[jcnewbie]

Lets say I have a contour with with a 45 degree chamfer on one end. contour toolpath I select 2D chamfer and the chamfer dialog.

It asks me to enter in a width. What should I enter in for the width and tip offset. Should it be based from the chamfer tool I am using ?

[Matt Berube]

The width would be the desired width of the chamfer.

The tip offset is how much of your cutter you want to be cutting air below the chamfer.

Mostly I use .020 for smaller stuff but around .080 for large items. The only reason I think I'd change it would be if you:

1. Have limited clearance around the chamfer and need to avoid gouging another feature

2. Want to use different areas of the carbide insert to maximize insert life...

Play with the options a bit and use "verify" to ensure you're getting the desired result.

[Superman]

Lets say I have a contour with with a 45 degree chamfer on one end ??????. contour toolpath I select 2D chamfer and the chamfer dialog.

It asks me to enter in a width. What should I enter in for the width and tip offset. Should it be based from the chamfer tool I am using ?

1/- Is the chamfer just at the end of the contour ?
eg a vertical corner of a shape
or
2/- Is the chamfer along the upper face of this contour ?

If 1/-, then incorporate the "end" chamfer into the operation that "side mills" this feature

If 2/-, then contour type is a 2D or 3D chamfer
contour to select is the one that describes the vertical wall
"top of stock" is the top of the chamfer, depth is also the top of the chamfer
Chamfer dialog- width is the size of chamfer, tip offset is how far past the bottom of the chamfer

eg
width=0.1"
tip off = 0.05"
output Z depth will be -0.15" below the top of the chamfer
note!!!! --- you must describe the tool correctly and accurately

[jcnewbie]

Thank you ! Thank you ! This forum is freakin amazing !

[thebowman]

"Should it be based from the chamfer tool I am using?"

Yes. Don't forget that chamfer tools often don't come to a perfect point and have a flat on them. You have to compensate for this.

[Superman]

"Should it be based from the chamfer tool I am using?"

Yes. Don't forget that chamfer tools often don't come to a perfect point and have a flat on them. You have to compensate for this.

Try not to use a "Drill" or "Spotdrill" for chamfering as these are drawn to a point
Use a "Chamfer Tool" to define the spotting drill and everything will be OK and there will be no need to fudge it.
This tool can be used both for spotting ( to give a diameter chamfer ) or for creating a chamfer in a contouring operation.