Chamfering Techniques

[Nominal]

What is the proper procedure to mill a chamfer using V9? Here's the way I've been going about this, if someone has a better way I'd like to hear it. For simplicities sake lets say I have a piece of material thats been milled to .100" thick. Along one edge you need a .06 x 45 deg chamfer. In mastercam I'd offset the edge in .080. I'd do a regular contour on that line and give the depth as an absolute value of .120". This way I'd comp the dia of the tool to what its dia actually is using wear offsets, and set the length to the intersection of the angle and the outside dia. This gives me the best chance at a perfect chamfer from go regardless of how the chamfer tool has been ground at the tip. The only problem with this method is it can't be verified graphically since mastercam thinks the tip of the tool is .020 above the part. I screwed around with the chamfer 2d setup but its not making sense to me and the system help on it isn't very much help. Thanks. Hoping I don't get flamed too badly for this one :-)

[Keith Graydon]

Hi Nom,

 

here is what i do. Im sure ill get arguments from many sides but that is OK.

 

 

Chamfer .06 regular contour path

using a .250 dia 90 degree countersink. I use NO side passes and one or two base passes with the final at about .005 for finish. for .06 deep i'd use 2 paths. for cycle time i'd only use one.

 

 

Stock left XY -.115

 

depth of cut -.07

 

this method allows that the tip of the tool might not be a perfect point. AND, you can use ANY diameter tool within reason of course.

 

You can see the chamfer in verify too

 

 

[ 02-27-2003, 03:59 PM: Message edited by: Keith L. Graydon ]

[chris m]

We program the "real" size of the chamfer and use mostly inserted chamfer tools so the tools aren't hacked up; we know what they will be (within reason). If you don't know exactly what tool the guy is going to use in the machine, one thing you could do is program the correct chamfer size and establish a policy in you shop that the guys comp all of the chamfer tools up .020 or .030 as a rule when setting up. You'll probably find they do that anyway; it sucks making a nice part and blowing it on the (typically) last operation because you chamfer tool cuts way O/S.

 

C

[P_Scott]

Nominal,

 

Use the 2D Chamfer Contour toolpath in Mastercam as follows. Chain the geo. at the top edge (non-chamfered geo.) of your part. Set to Absolute depth at top edge of part, or Incremental 0". In the Chamfer button, set your chamfer width and Tip Offset, which allows for the depth to be adjusted so there isn't a scribe line at the bottom of the chamfer. Mastercam will calculate the depth by adding the Width and TO values together, based on tool angle and land size greater than the Width and TO specified. HTH

[Rekd™]

Yeah, what Peter said.

 

The 2D Chamfer option in Contour Toolpaths is da bomb.

 

'Rekd

[cadcam]

I perfer Petters way but I have done it the the other ways suggested to.

 

there are alwas advantages to have more then one way.

[Toolfab]

I'm with Jay, I preffer Peters method but its always better to leave your options open!

[MetalMarvels]

The 2D chamfer works very nicely and I have also successfully used it to chamfer around a contour that varied in Z-height. The only "issue" that I have had is properly setting up a flat-pointed chamfer mill, when it is somewhat difficult to accurately measure the diameter of the flat. I agree with Chris M - when using a chamfer tool, I usually start a little high in Z and comp the tool down until I get the chamfer I want.

[rchoward]

sometimes i want my chamfer to be dead on the first time

 

the 2d chamfer featur in contour is what i use the size that come out are dead on iff the tool is defined correctly (u also get a good verify)

 

chamfer tools almost always have flats on them... i use solid carbide 90deg spot drills so i can chamfer and spot drill/countersink in the same tool change i find the fastest u can turn the tool and .005/tooth breaks the edge nice

 

finally the tool set up secret THIS IS THE SECRET TO DETERMINE THE FLAT SIZE

 

put the tool in question in the mill z it out on a piece of alum drill a hole so a conic section is there. Note the z depth u went

 

Put a ball bearing of known size in the conic section and note the difference between the top of the sphere and the surface of the plate.

 

take this info to your drawing package and with a little bit of creativity u voila the flat size, put that in mastercam an run your first off with complete confidence... record the number and use the same tools and u will alwys be set up

 

this works for a wide variety of tools... draft mills come to mind... good luck

[Nominal]

Thanks to everyone for their input, alot of decent suggestions. Perhaps I wasn't very clear on the how or the why of my method. What I'm trying to do ( and do everyday with success ) is establish a point on the tool which is the point I'm driving against my geometry. This reference point on my chamfer mills is the intersection of the angle and the outside dia of the tool. I typically create some geometry of my chamfers which is offset just slightly ie. (.02"). This way the edge of the tool is not trying to coincide with the edge of the part, but is actually overlapping by being .02 beyond and .02 above the suface in the case of a 45 deg. This takes care of any irregularities in the part surface etc. When setting chamfer tools, people can put it on a comparator ( shadow graph for you old timers )and see what the offset is from the end of the tool to the intersection of the angle and od. This way when they "touch off" they know how much to adjust the tool length by. For thier diameter compensation, it would be done to the outside diameter like any other milling cutter. The result is that the same point on the tool to which both compensations are being done is the same point on the tool that I drove in mastercam. When I have preset tooling that is set with an electronic toolsetter, I give a diameter target on the conical, to which the length value is to be measured. Either way the chamfers come out as close to perfect as the person setting the tool. Also it helps to have the chamfers actually drawn on the part rather than just compensating using the 2d chamfer as someone suggested, that way I don't forget to do them. :-) The whole point of my post was to get a sense of how other people were doing this in mastercam, since the graphic verify doesn't work for me doing it the way I do. Sounds like everyone is doing this in a variety of different ways. Thanks again.

[Mike-T]

I've done it several ways myself, But am very happy with the 2d chamfer that MC has come out

with, It saves me alot of time. I too have used

90 Deg spot drills, but only in softer materials.

Theres not unuf clearance on them for the harder

Materials.

[heeler]

We us a insert ball mill and do it as a surface. This has always produced the desired results the first time. We are generally doing 1-5 parts at a time. You can run a very high spindle speed and feed rate this way. You can also do many other things with the same tool.

 

HTH

 

Glenn