1. ## Chamfering question

Hello, lets say I have a plate with a 0.75" hole in it. I want to put a small chamfer on the top (inside) of the hole just to break the edge, so I don't have to do it by hand. So I go into Mastercam X4, select circle mill, set up my 90° 0.5" chamfer mill. Is there a way to set up my offsets for the chamfer mill, so I am not using just the tip of the tool? I want to use something like 2D Chamfer, but everytime I use 2D CMFR, the tool always starts on the outside of the hole, instead of the inside, is there a better way? I am new to Mastercam, thanks.

2. Hi, click on the geometry tab of the operation, right-click on the chain and then select "change side". Regenerate and the tool will cut inside of your circle.

3. Thank you, that helped for the start of the tool. However now it says that the tool is too small to create the chamfer. I am using a 12 mm chamfer tool, with a .039" diameter flat on the bottom of the insert, and a .472" diameter on the diameter of the whole insert. In the 2D chamfer I am using .1" for the width, and 0.0 for the tip offset, so I can use the side of the insert instead of the tip so it doesn't leave a flat on the chamfer. The tool diameter in the tool page I am using .039 for the flat. If I use .472 (12mm) it creates too large of a chamfer. My Z depth in the Linking parameters is 0.0. I am not sure what to do next.

4. Forget the "Circle Mill" and just use "Contour". Then, since your angle is 45^, offset the edge you want to chamfer. Go equal amounts over and down. If you offset a 1/4" your cut depth will be 1/4".

• If you zip and upload your .mcx file I can have a look at the parameters.

• Originally Posted by utengineer04
Thank you, that helped for the start of the tool. However now it says that the tool is too small to create the chamfer. I am using a 12 mm chamfer tool, with a .039" diameter flat on the bottom of the insert, and a .472" diameter on the diameter of the whole insert. In the 2D chamfer I am using .1" for the width, and 0.0 for the tip offset, so I can use the side of the insert instead of the tip so it doesn't leave a flat on the chamfer. The tool diameter in the tool page I am using .039 for the flat. If I use .472 (12mm) it creates too large of a chamfer. My Z depth in the Linking parameters is 0.0. I am not sure what to do next.

.1" width is more than 'just breaking the edge'. Use 0.01" as width
Always add a something to the tip offset unless you are chamfering straight off a flat face. try 0.02"
For best results always have a lead in bigger than the chamfer you are cutting!

Hope this helps

C

• The guy's are correct, don't use circlemill

Tool
Use a chamfermill, set the point diameter and Taper angle very accurately ( these are what are used in the toolpath calculation )
Op
use 2D contour
Top of stock = the TOP face of the chamfer
Depth = the TOP face of the chamfer
XY stock to leave = 0
Z stock to leave = 0
Contour type = 2D chamfer ( or 3D chamfer- with some restrictions )
Width = 0.01" ( will give this size chamfer )
Tip offset = 0.04" ( how far the tip extends below the bottom of the width size ) ( adjust only this to make it cut higher up the flutes )

line perpendicular length = 0.05"
arc = 0 ( you can try 0.05" )
arc sweep = 45°

then, copy LH to RH

PS
on profiles, you can lengthen or shorten the path, if near walls etc.

using the above settings, the tool tip will be passing 0.05" below your "Depth" value setting [0.01"+0.04"])

• Originally Posted by Superman
The guy's are correct, don't use circlemill

Tool
Use a chamfermill, set the point diameter and Taper angle very accurately ( these are what are used in the toolpath calculation )
Op

PS
on profiles, you can lengthen or shorten the path, if near walls etc.

using the above settings, the tool tip will be passing 0.05" below your "Depth" value setting [0.01"+0.04"])

Thank you very much, that is what I was wondering, what diameter is used to create the toolpath. Excellent, thanks for everyones help, I appreciate it.

• I've had troubles getting the chamfer operation to perform exactly like I wanted. What I prefer to do instead is define a 45º angled too with an outside diameter of, say, 0.25, tell it to do down half of it so mastercam thinks it's right on the edge. Then, in reality I use a tool with a larger diameter, like 3/8" or more (depending on what the geometry allows). Use CDC with the toolpath and program it as 0.25 in your machine's CDC diameter register. The machine will compensate the tool enough that it doesn't cut in the middle, and doesn't cut on the absolute edge either.

Basically I call upon the number in the CDC register to determine what will happen on the fly. It can be useful when you have inside edges being chamfered, where you don't have much room to go crazy with large tools.

• Use contour and select 2D Chamfer instead of just 2D.
Set the amount of chamfer you need (.012).
Depth will be how much past the bottom of the tool you want.

It's really very easy. No math required.

Mike Mattera

SEO Blog

#### Posting Permissions

We are the largest and most active discussion forum from DIY CNC Machines to the Cad/Cam software to run them. The site is 100% free to join and use, so join today!