Unwanted Y Values With Rotary Tool Paths Denford 4th Axis Post

[smunzer8ZZFW]

I am currently using a Denford MRC 40 with a rotary axis setup the x or a axis. I have been working to find or edit a post that will work for this machine but have ran into a road block I can not seem to figure out. when posting my rotary tool path the code produced moves the bit along the y axis away form eh work piece instead of keeping it above the rotary axis. it seems the post is trying to mill the part using both 4th axis and 3 axis machining. I will attach a snip of the gcode produces below as well as the post and test file. https://a360.co/40cTvNC 

[serge.quiblier · Accepted solution]

Hello @smunzer8ZZFW 

you have made a mistake in the kinematic definition of the axis, and the kinematic settings.

A 4th axis machine is rarely supporting TCP. But your config may activate it.

That's why the Y axis is moving.

Your current config is:

  if(true) {
    var aAxis = createAxis({coordinate:0, table:true, axis:[1, 0, 0], range:[0,360], cyclic:true, preference:0}); // <<< ADD 'cyclic:true'
    machineConfiguration = new MachineConfiguration(aAxis);
    setMachineConfiguration(machineConfiguration);
    optimizeMachineAngles2(0);
  }

For deactivating tcp, change the code to that one:

  if(true) {
    var aAxis = createAxis({coordinate:0, table:true, axis:[1, 0, 0], range:[0,360], cyclic:true, preference:0, tcp:false}); // changed
    machineConfiguration = new MachineConfiguration(aAxis);
    setMachineConfiguration(machineConfiguration);
    optimizeMachineAngles2(OPTIMIZE_TABLES);  // changed
  }

We are defining the rotary axis as not supporting tcp, and calculating angle and coordinates for a NON TCP Table machine kinematic.

Regards

______________________________________________________________

If my post answers your question, please click the "Accept Solution" button. This helps everyone find answers more quickly!

[smunzer8ZZFW]

@serge.quiblier This has worked flawlessly for removing the unwarned y values. another question that has come up is the rotary tool path I have set up is supposed to do a path along the rotary axis then rotate a degree or two then cut the next line. however the machine seems to be cutting the line tool path at random degrees around the workpiece these tool paths will not line up to create the spiral I am looking for. I will attach photos of what it is actually milling 

[serge.quiblier]

Have you set your toolpath correctly?

The differents toolpaths are switched by this parameter

The spiral variant seen from the part side:

The linear variant

And then the circular passes

Regards.

______________________________________________________________

If my post answers your question, please click the "Accept Solution" button. This helps everyone find answers more quickly!

[smunzer8ZZFW]

Yes the model you see cut above was done with the line variant. The entire code ran through that part and that is what came out. It’s almost like the machine was skipping lines. 

[serge.quiblier]

Hi,

Can  you share the gcode file generated.

That way, we can try to back plot it, in order to detect the issue.

I don't think the post have "forgotten" some lines.

But something else, like positive and negative values for the rotary axis may not be dealt correctly, depending on the controller and it's settings.

Regards.

[smunzer8ZZFW]

Sure thing,

[serge.quiblier · Accepted solution]

Hello @smunzer8ZZFW 

Backplotting your code using HSMEdit is giving the following result:

Passes every 5 degree approximately:

Nothing in the coordinates is "traversing" the part.

The side view of the part

An Isometric view

A solid rendering, several flaws, the stock is defined in HSMEdit as a rectangular part. (cylinder is only along Z)

So some cutting "collision" shown in red.

Poor angular increment, a smaller value would be needed for a finer finish.

The solid rendering from HSM Edit:

The only strange move is the first rotation when going from 0 to 359. The machine may do a full revolution around the part. (at least hsmedit is showing that)

[smunzer8ZZFW]

Okay so this must be an issue with the machine controller because that is not at all what the part looks like when machining. the machine doesn't move in normal rotational values instead seems to move some arbitrary rotation value and the just decide to start eh toolpath there. also sometimes it doesn't move the tool out of the part and start rotating cutting a channel in the part itself. its almost like the controller cant process the code coming at it and skips lines of code then picks back up where it wants too. 

[serge.quiblier]

Hi @smunzer8ZZFW 

I don't know what is the controller.

But in the g-code I have noticed one or two unusual things.

If G1 is never alone, being alongside X, Y Z or A coordinates, G0 is always alone on a line.

Is it usual for this controller?

Some machines sometime require all axis coordinates, to be defined on the line, i.e. X Y Z A must always be output.

Can it be the issue on the machine?

Regards.

______________________________________________________________

If my post answers your question, please click the "Accept Solution" button. This helps everyone find answers more quickly!

[smunzer8ZZFW]

I don't think this controller needs those coordinates because it still moves it just moves erratically. the problem i was having before and the creation of this forum is that the values it was inputting where pulling the tool off the axis of rotation. so the kinematic value of y needed to be changed in the post processor. this controller is very old and so is the machine it may be time to look into upgrading it with a  centroid controller.