Has anyone used an Adjustable Angled Driven Tool holder with Fusion 360?

[MetalDawg]

I have a Doosan lathe. A Lynx 2100 LSYB, and I am thinking about purchasing a 0-180° Adjustable Angle Driven BMT holder to mill the angled flats on this part instead of moving it to another machine for a second operation. The problem is, how do you program this? I have a 5th axis machine, so I know about tool orientation, but won't the program just fail to output it as it will assume I need a B axis in my lathe? I thought about programing it as a non-angled flat, thinking that it will just machine it as an angle since the cutter will be at an angle anyway. Still, since I will need to make several WOC passes or do an adaptive strategy, each pass will need to be higher than the last. Has anyone used an adjustable angled holder in a lathe programed with Fusion 360? If so how did you do it?  Thank you.

[Anonymous]

Program it using tool orientation and post with Doosan post set to MX, B axis should be called to angle you set in tool orientation in Fusion, you later delete all B axis code from program because tool will be set to fixed angle. 

You'll have to touch front edge of tool for Z and bottom edge for X axis then shift tool in both axis so that center point of tool is in reference to origin on part.

I haven't done this before but it seems to me it should work without any issues.

[MetalDawg]

VicKosta, I will try that once I get the tool holder. This project is about a month away, but I didn't want to wait until the last minute to figure it out. I called the manufacturer and spoke with an applications guy, and he suggested touching off on the edge in Z and then use paper to touch off on the angled part in X.

Since my machine is a BMT45, the angled tool holder only comes in an ER16 size. If I can find an ER20 from another manufacturer, I can use a half-inch endmill and then just slot it since it is a shallow cut.

Thank You,

Darryl

[Anonymous]

When you touch tool for radial or axial orientation, you are setting center point and face of the tool to origin of the part. 

Same is true when tool is tilted at 45 degrees, this would be no issue on Dusan MX because tool gets tilted (B axis move)  when called to action.

If tool was touched on Doosan MX, perpendicular to Z axis, machine control would account for X and Z shift at 45 degree tilt before approaching work piece.

In your case, you will set geometry offsets including that shift because tool is fixed in tilted position.

In order to set tool center point and face to origin on part, you have to touch point A on part face for Z axis then offset  number in Z minus for value depending on tool diameter so that tool center is on part face or origin.

For X axis, you touch point B on part OD and measure that position at the control, then offset in X minus direction by two times the value required for toll center point to be at origin of the part, diameter programming assumed.

When tool is set correctly, it will make accurate cut as programmed, be sure to account for adequate lead in and out clearance because of tilt.

In Fusion, use "in computer" compensation for roughing and "wear" for finishing.