[COPO427]

Hi guys I would like to break the edge of my part with a chamfer tool in my HAAS minimill.

When I select 2D chamfer Mastercam cuts the chamfer but it looks heavy. If I set a "0" z depth it automatically puts it -.2 on the Z. Much too deep. How do I correct this? I must not be setting something right?

Thanks

[HuFlungDung]

What shape is your tool? I do not know Mastercam, but there could be a typical problem with setting the Z offset to the end of a truncated cone. Since you cannot touch off the non-existent point, you might still have to allow for the depth of the non-existent portion of the cone.

You might have to fiddle with your tool description (correct it) or else reinterpret the manner in which you set the length offset for this type of tool.

[COPO427]

What shape is your tool? I do not know Mastercam, but there could be a typical problem with setting the Z offset to the end of a truncated cone. Since you cannot touch off the non-existent point, you might still have to allow for the depth of the non-existent portion of the cone.

You might have to fiddle with your tool description (correct it) or else reinterpret the manner in which you set the length offset for this type of tool.

Thanks for the reply. The shape is 1/2" round chamfer tool with a 45 deg angle When I set the Z depth to "0" in parameters page Mastercam post process's a Z depth of -.200

I set the Z to +.180 in parameters page to get a -.020 Z depth of cut. Weird.

I guess I will have to modify it each time I want to use it.

[psychomill]

Must be something to do with your geometry. Are you programming on a 2D wire? or 3D? For example, this will post out a different Z then what you set:

If the Z level of your feature is below 0 (say @ -.200), and on your tool parameter page, you tell it to cut at 0 incremental. It will then post out a cut at Z-.200.

There are other variations too. 3D geometry can also "alter" what you think you might be cutting at if the tool/cut parameters aren't set correctly.

[Matt Berube]

Hi guys I would like to break the edge of my part with a chamfer tool in my HAAS minimill.

When I select 2D chamfer Mastercam cuts the chamfer but it looks heavy. If I set a "0" z depth it automatically puts it -.2 on the Z. Much too deep. How do I correct this? I must not be setting something right?

Thanks

Have you played around with the numbers in the chamfer dialog ?

I suspect the tip offset is responsible for the confusion...

See picture...

[rickyt]

+1000 to matt, look there.

[psychomill]

Good call Matt.....

I don't ever use the chamfer dialog and didn't think of it...

[Derek Goodwin]

You can check your tool point also. Mastercam defaults to a tool with a flat on the bottom. Edit the tool to a point if that is the type you are using

[bennett71]

I would do what Matt sugested then run a backplot in the side view. Here you will get an idea of how deep the tool will cut.

[bennett71]

I would do what Matt sugested then run a backplot in the side view. Here you will get an idea of how deep the tool will cut.

[Dugg]

I've had some difficulties with chamfer tools in that I now input .062" for the tool tip and the same .062 for the tool diameter. I use tool comp with lead in and lead out, set the Z at -.035 and then use changes in the Z and D to get the edge I'm looking for. I'm sure there's an easier way, but I plod alone with what I know hoping to learn more.

[Matt Berube]

I've had some difficulties with chamfer tools in that I now input .062" for the tool tip and the same .062 for the tool diameter. I use tool comp with lead in and lead out, set the Z at -.035 and then use changes in the Z and D to get the edge I'm looking for. I'm sure there's an easier way, but I plod alone with what I know hoping to learn more.

There is an easier way...

I define my tool exactly as it measures. I set the chamfer dialog exactly as the work piece requires. I get a chamfer that is exactly right. There is no smoke and mirrors involved with this feature.

What difficulty have you had ?

[tobyaxis]

I've had some difficulties with chamfer tools in that I now input .062" for the tool tip and the same .062 for the tool diameter. I use tool comp with lead in and lead out, set the Z at -.035 and then use changes in the Z and D to get the edge I'm looking for. I'm sure there's an easier way, but I plod alone with what I know hoping to learn more.

Matts Method is a great way to achieve what you want. You can also go to the Manufactures website and get the specs on your tooling to help you. This way there is no constant running back and forth to the shop floor to measure tools that your going to use. All is good in the world of "WWW".

BTW: Keep using Cutter Comp so adjustments can be made for tool wear.

[Matt Berube]

constant running back and forth to the shop floor

Well all you have to do is save it to your tool library. I am WAY too lazy to actually run back and forth...

[tobyaxis]

Well all you have to do is save it to your tool library. I am WAY too lazy to actually run back and forth...

I don't know who buys what lately but you have to realize that most Shops today don't always buy from the same company all the time. If you take a simple 90 Degree HSS Spot Drill and compare it to 3 different name brands you will get 3 different tip geometries that vary from .005 to .015 (Tool Tip Flat). When using it for a thread Lead or to put a Chamfer on a Profile the cutting size will be different. That is why I also prefer to use Cutter Comp when profiling. Check the Geometry of a 82 degree counter sink. Consistancey these days is terrible.

This is also why I suggest that when someone touches a tool off (90 Degree Spot Drills) to add .02 to the Z offset for tools 1/8-5/16 and .03 for anything higher up to Half inch.

Usually someone can scrap one part, but what if they only have one part? Parts get rejected for stupid stuff these days as well.

LOL. "What do you mean my Chamfer is a half of a degree Off ? " "What do you think the function of a Chamfer is anyway ?"

The other day I heard someone ranting that their part was rejected because their radius was .001 Oversized using a 1/16th Form Tool. Go Figure, tool was made in a different Country.

BTW: I still don't trust CMM's.:rainfro: