C-axis (4th axis) vertical to spindle on a mill/cnc router - how to configure?

[fusion1BXBB2]

Hello,

i will soon need to do some work on a 4th axis, but the 4th axis will be fixed vertical or face to face to the spindle, something like a vertical lathe. I will use a 80:1 harmonic drive for that job. I need to do drilling operation, where i want to rotate the 4th axis to position for drilling operation. (for example, one hole each 45 degree)

Also, i want to do milling operations where i want only use the X Z and C axis, without the Y axis. This will be as the most accurate way to do what i want to do, same for the drilling operations.

I cannot use wrap function, because of the wrong tool orientation, which works only for horizotal positioned 4th axis, so the standard way.

As i understand correctly i should use "Turning or millturn" as operation type in the setup up, but then the XYZ axis are used for the operation.

I made some research and found out that i need to change something in the post process, but i am not good in such things, so i hope you can help me out with that.

I am using Linuxcnc for my diy CNC Router.  I have attached the Postprocessor file of my cnc router.

Thanks in advance.

[a.laasW8M6T]

Hi

You don't need to select turn/millturn for your setup, just a normal milling setup will be fine.

What you want to do requires "Polar Mode", which is available in most of the millturn posts, but also in the Standard haas post.

You could try that one and just turn on Has C axis

Then you put a manual NC before each operation that is "USEPOLARMODE"

The tool will be positioned in the +X direction at Y0 and the C axis will rotate to drill the holes.

Can be used for milling toolpaths too.

Try the Haas post out and see if that works for you.

[fusion1BXBB2]

Thank you very much for that.

I just did exactly that (besides that, that i did not choose a machine e.g. like Mazak in your screenshot) and when i save the post process from the operation and check the code i see that the c axis is turning.

But, i opened the file in a nc simulator and it seems to drill a hole, then the drill stays at the z-position on the bottom of the hole and the c-axis turns without going out of the hole, so the drill would brake.

I am not sure if i have something wrong set up, but i uploaded the .nc file i created.

Also, in the Fusion operation simulation i see that the Y axis is moving. Do i understand correctly, that its not possible to simulate the rotary movement in Fusion?

EDIT: I tested milling, with multiple depth and this seems to work and i can see in the nc simulator that the C axis is moving and also the multiple depth movement is there. For the drilling operation it seems that i need to change something to drill the hole, move out of the hole, change c-axis position and drill next hole.

[a.laasW8M6T]

Hi

to answer your questions

But, i opened the file in a nc simulator and it seems to drill a hole, then the drill stays at the z-position on the bottom of the hole and the c-axis turns without going out of the hole, so the drill would brake.

I am not sure if i have something wrong set up, but i uploaded the .nc file i created.

It seems the NC simulator doesn't simulate the G81 cycle correctly, have you drilled on your machine using this cycle before, it should actually work just fine, but to be safe you could run the code up above the job just to check

Also, in the Fusion operation simulation i see that the Y axis is moving. Do i understand correctly, that its not possible to simulate the rotary movement in Fusion?

In normal simulation Fusion isn't using the posted code to simulate, and in this case the Postprocessor is doing the conversion into polarmode so it won't simulate correctly.

If you create a machine for machine simulation with and XYZ and C axis and use that to simulate then it will correctly show the rotation.

[fusion1BXBB2]

Thank you for the information. I will try out the drlling operation at the end of this week, due to the fact that i am waiting to get my harmonic drive for the 4th axis. I understand that it does not simulate the rotary movement of the stock material, but i am wondering why it does not show the drill going up to the safety height after drilling one hole, but maybe it is like that. I will try it out as soon as my 4th axis is working.

Okay, then i will maybe design a small machine and see how the simulation looks exactly in fusion with the rotary axis.

Thank you for your help.

[programming2C78B]

NC Viewer does not simulate canned drill cycles. It will stay at the Z- and just go point to point-  this is a tool to view gcode, not a simulation of it.

[fusion1BXBB2]

Thanks for the info.

I forgot to reply - but in meantime i found out that its not simulating visibly as it should - as you mentioned, but i connected the A axis motor, tested a postprocessor and it seems to work.

Currently i am building the 4th axis and maybe on tomorrow i can do first machining tests, then i will know if everything works. I want to test the A axis and C axis.