Chamfer Tool Path

[warrguitars]

What is anyones opinion on creating a chamfer tool path. For example, is simple rectangle with a .02 chamfer on the outside profile using a 45 degree milling bit. When I program it in such a way that I would normally approach it with my other cam program, madam does not do what I expect. So it seems that I need to make compensations in order to get madam to do what I need.


Thanks,

Mark

[keebler303]

You need to get your Z depth and effective diameter set correctly. The deeper you go in Z, the larger the effective diameter of your cutter. I normally just use an effective diameter of about half the full diameter of the cutter, then just adjust Z (through a tool length offset) to get the size chamfer you need. I'm sure any decent CAM program can do all this for you but on the stuff I use most there is no special handling of a chamfer tool so thats how I do it.

Matt

[svenakela]

Originally Posted by warrguitars What is anyones opinion on creating a chamfer tool path. For example, is simple rectangle with a .02 chamfer on the outside profile using a 45 degree milling bit. When I program it in such a way that I would normally approach it with my other cam program, madam does not do what I expect. So it seems that I need to make compensations in order to get madam to do what I need. Thanks, Mark

I have a lot of opinions, and if you describe the particular problem instead of talking in general terms I'm pretty sure I will reply with an answer.
Secondly, as long you don't describe the problem we cannot know why MadCAM is doing something you aren't expecting - which in the other hand very well could be because MadCAM knows the cutting better than you do. But I can't answer on that either because there are no facts to base an answer upon...

Have you ever read the book Catch 22?

/S

[warrguitars]

The project is a guitar bridge plate our of brass and has many details. I have success with all the slots and holes and profiles, etc. Just having trouble with chamfers.

One method that I have tried was to first use the taper cutter option and fill in all the details; I use 45 for the angle. Then I used profile as the 2D operation and chose the outside perimeter curve. I checked the "outside" option. I also set the Z -.02. The simulation shows the cutter cutting air (outside of the stock not above) and not the part. I then did the same but instead chose "on curve" setting as well as creating and choosing a curve where the chamfer began at the top face of my part (instead of using the outside curve like the previous operation I tried). The simulator showed that I was close to getting what I want but left a small ridge all around the part since the cutter did not go past the bottom edge of the stock.

I tried using a few 3D options and this did not work at all.

I can get a chamfer but I need to trial and error a bit with diameters and Z settings as if the cutter were just a end mill and eventually I can get the desired result.

I'm probably just missing something.... The style of madam is a bit different from what I have been use too. In so many ways I really like madam; hence my desire to learn the use of this tool.

Thanks

[svenakela]

If you use a taper cutter you should get what you want with a 2D profile. When doing chamfers small changes will make a noticable difference, or even uge differences.

Did you use the bottom profile of the chamfer? If there's no big deal if the chamfer differ a little bit from drawings, you could use the bottom profile of the part and then adust the height of the 2D cut. In the end, it's really important that you set the tool correctly in the machine as well, a fraction higher or lower and the result will be something else. But you probably know that.

[warrguitars]

Well, the way I am dealing with it at this moment is thus... I am drawing an offset then adding to my depth in madcam. i.e. if I want a .030 chamfer, I draw an offset curve of .020 and assign a cutting depth of .050. Using a taper of 45 degrees, this method gives me a beautiful chamfer cut of .030 and the tool tip is past my stock so I leave no slight edge.

[Dan B]

Sounds like you have this working well for you. We do something similar, except that we offset the curve and move it down. Then we program to Z0. We've established constants for the moves that will provide the chamfers we want.

Dan