Chamfer mill in a C Axis lathe and wrap a Radius.

[crazy^millman]

Okay I got a new one I have never had to do before. I have a part that has a slot cut through it. It has a Radius tuned on the end of the part and the chamfer of the slot wraps from the OD along the Radius to the face and I need to cut a constant chamfer from the OD to the Face while following that radius. The OD chamfer to the slot was easy I just milled that when I face milled the slot in a C Axis motion. The face and face face chamfer was easy with a double angle tool. The tricky one is cutting this chamfer along the Radius with a chamfer cutter. At the Face I have 45 Deg Angle and at the Diameter to edge of slot I have 45 degree, but getting this tool to sweep along that and maintain the correct 45 degree angle while doing that in a C axis motion I am thinking not possible.

I could 5 Axis or surface machine this all day long, but take a chamfer tool and have it create a chamfer from the face of a part to the OD of a part while following a radius is a new one. I typed this thinking okay someone is going to go sure thing I do that all the time and I will be thankful to you that have, but I think I am going to have to tell the customer to throw a ball endmill in their machine and just surface machine it. Now thew question will be do they have one more live tool.

Here is a sample for those that want to get an idea what I am trying to do.

MODEL CHAMFER RADIUS

 

 

[huskermcdoogle]

You could mange that with a back chamfer tool and undercut it couldn't  you?  

[crazy^millman]

17 minutes ago, huskermcdoogle said:

You could mange that with a back chamfer tool and undercut it couldn't  you?  

Come in normal to the face and cut that with the chamfer tool. I just figured out how to do it with a 3/8 ball endmill in one pass cutting both. Will not be a perfect chamfer, but close enough to make the customer happy.

Here is the example for those who have never done a rib cut to make a chamfer before.

MODEL CHAMFER RADIUS

[jlw™]

Am I misunderstanding what you want?

Is this it:

https://www.dropbox.com/s/oug4zq8dbw5ttdr/CHAMFER TO RADIUS.mcam?dl=0

 

[crazy^millman]

16 hours ago, jlw™ said:

Am I misunderstanding what you want?

Is this it:

https://www.dropbox.com/s/oug4zq8dbw5ttdr/CHAMFER TO RADIUS.mcam?dl=0

 

Yes this is not on a 5 axis machine this is on a C axis Turn/Mill machine where the tool will be fixed parallel to the Z axis or center line of the machine.  Take that chamfer tool and cut just the radius on the face.

[Jayson Kramer]

17 hours ago, 5th Axis CGI said:

Come in normal to the face and cut that with the chamfer tool. I just figured out how to do it with a 3/8 ball endmill in one pass cutting both. Will not be a perfect chamfer, but close enough to make the customer happy.

Here is the example for those who have never done a rib cut to make a chamfer before.

MODEL CHAMFER RADIUS

Without pulling the part. Did you do a flow with rib cut?

[crazy^millman]

1 minute ago, Jayson Kramer-CNC Software said:

Without pulling the part. Did you do a flow with rib cut?

Yes.

[jlw™]

3 hours ago, 5th Axis CGI said:

Yes this is not on a 5 axis machine this is on a C axis Turn/Mill machine where the tool will be fixed parallel to the Z axis or center line of the machine.  Take that chamfer tool and cut just the radius on the face.

I see, boy that sucks.  Not happening with a 90deg chamfer tool, imo.  I mean, there is no question you can drive the toolpath but the geometry just isn't suited for the cut.  They are probably pushing for cycle time and limited on tooling available in a turret as well.

[crazy^millman]

On 12/22/2018 at 2:05 PM, jlw™ said:

I see, boy that sucks.  Not happening with a 90deg chamfer tool, imo.  I mean, there is no question you can drive the toolpath but the geometry just isn't suited for the cut.  They are probably pushing for cycle time and limited on tooling available in a turret as well.

Exactly the dilemma the only saving aspect is a 2 turret 2 spindle machine so it does help. Chamfered many parts using a ball endmill so this one will be no different.

[mkd]

hope this isn't too much of a captain-obvious comment:

what about a 45° woodruff to contour 90% of the chamfer (one cut @ C0 and another @c180) followed by a little flowline 3D work, on the face, to finish the full radius in between?

[crazy^millman]

1 minute ago, mkd said:

hope this isn't too much of a captain-obvious comment:

what about a 45° woodruff to contour 90% of the chamfer (one cut @ C0 and another @c180) followed by a little flowline 3D work, on the face, to finish the full radius in between?

I am trying to reduce the run time. I cut the chamfer on the OD when I cut the slots so no need to worry about having to use a chamfer tool on the chamfer that is on the OD. On the face and radius I am going to use a ball endmill as one of the methods I submit with the programming package. The requirement is break all edges not that is has to be perfect chamfer. The difference on the real part is .0007 from a perfect chamfer to the edge of the radius of the ball endmill. I think we will be okay, but I will give the customer a couple choices of toolpaths to choose from that can decided which one make them happy. 

[mkd]

Cycle time will be (might be) quicker with a woodruff being it will only need one tool call. Feed rates may also be faster due to more flutes of a woodruff.

tool life and tweaking the program to work with a woodruff could be a bigger issue, compared to a little carbide chamfer tool.

_ just playing devil's advocate.

[crazy^millman]

34 minutes ago, mkd said:

Cycle time will be (might be) quicker with a woodruff being it will only need one tool call. Feed rates may also be faster due to more flutes of a woodruff.

tool life and tweaking the program to work with a woodruff could be a bigger issue, compared to a little carbide chamfer tool.

_ just playing devil's advocate.

Thanks and why I throw these things out here. I can't see it all and being on the island most of the time talking to Wilson it is nice to have a sounding board.

[mkd]

Meant to say Dovetail, dang it, dovetail!

[JoshC]

since you cant cut it like JLW showed in his video I think that I would use a Ball endmill since its not an extremely large chamfer and would prorably only require a few passes with a ball endmill anyways. I would not use a chamfer mill since it wont look correct in that area where the chamfer transitions from the face of the part to the OD so i would use a ball endmill to 3d/surface mill the chamfer. Sure it will be more passes than a chamfer mill but at least you can get very accurate results around where that radii transitions from the Face to the Od of that part. that is my opinion on this one and I would just use like a flowline with a Right side plane and tool axis control page set to C-axis. Or just cut everything possible with a chamfer mill and only use the ball endmill on that one specific area where the chamfer transitions from the face of the part to the od.