Selecting a post-processor

[vaishnavinambiarr]

I have a 5-axis machine, with XYZ on the head and conventional B and C axes on the bed. However, the CNC machine responds to A and B commands, so I've been replacing the "B"s in the code with "A"s and "C"s in the code with "B".

Additionally, the head is cutting at a position slightly off in the XY plane.

Is there a way to pick a post-processor that would give me the right code?

[KrupalVala · Accepted solution]

Hi @vaishnavinambiarr ,

You can find the correct post processor for your machine from here.

Please read the following article to configure your machine kinematics in the post processor.

• How to set up a 4/5 axis machine configuration - Autodesk Community - HSM

For more detail, Please go through the post processor manual guide.

• Post Processor Manual

Thanks,

[vaishnavinambiarr]

Hi, thank you for your reply! About

• How to set up a 4/5 axis machine configuration - Autodesk Community - HSM ,

How do I open the code of the post-processor as shown in Step1? Which app should I install?

[vaishnavinambiarr]

 @KrupalVala 

The first step of editing the post-processor is to change the "false" to "true", but the code for this post-processor is quite different. Could you please guide me as to how I should proceed?

[vaishnavinambiarr]

Hi, thank you for your reply! 

For a FANUC post that I used, the process worked just fine and it is now giving A,B outputs as required!

However, the head is still cutting at a position slightly off in the XY plane.

[KrupalVala]

HI @vaishnavinambiarr ,

You can use Visual Studio Code or any editor tool for post edit.

Can you please tell which controller is in your machine? is it Mach or Fanuc or Else? Sorry but I'm confused. 

If it Mach then, Mach3Mill is 4 axis configured post that's why codes are different.

You can test with 5AXISMAKER post. It's Generic 5-axis post for 5AXISMAKER with Mach3 control. It should work fine in your machine.

Thanks,

[vaishnavinambiarr]

@KrupalVala I am unsure about the controller, as the CNC is not name-brand.

5AxisMaker does not work for it, it gives out a very scattered toolpath, and the head tries to move out of its range even though the part is quite small.

The edited FANUC post works fine in terms of the toolpath, it's only the positioning of the head and table that does not seem to match. 

I believe the code is generated correctly (toolpath generated in Mach3Mill seems accurate) and the zeroing in has been done perfectly(verified position), the head is cutting at a position slightly off in terms of X, Y coordinates with respect to the position of the part on the table. 

What could be the problem?

[KrupalVala]

HI @vaishnavinambiarr ,

Please send me your Machine and Controller picture.

Thanks,

[vaishnavinambiarr]

@KrupalVala I have PMed you the pictures, thanks

[vaishnavinambiarr]

@KrupalVala 

[KrupalVala]

Hi @vaishnavinambiarr ,

You can use Mach3Mill post processor And add following codes in your post processor.

function onOpen() {
  if (getProperty("useRadius")) {
    maximumCircularSweep = toRad(90); // avoid potential center calculation errors for CNC
  }
//update the logic from here to..

  if (true) {
    var bAxis = createAxis({coordinate:1, table:true, axis:[0, 1, 0], offset:[0, 0, 0], range:[-180.00, 180.00]});
    var cAxis = createAxis({coordinate:2, table:true, axis:[0, 0, 1], range:[-360.00, 360.00], cyclic:false});

    machineConfiguration = new MachineConfiguration(bAxis, cAxis);

    setMachineConfiguration(machineConfiguration);
    optimizeMachineAngles2(1); // map tip mode - we compensate below
  }
//here

  if (!machineConfiguration.isMachineCoordinate(0)) {
    aOutput.disable();
  }

Please Add the offset value of the rotary axis in offset[0, 0, 0]. 

What if offset ? : Defines the rotational position of the axis in the format of a coordinate, i.e. [0, 0, 0]. For machines that support TCP the offset parameter can be omitted. The offset values for tables are based on the part origin defined in the Setup. The offset value for the rider or primary rotary head is based on the distance from the tool stop (or spindle face) position to the pivot point of the rotary head. The offset value for the carrier rotary head (when the machine has a head/head configuration) is based on the pivot point of the rider axis to the pivot point of the carrier axis. The default is [0, 0, 0].

You can set the workplane at top of you chuck or resting face of the Job.  

Thanks,

[vaishnavinambiarr]

@KrupalVala 

Hey, thank you for the reply!

I made the changes and the G-code is getting exported now with all 5 axes' codes. However, the toolpath is very random. I have attached a snip of it. Please let me know what you think of it.

[KrupalVala]

Hi @vaishnavinambiarr ,

Please share your Fusion project.

Thanks 

[vaishnavinambiarr]

@KrupalVala 

Hi, I've attached my project, and the post I edited below:

[KrupalVala]

HI @vaishnavinambiarr ,

Could you please dry run the toolpath on your machine? The code looks good to me. It should work fine.

Thanks,

[vaishnavinambiarr]

Hi, @KrupalVala 

I tried a dry run, but the head is still moving in a different location with respect to the bed.

At some points the Z coordinates for the head are much below the part location as well

The tool has not been inserted and the spindle is not attached to its power supply. The CNC was zero-ed in at the + on the bridge-like structure with the screws.

I have attached a picture of the dry run in progress.

[KrupalVala]

HI @vaishnavinambiarr ,

Do you have your Controller or programming manual? 

Thanks,

[vaishnavinambiarr]

@KrupalVala 

No, the CNC didn't come with any manual/ instructions except that I can use Mach3 Mill with it. 

[KrupalVala · Accepted solution]

HI @vaishnavinambiarr ,

You have Two options make it work.

1st solution: Permanent  

Set the pivot distance in the post processor as I mentioned in my previous post. set the value in offset [0,0,0]

From Chuck top to center of the B axis rotation.

2nd: Temporary

Create workplane and shift it to Pivot distance and generate the output from the shifted workplane.

I hope this helps.

Thanks,

[vaishnavinambiarr]

Hi @KrupalVala ,

This worked, thank you so much! I really appreciate the help and patience!!😊