4 axis tombstone toolpath links

[Anonymous]

I have a tombstone fixture on a 4 axis machine. I face one side of the part with a face mill and then face mill the opposite side, when I simulate it, the tool collides with the part. I  have messed with the settings in toolpath connections but cannot find one that will avoid the collision. Ideally, the Z-axis retracts and the spindle doesn't move when the table rotates, but the issue is too many axes moving simultaneously.

https://www.reddit.com/r/Autodesk/comments/cqnm9a/ive_messed_with_all_the_settings_i_can_think_of/?s...

[Michaelangelo631]

I encounter this all the time.  Since my post processor is setup to do a full "Z" retract in between toolpaths I am able to work around this.  If I need to see a clean verification inside of powermill then my workaround is to insert "workplanes" between the toopaths in the NC program and then run the simulation by choosing to verify the whole nc program and not just the individual toopaths.  Take a look at this prior article on the forum.  This post is what got me over the hump when I first ran into this issue.

https://forums.autodesk.com/t5/powermill-forum/issue-with-collision-between-axis-toolpath-changes/td...

Regards,

Mike

[Anonymous]

Thanks for your comment.

I saw this post before, and adding these workplanes helped a little but there were still collisions unless I added 2 workplanes (safe move in z, then another for the safe rotation) but this just clutters the sidebar with the extra workplanes, which still isn't a true representation of the program.

I have now realized that the post-processor includes a return to home position line at the end of each toolpath. I think it is a shame this isn't included in the simulation.

[Michaelangelo631]

I agree with you 100% on it being cumbersome to add the workplanes.  I often have to add 2 or 3 in between toolpaths when I am trying to get to the other side of a workpiece.  Also when I post out the program these moves are not really happening in the posted G-code (although I could have my post modified to include them). I just have to rely on experience that the posted file has the "Z" retract moves built in.  I would definitely raise my hand to vote for this retract feature to somehow be incorporated into the simulation for the NC program.  Would save allot of extra work.

Regards,

Mike

[Anonymous]

https://forums.autodesk.com/t5/powermill-forum/issue-with-collision-between-axis-toolpath-changes/m-...

From what you described here, I created a sketchy macro for connecting four-axis toolpaths in the simulation

[Anonymous]

Thanks

I haven't touched macros in powermill yet so I might need some advice on bringing that into my project and using it.

[Anonymous]

So I got the macro in, but I get this error message. I can't comply with the error message I don't think as I have to have Z facing in the Z direction.

[Anonymous]

The macro queries the NC program coordinate system, the B-axis coordinate system ('RotaryAxis'), and requests two toolpaths (A,B) to connect. Then create connect pattern, and toolpath from pattern. Finally create a NC program with tooolpath A, connect pattern, toolpath B.

The macro does not work when a toolpath uses the Global workplane. RotaryAxis Z-axis must be in same direction with ncprogram and toolpaths coordinate systems Y-axis.

[Anonymous]

Sorry for the ambiguity, but for convenience, I use the "RotaryAxis" Z axis, in the macro, the layout in the picture corresponds to your Y axis. The "RotaryAxis"  X,Y directions indifferent, X0 and Y0 at  the table center.

[Anonymous]

In the meantime, I've made a model of the configuration, so hopefully my idea is clear.

[Anonymous]

Thanks this has been a big help in learning powermill, but when this macro created path is in the NC program, the simulate from start option is grey'ed out.

[Anonymous]

The "connect" toolpath is calculated? The  Wireframe Swarf  Finishing startegy  require minimum Premium license.

Please upload your project, if possible then PM 2017 or older version. (We have stayed with the PM2017, and we are planning a transition to PM2020 the next month.)

[Anonymous]

Another workaround for this problem:
The SimuNc.mac does not simulate NC programs, but the toolpaths contained within them, so the result of joining movements is not visible. The SimuNC-Hermle.mac is the same as the previous one, just a simple example of how to manipulate a machine model. The example limits the movement of the 'A-axis' to a negative range. Before running this macros, you must turn on ViewMill and set the desired mode.

FUNCTION Main () {
// Simulate selected ncprograms
   IF $widget('ViewmillBar.VMOnOff').Value == 'FALSE' {
      MESSAGE INFO 'Please turn Viewmill on, and prepare'
      RETURN
   }
   ENTITY LIST NcProgs=INPUT ENTITY MULTIPLE NCPROGRAM 'Please select Nc programs'
   EDIT PAR 'SimulationState.Issues.Collisions.CheckCollisions' 1
   EDIT PAR 'SimulationState.Issues.Collisions.Clearance' "10"
   EDIT PAR 'SimulationState.Issues.Collisions.CheckToolAndHolder' 1
   EDIT PAR 'SimulationState.Issues.Collisions.HolderClearance' "1"
   EDIT PAR 'SimulationState.Issues.Collisions.ShankClearance' ".05"
   EDIT PAR 'SimulationState.Issues.CheckReconfigurations' 1
   EDIT PAR 'Powermill.Simulation.Issues.PlaybackSetting' 'never'
   SIMULATE ISSUES CLEAR

   STRING Messages=''
   DEACTIVATE TOOL
   FOREACH Nc IN $NcProgs {
      FOREACH item in components($Nc) {
         IF lcase($item.RootType) == 'nctoolpath' {
            ENTITY TP=entity('toolpath',$item.Name)
            IF (NOT $TP.Computed) OR (SEGMENTS($TP)==0) {
               $Messages=$Messages+'Not computed/empty toolpath: '+$Nc.name+' '+$Tp.Name+crlf
            } ELSE {
               SIMULATE TOOLPATH $item.Name
               SIMULATE PLAY               
            }
         }
      }      
   }
   IF $Messages != '' {
      MESSAGE INFO $Messages
   }
   FORM MACHINEISSUES
}