Doosan DNM200/5ax only commissioned with 4+1 and 3+2.. Need PP ASAP(or how to alter one)

[rjd_cnc_programmer]

I am working on a small Doosan 5 axis trunion machining center. It was bought sight unseen from an auction house and the current owner had no idea the 5 axis simultaneous was in fact turned off. Guess whose problem it is right now? Yep...it's mine. I tried the standard 3 axis/5 axis post from the Fusion library. It works great for 3 and 3+2. But 4+1? Nope!! So if anyone has a post that will work for this, I'll dance at your wedding or whatever floats your boat for sure. Otherwise I am going to be trying a bunch of different stuff to complete this job I am working on. Thanks to all who contribute...

[a.laasW8M6T]

when you say 4+1, is it only the C axis that can rotate simultaneously? and the A axis is just for positioning?

does the machine support tilted work planes(G68.2)?

and TCP (G43.4?)

You should be able to get this to work with that Doosan 3/5 axis post and a machine configuration.

but it could just be a simple change to the post.

[rjd_cnc_programmer]

The machine doesn't support the G43.4...I have to have inverse time feed
G93 also. I have no idea why the previous owner ordered it like this. The
program that I have that runs has the G68.2 for position only. Yes the A
locks and C spins.

[a.laasW8M6T]

Ok

I think I have a solution, but I need to spend a little more time on it to make sure its safe, I'm still at work so will look at it later on

[CNC_Lee]

@rjd_cnc_programmer 

 You will need to get a custom post processor written if the generic posts are not providing the required output for your machine. I offer post processor development services and happy to work out a solution for your machine! Message me if still needing assistance. 

[a.laasW8M6T · Accepted solution]

If you go into the post processor and search for TCP, you will find a line that says var useTCP = true.

Change that to false and it will now output non tcp code using g93.

The only issue will be you have to program your parts from center of rotation of the A/C axes in fusion, ie the WCS needs to be set there, so it will be somewhere below the part in space.

if the c axis  centerline is offset in Y from the A axis centerline this needs to be compensated out with an offset in the postprocessor.(or in a machine configuration, which is my preferred method).

If your not comfortable doing these post edits, it is wise to reach out to a reseller like Lee, because with 5 axis stuff without TCP it can be tricky to set up and it really is worth spending a little money instead of messing around trying to get it to work yourself.

[rjd_cnc_programmer]

Hey.... I appreciate it. I can do the edits and I know the old fashioned way on the center lines. I used to do head porting on a Fadal 6030 for Warren Johnson. Using Camplete Port. It was the same as this. I will change that tomorrow morning and let you know how it went. Thanks again.

[rjd_cnc_programmer]

worked like a champ....thank you