed to get a nice little edgebreak toolpath without alot of aircutting.

[medaq]

1/4 " csinks do the trick also. I would stay away from the spot drill though.

 

Jim

[medaq]

Oh if you dont want to use 2d chamfer, Just write a normal contour, with your csink. If the first deburr was the top of the part z0. Just type in z-.12 and off set -.02. Should do a nice little chamfer.

 

Jim

[Bryan Johnson]

Spot Drill for Chamfering.

Yes, I use with contour, chamfer and cutter comp and have had no problems. Except you can not allow for any flat on the cutter.

 

The problem I have with using a Chamfer Mill as the tool type is that there is no option to define the default drill cycle. When I pick a drill I like for the cycle to be set automaticly.