topic Re: Lathe Tool Orientation in Parting Operation ? (Multitasking Machine) in Fusion Manufacture Forum

Lathe Tool Orientation in Parting Operation ? (Multitasking Machine)

bac244 — Fri, 03 Jan 2020 14:45:42 GMT

Does Fusion send the tool orientation to the Post Processor when using the "Turning Part" operation? My testing shows no. I told fusion I had a straight external parting tool, and told it I had a 90 degree oriented Face Grooving tool and either way outputs B=0. Seems like turning tool orientation only is sent to the post if the toolpath has the "Tool Orientation" section. (IE grooving, parting don't send this data, is always 0)

Some background: I'm using a heavily modified Doosan Fanuc 31 Mill/Turn (I probably have 40 hours into coding and testing) post to run on my Hitachi Seiki CH 250 Super Hicell. To overcome this problem I added logic: if operation is parting, B = 90 because I will always be parting off at B90. With the B axis at any other orientation, the sub spindle will crash into the turret. I have a good work-around and I'm happy with it, just thought I would ask because it seems more logical that the CAM would have control over B orientation, not the post.

Re: Lathe Tool Orientation in Parting Operation ? (Multitasking Machine)

johnswetz1982 — Fri, 03 Jan 2020 18:46:49 GMT

So is it a parting tool or face grooving tool?

Re: Lathe Tool Orientation in Parting Operation ? (Multitasking Machine)

akash.kamoolkar — Fri, 03 Jan 2020 20:10:42 GMT

@bac244

When a tool is oriented in the library the software assumes that this is how the tool is already oriented on the machine and no additional commands will need to be passed in the NC code. The tool orientation parameter in the operation is what passes dynamic orientation commands to the NC code. Unfortunately parting seems to be a special operation where we didn't envision someone dynamically orienting a tool before the operation and therefore does not have an orientation field.

Regards,

Akash Kamoolkar

Re: Lathe Tool Orientation in Parting Operation ? (Multitasking Machine)

bac244 — Fri, 03 Jan 2020 20:24:18 GMT

Akash,

Thank you. That's what I thought was going on. My Post Processor mod works and didn't seem to mess anything else up. Cutting right now!

In answer to the other question, it is a straight shank parting tool I was just trying to fool the post processor into outputting a B90. orientation command for the parting operation. In another operation where I am doing face-grooving, I have a straight tool in a 90 degree holder so I had to tell Fusion it was a facegrooving tool and it output the correct B angle. Telling it I had a straight tool at 90 degrees wouldn't make any code (orientation not supported). Tricky tricky

Re: Lathe Tool Orientation in Parting Operation ? (Multitasking Machine)

bob.schultz — Fri, 03 Jan 2020 20:50:48 GMT

There are actually two methods for controlling the B-axis orientation from within Fusion for a lathe. The first as you noticed is the Tool Orientation field in certain turning operations. The second is using the Orientation in Turret field in the Setup tab of the tool definition.

Selecting a Face Grooving tool and an orientation of 90 should give you the same results as if you were able to define the Tool Orientation in the operation.

Re: Lathe Tool Orientation in Parting Operation ? (Multitasking Machine)

bac244 — Sun, 05 Jan 2020 17:40:27 GMT

Bob,

Indeed this gave the same behavior in the posted code but looked closer to reality in the Fusion simulation.

Thank you!

Re: Lathe Tool Orientation in Parting Operation ? (Multitasking Machine)

ptNYQCR — Tue, 30 May 2023 06:48:54 GMT

Have you got a post processor that works for the Hitachi Ch250?

Im new to fusion and also to Hitachi CH250.

Would you share the post ?

Peter

Re: Lathe Tool Orientation in Parting Operation ? (Multitasking Machine)

bac244 — Tue, 30 May 2023 12:56:13 GMT

Hi Peter,

Responded to your DM just now. I have a partially baked post for Hitachi CH250 I am willing to share with anyone. I have since sold both of my HiCells so I stopped working on the post processor at some point where there are still mistakes and errors and usability issues. I'm sure it also has developed new problems with F360 updates I am not keeping up with.

I also have worked up 2 post processors for Mori Seiki NT/NTX series machines (I have NT4200). One for the upper and one for the lower that work together to make 2 programs (1 for upper and 1 for lower). So they support 2 channel machining using Fusion 360. Not like pinch turning but there is support to "park" the opposite channel while the one does work and vice-versa or have both doing operations on different spindles.