5 Axis, Table BC, NO-TCP, milling post/machine setup

[dpm-lic01]

Hi, i am currently trying to create a post processor for 2 machines i have here, they are both very similar. 3 axis code runs fine without changes to the default fanuc post, but i havent even tryed 5 axis on the machines, one look at the G Code and i know it will not work. I created a machine, using machine builder, when i test the axis in cam everything is fine, limits, pivot point positions, axis directions, everything. I want the ability to simulate with machine, so i havent even tryed to override the kinematics inside the post.

I have made some small changes to the post, it reacts to 5 axis, it tilts the table, but the coordinates generated (X,Y,Z) will not mill in the correct position.

I dont know if i am doing this the right way, with the software i used before (and still do, because i cant get the post to work in fusion), the machine is defined in relation to the machine zero point. After the cam is ready, i place the parts in the machine, find their midpoint, and save to G54. I then take a picture of the offset values in G54, and when i press generate G-Code, a pop up window apears asking me to fill in the offset values, i fill them in(from the picture i took), and the g-code is generated. I usually make big series of equal parts, and i make sure they are placed in the same exact point every time with custom fixtures attached to the table, if i need to relocate them in the machine, or rebuild the fixtures, i need to get the part offset again and generate new g code. I tryed doing it the same way in fusion.

I will attach a picture of the machine(from CAM), in a pdf file that contains images with of my machine setup.

For now, i can see that when the rotary axis move, XY and Z, coordinates in g code will mill very far from the part, sometimes in unreachable coordinates. 

I described how i did thing in another program, just to let you know how i tryed to do it in Fusion, doesnt mean it has to work exactly how i described. Let me know how you do it. I couldnt find any good tutorial on this. 

Any help would be greatly apreciated.

Thanks

Miguel Carreira

[KrupalVala]

HI @dpm-lic01 ,

I'm interested in understanding how you define the work offset for Three Axis.

In the machine builder, the attachment point for parts should ideally align with where the part is going to be loaded on the machine table. The center of the table typically serves as the ideal position for this purpose. For machines without TCP, the workflow typically follows the process outlined in the attached screenshot. In this scenario, there are two options available:

1. Users can define the machine origin to pivot distance, which will automatically zero the offset value in machine kinematics. Users then need to create a Work Coordinate System (WCS) at this pivot distance.
2. Alternatively, as depicted in the screenshot, one can define the origin at the table center and automatically calculate the pivot distance in offset. This allows users to define the WCS at the table center, same as the machine origin.

   Non-TCP 5-axis table-table machines

   • Measure the Pivot distance:
   
   • In the machine configuration window, go to the settings for the rotary TCP and turn it off.

   Define the pivot distance in the Z direction. If the pivot distance is above the part attachment point (table top) give it a positive value; otherwise, give it a negative value:

   
   
   
   • Define the origin (WCS) at the table top center.
   • In the post-processor define optimizeMachineAngles2 or optimizeType as "OPTIMIZE_AXIS".

However, in your case, where the machine origin position differs and there's no option to define the machine origin directly, one approach could be to create a part attachment point at the table center and define the WCS at the machine origin. However I'm not entirely certain. Also can you check with method Two : What would happen if you go with Option Two were we define the WCS at the Machine Origin/Table Center?

Thanks,

[dpm-lic01 · Accepted solution]

Hi,

---

@KrupalVala wrote:

HI @dpm-lic01 ,

I'm interested in understanding how you define the work offset for Three Axis.

---

I am not exactly sure what you want to understand, english is not my native language, so i will just give you the long explanation...

That depends on the part, i have some fixtures that resemble a vise, others are built to hold the stock in the center (aligned with the pivot point). If it is a vise, the part can be anywhere, so i find the part center with an edge finder for XY, and a known length tool to get Z, save the result to a work offset (G54 to G59) and i make sure that offset is activated in the program before the milling starts, if it is centered, i do the exact same thing, it is just a little less work, because i dont realy need the edge finder, i just look at my notes and fill in the values for X and Y manually, if it is centered, then the center is the pivot point, and i know where it is.

As for the CAM i dont really need to worry about it, when there is no kinematic calculations involved, i just  place the WCS in the part (at the same location i will try to find with the edge finder) and generate milling strategies, part placement inside the machine (in CAM) becomes irrelevant, unless i want to simulate, witch i never do for 3 axis strategies, but if i want to, i just comy the values from the machine's work offset, and place the part in CAM in the same position(in relation to the Machine Origin), because the values i get from the offsets table are in relation to Machine Origin i have to do the same in cam, if i want to use those values.

That is actually why i tryed to do things this way. If my table attach point in CAM is the machine origin, then i can just copy the work offset values i get from the machine and paste them in the part position of my CAM setup, and the part snaps into position.

I'm done for today, tomorrow i will get back to this, an i will try the solution you proposed.

Thank You @KrupalVala

Miguel Carreira