5 axis drilling

[iamcdn79]

In the attached project I created a bunch of 3+2 drilling toolpaths but apparently, Toolpaths #38 and 40 are 5 axis toolpaths according to my postprocessor. For toolpath #38 this caused the tool to go to the wrong position.

The way to solve this problem was to make it invalid and recalculate, this changed it to a 3+2 toolpath and went to the correct position.

Now my question is how can I see in Powermill that this is a 5 axis toolpath or a 3+2? Both toolpaths have tool axis set to vertical and the machine axis control set to Fixed orientation.

And how does a toolpath become a 3+2 toolpath from a 5 axis toolpath simply by making it invalid and recalculating?

[Anonymous]

I can not open the project, because I use powermill 2019.
In the Postprocessor, on the tab Option file settings - canned cycles, there is a switch "Treat vertical drilling as " with options: 3 axis, 5 axis or 3 + 2 axis.

Therefore, in my opinion, it’s all about the postprocessor settings, and you don’t have to look at anything at Powermill (with properly configured postprocessor).

[iamcdn79]

It was set as 3+2, see attached pic. I also attached the 2019 version.

[cfastNJWK6]

The only way I know of to tell if powermill is seeing something as 3-axis, 3+2, or live 5, is to make an NC Program.  The symbols in the upper left hand corner of the NC Program settings form signify how powermill "sees" the program.  If there is no symbol it is 3-axis. The attached picture explains 3+2 and live-5.

[Jonathan_Artiss19]

Hey All

The compass symbol doesn't mean that the toolpath is live 5, it's meant to show that orientation vectors are turned on. 

@iamcdn79  was the check box for "Use orientation vectors calculated during simulation" turned on during the calculation?

[cfastNJWK6]

Here is a toolpath calculated with orientation vectors turned on and the symbol doesn't appear in the NC Program:

[Jonathan_Artiss19]

Hey @cfastNJWK6 

The Proposed Orientation needs to be set some something other than "free". Fixed direction is most common. 

[cfastNJWK6]

Here is a picture of a toolpath calculated with orientation vectors turned off and the symbol does appear:

[Jonathan_Artiss19]

[cfastNJWK6]

My apologies,

I thought you were simply saying that the symbol appears when the tick box "Use Orientation vectors calculated during simulation" is turned on.

We recently had an issue with a post that was flagging toolpaths as live-5 when this symbol would be on an NC Program.

[Jonathan_Artiss19]

No need for apologies, we are all here to help one another. 

Sorry for hijacking your thread @iamcdn79  😉

[iamcdn79]

---

@Jonathan_Artiss19 wrote:

Hey All

The compass symbol doesn't mean that the toolpath is live 5, it's meant to show that orientation vectors are turned on. 

@iamcdn79  was the check box for "Use orientation vectors calculated during simulation" turned on during the calculation?

---

Yes it was turned on

[Jonathan_Artiss19]

I've just ran into another issue where this setting triggers a different callout in the post. Can you try without this checked and see if it makes a difference? 

[iamcdn79]

Turning it off and recalculating achieved the same result as leaving it on and recalculating

[jake.montgomery]

Hello,

We are having a similar issue with the "Use orientation vectors calculated during simulation" option. What we found was recalculating the toolpath reset the OV's to it initial state. If you post it without running simulation or NC Program verification it will treat it as 3+2.  When you simulate or verify the NC Program the OV's are modified to match the simulation, thus triggering it to be 5x rather than 3+2. This was only happening if the simulation made changes to the OV's. 

[Anonymous]

With the option “Use orientation vectors calculated during simulation” is turned on, after simulation, the Axis mode and the Toolpath axis mode in the postprocessor become "Polar" instead of "3-axis". Thus, if there is a need to use this option, the postprocessor settings for the "Polar" axis mode is required.