Rotate C axis for chamfer on circle

[Metallic]

This may be a dumb question but forgive me.

Lets say I want to mill or chamfer a circle, but instead of interpolating X and Y coordinates, I want X and Y to remain fixed, while instead the C axis rotates to produce the cut.

What is an appropriate 5 axis toolpath to use if I have a trunnion style table? Or is it a manual coding thing?

Thanks in advance

[crazy^millman]

Check out 2019 is has this built into it as a toolpath.

It can be done and have to assume you don't have enough travel in one of the axis to machine it with X and Y and want to spin the table to machine it? Questions are many, but can it be done with a 2D Chamfer or does it need to be a 3D chamfer? Got a sample file so someone can wrap their brain around the hole and the shape and see what your seeing. Sorry, but I have programmed a lot different 5 Axis CNC Machines and seeing a picture of what you trying to do or a model would be very helpful.

Yes you can do this and if you can hand code it I can do it with Mastercam.

[K2csq7]

Multiaxis curve. 

The circle you are using for Cut pattern geo must be on center (X0, Y0).

Tool axis control = line (just use one line)

Ensure you check the box for "Relative to direction".

Tighten up the cut tolerance until the X's and Y's vanish from your posted code. 

 

[Metallic]

16 hours ago, C^Millman said:

Check out 2019 is has this built into it as a toolpath.

It can be done and have to assume you don't have enough travel in one of the axis to machine it with X and Y and want to spin the table to machine it? Questions are many, but can it be done with a 2D Chamfer or does it need to be a 3D chamfer? Got a sample file so someone can wrap their brain around the hole and the shape and see what your seeing. Sorry, but I have programmed a lot different 5 Axis CNC Machines and seeing a picture of what you trying to do or a model would be very helpful.

Yes you can do this and if you can hand code it I can do it with Mastercam.

 

Its merely for experimenting with axis controls and getting my head around different methods of controlling each of the 5 axes on my new mill, so its just a cylinder on the center line of the C axis rotary.

 

Thanks for the heads up on the Public Beta, I am currently migrating my files over and will take a look.

If not ill do what K2 suggested.

Thanks for pointing me in the right direction, will update if I can figure it out.

[jlw™]

16 hours ago, C^Millman said:

Check out 2019 is has this built into it as a toolpath.

It can be done and have to assume you don't have enough travel in one of the axis to machine it with X and Y and want to spin the table to machine it? Questions are many, but can it be done with a 2D Chamfer or does it need to be a 3D chamfer? Got a sample file so someone can wrap their brain around the hole and the shape and see what your seeing. Sorry, but I have programmed a lot different 5 Axis CNC Machines and seeing a picture of what you trying to do or a model would be very helpful.

Yes you can do this and if you can hand code it I can do it with Mastercam.

Ron, am I missing this path in 2019?  What path in 2019 give the option to rotate the table in a mill definition?

[Aaron Eberhard]

I would use 2d Contour, myself. 

Contour your circle in the picture above, then, on the Axis Control > Rotary Axis Control, set the thing to 3 Axis with Rotary Axis set to Rotate About Z Axis.  

If you look at the NCI, you'll see that the 1002 line is now set to 13 in the 17th position, which stands for "Polar conversion, rotate about Z"

 

Now, you might not be able to post it, depending on how your post interprets it, but that's how I'd try first.

 

Otherwise, the problem is when we generate a vector inside of a toolpath, there's two ways to get there.  You can either move X & C and keep the Y stationary, or you can you can move X & Y and keep C stationary.   By default, most posts will choose the linear motion as that's traditionally been faster and preferred.   If you talk to your post vendor, they should be able to give you a specific switch mode that will ask it to choose rotary instead.

[crazy^millman]

1 hour ago, jlw™ said:

Ron, am I missing this path in 2019?  What path in 2019 give the option to rotate the table in a mill definition?

Aaron has a Video up that had this defined check it out on the Official Forum. The post should be able to take that new process and give us what was laid out here. I agree with Aaron I would just use a 2D process for the above part, but the new stuff looks very promising. Don't tell anyone I talked about 2019 stuff they might kick me out of Beta oh that's right it is Public Beta so I am covered.

[Metallic]

1 hour ago, C^Millman said:

Aaron has a Video up that had this defined check it out on the Official Forum. The post should be able to take that new process and give us what was laid out here. I agree with Aaron I would just use a 2D process for the above part, but the new stuff looks very promising. Don't tell anyone I talked about 2019 stuff they might kick me out of Beta oh that's right it is Public Beta so I am covered.

Luckily for me I messed up my Control File and for some reason it wont work on 2018 anymore ; )

 

It claims it saved a backup file version of it but it clearly did no such thing.

Am I screwed or is there a way to get it back? I guess im this far in moving to '19 so I may just finish the process and deal with it.

 

I am pretty sure my post wont output the correct code I want, so I would need to talk to the developer to add a rotary switch to it if I feel like it.

[Leon82]

you could swarf it.

Ive experimented with the the axis substitution it worked, but it was ugly and only for 1 fixture with a generic post I played with

[jlw™]

If you have a lathe def it's easy peasy.  I wish the c axis face contour was available for mill.  Having said that, contour with axis sub works great for me.

[John Llacza]

? Te sirve así